Library Explorer and Part Developer Tutorial

Transcription

Library Explorer and Part Developer
Tutorial
Product Version 14.2
January 2002
 1999-2002 Cadence Design Systems, Inc. All rights reserved.
Printed in the United States of America.
Cadence Design Systems, Inc., 555 River Oaks Parkway, San Jose, CA 95134, USA
Trademarks: Trademarks and service marks of Cadence Design Systems, Inc. (Cadence) contained in this
document are attributed to Cadence with the appropriate symbol. For queries regarding Cadence’s trademarks,
contact the corporate legal department at the address shown above or call 1-800-862-4522.
All other trademarks are the property of their respective holders.
Restricted Print Permission: This publication is protected by copyright and any unauthorized use of this
publication may violate copyright, trademark, and other laws. Except as specified in this permission statement,
this publication may not be copied, reproduced, modified, published, uploaded, posted, transmitted, or
distributed in any way, without prior written permission from Cadence. This statement grants you permission to
print one (1) hard copy of this publication subject to the following conditions:
1. The publication may be used solely for personal, informational, and noncommercial purposes;
2. The publication may not be modified in any way;
3. Any copy of the publication or portion thereof must include all original copyright, trademark, and other
proprietary notices and this permission statement; and
4. Cadence reserves the right to revoke this authorization at any time, and any such use shall be
discontinued immediately upon written notice from Cadence.
Disclaimer: Information in this publication is subject to change without notice and does not represent a
commitment on the part of Cadence. The information contained herein is the proprietary and confidential
information of Cadence or its licensors, and is supplied subject to, and may be used only by Cadence’s customer
in accordance with, a written agreement between Cadence and its customer. Except as may be explicitly set
forth in such agreement, Cadence does not make, and expressly disclaims, any representations or warranties
as to the completeness, accuracy or usefulness of the information contained in this document. Cadence does
not warrant that use of such information will not infringe any third party rights, nor does Cadence assume any
liability for damages or costs of any kind that may result from use of such information.
Restricted Rights: Use, duplication, or disclosure by the Government is subject to restrictions as set forth in
FAR52.227-14 and DFAR252.227-7013 et seq. or its successor.
Contents
1
Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 13
Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Audience Profile . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Pre-requisites . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Using the Samples . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Chapter Summaries . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
13
14
14
15
15
2
Library Basics . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 17
Objective . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Library Concepts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Physical Organization of Libraries . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Lib-Cell-View Architecture . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Views . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Category (.cat) Files . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Summary . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
17
17
18
18
19
19
24
24
3
Working with a Library Project . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 27
Objective . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Types of Projects . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Library Management Use Model . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
As a Librarian . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
As a Designer . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Library Project Concepts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Using Library Explorer . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
January 2002
3
27
27
28
28
29
30
31
31
Creating a Library Project . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Task Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Steps: . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Creating Libraries in the Build Area . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Task Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Steps . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Viewing by Categories . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Task Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Steps . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Copying Parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Task Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Steps . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Viewing Footprints . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Task Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Steps . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Verifying Parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Overview of Types of Verifications . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Task Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Steps . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Deleting Parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Task Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Steps . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Summary . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
32
32
32
39
39
39
39
39
40
41
41
41
42
42
42
43
43
45
46
46
46
46
47
4
Creating Parts With Pins Split Across Symbols . . . . . . . . . . . . . . . 49
Objective . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Part Creation Methodology . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Creating a Part . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Task Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Starting Part Developer . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Setting up Part Developer . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Task Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Steps . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
January 2002
4
49
49
50
50
51
52
52
52
Entering Part Properties . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Task Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Steps . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Entering Logical Pins . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Task Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Steps . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Intermediate Saving of Parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Continuing Pin Entry . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Creating Packages . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Task Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Steps . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Creating Split Symbols . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Task Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Steps . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Saving Parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Task Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Steps . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Verifying Parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Task Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
View Verification Check . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Instantiation and Packaging . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Steps . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Viewing the Part in Concept HDL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Task Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Steps . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Exporting Parts to the Reference Area . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Task Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Steps . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Summary . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
61
61
61
62
62
63
64
65
66
66
66
72
72
73
75
75
76
76
76
76
77
78
81
81
81
83
83
83
85
5
Modifying a Split Part. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 86
Objective . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 86
Importing a Part . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 86
Task Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 86
January 2002
5
Steps . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 87
Setting Up Part Developer . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 87
Task Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 87
Steps . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 88
Opening an Existing Part . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 88
Task Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 88
Steps . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 88
Modifying Pins List . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 89
Task Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 89
Steps . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 89
Modifying Packages . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 90
Task Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 90
Steps . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 90
Modifying Symbols . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 94
Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 94
Task Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 95
Steps . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 95
Viewing the Bits of a Vector Pin . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 101
Task Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 101
Steps . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 101
Summary . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 102
6
Creating a Multi-Section Symmetrical Part . . . . . . . . . . . . . . . . . . . 104
Objective . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Starting Part Developer . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Task Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Steps . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Setting Up the Part Developer . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Task Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Steps . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Entering Part Properties and Logical Pins Information . . . . . . . . . . . . . . . . . . . . . . . . .
Task Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Steps . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
January 2002
6
104
104
105
105
105
106
106
106
107
107
107
Intermediate Saving of Parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Creating Packages . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Task Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Steps . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Creating Multiple Packages . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Task Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Steps . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Creating Symbols . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Task Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Steps . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Copying Symbols . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Task Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Steps . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Creating HAS_FIXED_SIZE Symbols . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Task Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Steps . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Summary . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
7
Modifying Multi-Section Symmetrical Parts
. . . . . . . . . . . . . . . . . . 130
Objective . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Importing a Part . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Launching Part Developer . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Setting Up the Part Developer . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Task Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Steps . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Modifying Pin List . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Task Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Steps . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Deleting Packages . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Task Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Steps . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Deleting Symbols . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Task Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Steps . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
January 2002
7
110
110
110
111
119
119
119
122
122
122
128
128
128
128
128
128
129
130
130
131
131
131
131
132
132
133
134
134
134
134
134
134
Modifying Packages . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Task Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Steps . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Modifying Symbols . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Task Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Steps . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Summary . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
135
135
135
137
137
137
139
8
Creating Asymmetrical Parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 140
Objective . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Entering Part Properties . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Configuring Pin Name Interpretation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Task Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Steps . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Entering Logical Pins . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Task Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Creating Packages . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Task Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Creating Multiple Packages . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Task Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Steps . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Creating Symbols . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Task Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Saving Parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Task Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Steps . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Verifying Parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Task Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Steps: . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
January 2002
8
140
140
143
144
144
144
146
146
149
149
155
155
155
157
157
161
161
162
162
162
162
Alternate Method of Creating an Asymmetrical Part . . . . . . . . . . . . . . . . . . . . . . . . . . . 162
Summary . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 163
9
Modifying Asymmetrical Parts
. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 164
Objective . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Importing a Part . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Setting up Part Developer . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Task Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Steps . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Opening the Part . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Task Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Steps . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Modifying Logical Pin List . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Task Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Steps . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Modifying Packages . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Task Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Steps . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Updating Symbols . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Task Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Steps . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Saving Modified Part . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Task Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Steps . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Adding Symbol Pin Properties . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Task Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Steps . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Changing Symbol Pin Properties . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Task Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Steps . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
January 2002
9
164
164
164
165
168
168
169
169
169
169
169
169
170
170
170
174
174
174
177
177
178
179
179
179
182
182
182
Summary
. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 185
10
Handling Pin Texts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 186
Objectives . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Methodology . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Adding Libraries to a Library Project . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Task Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Steps . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Working with Unassociated Pin Texts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Task Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Steps . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Task Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Steps . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Summary . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
186
186
187
187
187
187
189
189
192
193
195
11
Data-Managed Projects . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 196
Objective . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Overview of Data-Managed Project . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Pre-requisites for Creating a DM Project . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Creating a Data-Managed Project . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Task Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Steps . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Summary . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
196
196
196
199
201
201
201
213
12
Using XML to Create Parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 214
Objective . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Importing Part Data from an XML Datasheet . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Task Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Steps . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Symbol Interpretation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
January 2002
10
214
214
214
214
217
Summary
. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 218
13
Creating Templates . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 219
Objective . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Creating and Applying a Part Template . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Task Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Steps . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Using Part Template to Create Parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Verifying Parts Against Templates . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Property Checks . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Pin Load Checks . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Symbol Checks . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Task Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Steps . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Summary . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
219
219
220
220
221
221
223
223
224
224
224
226
226
227
14
Extracting Templates . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 229
Objective . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Extracting Templates . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Task Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Steps . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Modifying Template Values . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Task Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Steps . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
January 2002
11
229
229
231
231
233
233
233
233
Summary
. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 234
15
Creating VHDL Wrappers and Map Files . . . . . . . . . . . . . . . . . . . . . 235
Objective . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Creating a VHDL Wrapper/Map File . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Task Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Steps . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Summary . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
235
235
238
238
238
243
16
Creating Verilog Wrappers and Map Files . . . . . . . . . . . . . . . . . . . . 245
Objective . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Creating a Verilog Wrapper/Map File . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Task Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Steps . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Summary . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
245
245
245
245
246
249
Index.............................................................................................................................. 251
January 2002
12
1
Introduction
Overview
In the 14.0 release, Cadence has introduced two new tool suites:
■
PCB Librarian
The PCB Librarian tool suite contains the following tools:
■
❑
Library Explorer
❑
Part Developer
❑
Allegro Librarian
PCB Librarian Expert
The PCB Librarian Expert tool suite contains the following tools:
❑
Library Explorer Expert
❑
Part Developer Expert
❑
Concept HDL
❑
Checkplus HDL
❑
CAE Views
❑
EDIF Schematic, symbol, and netlist reader/writer
❑
Verilog Model Library
❑
Allegro PCB (includes Allegro Librarian)
❑
General bi-directional mechanical interface (ver14)
❑
IDF bi-directional mechanical interface (version 2 and 3)
❑
IGES bi-directional electrical translator (level 5)
January 2002
13
Introduction
❑
PADS dB-in translator (version 4, 6 and PowerPCB version 3)
❑
PCAD dB-in translator (version 8)
❑
Zuken-Redac Cadstar dB-in translator (Cadstar 7.6 and Maxi)
This tutorial demonstrates the major features of the Library Explorer and Part Developer
tools. Using the Library Explorer and Part Developer, you can create and manage libraries
and parts in an easy and effective manner. You can create several different type of parts such
as asymmetrical parts and large pin count parts.
In addition, if you have the Library Explorer Expert and Part Developer Expert, you can
maintain versions of libraries and parts. You can also create parts from XML datasheets and
create and implement templates for creating parts.
Audience Profile
The intended audience profile for this tutorial are people who maintain and modify digital
libraries for design entry.
Pre-requisites
The tutorial assumes the familiarity with the following products:
■
Project Manager
■
Concept HDL
■
Allegro
How to Use this Tutorial
This tutorial provides a hands-on-exercise on creating libraries and parts. To gain the most
from this tutorial, you should try out all the steps as documented in the tutorial. The tutorial is
based on data provided through datasheets in PDF and XML format. The tutorial has 16
chapters. The first 9 chapters cover the features which are common to both standard and
expert versions of the Library Explorer and Part Developer tools. The chapters 10 to 16
contain the features that are exclusive to the expert version of the Library Explorer and Part
Developer tool.
January 2002
14
Introduction
Using the Samples
The tutorial works with the samples which are installed along with the software. The samples
are stored in the following location <your_install_dir>/share/fet/examples/
pcblibex. The name of the file is pl_db.zip for Windows NT platform and pl_db.t.Z
for UNIX platforms. You need to extract the samples from the compressed file.
When you extract the sample files, it will create the tutorial_project_data directory.
This directory has the following subdirectories that are required for the successful completion
of the tutorial.
Directory
Contents
datasheets
Contains the datasheets for the parts that you will be creating while
completing the tutorial
footprints
Contains the Allegro footprints
lcx
Contains the lcx library that will be used as a reference library
old_parts
Contains the parts created in older versions of Part Developer
test
Contains a sample library project named test.cpm
lsttl
Contains the ls00 and ls01 parts of the lsttl library. It also contains the
category file for the lsttl library
Chapter Summaries
The tutorial is divided into 16 chapters. Each of these chapters detail the steps involved in
creating the different types of parts. Although the steps are similar, each of these chapters
cover some of the unique features of Part Developer. Therefore, you should go through the
tutorial completely to benefit from the powerful Library Explorer and Part Developer tools.
Following is a brief summary of the chapters in the tutorial:
Chapter 2, “Library Basics,”, covers the physical organization of a part library. This chapter
also covers the different views of a part.
Chapter 3, “Working with a Library Project,” describes the types of projects, the library
management use models and the library development methodology. You also learn how to
create a library project and work in it.
January 2002
15
Introduction
Chapter 4, “Creating Parts With Pins Split Across Symbols,” details the methodology and
steps involved in creating a part with pins split across symbols. This chapter also details the
method to verify parts and importing them to the reference area.
Chapter 5, “Modifying a Split Part,” covers the steps involved in modifying a part which has
pins split across symbols.
Chapter 6, “Creating a Multi-Section Symmetrical Part,” describes the methodology and
steps involved in creating a multi-section symmetrical part.
Chapter 7, “Modifying Multi-Section Symmetrical Parts,” details the methodology and steps
involved in modifying a multi-section symmetrical part.
Chapter 8, “Creating Asymmetrical Parts,” covers the methodology and steps involved in
creating asymmetrical parts.
Chapter 9, “Modifying Asymmetrical Parts,” describes the steps involved in modifying an
asymmetrical part.
Chapter 10, “Handling Pin Texts,” details the methodology followed by Part Developer to
handle pin texts for a part.
Chapter 11, “Data-Managed Projects,” describes the methodology and steps involved in
creating and working with data-managed projects.
Chapter 12, “Using XML to Create Parts,” details the steps involved in creating parts from
XML datasheets.
Chapter 13, “Creating Templates,” covers the steps in creating part templates. This chapter
also covers the steps involved in using the templates to create parts.
Chapter 14, “Extracting Templates,” describes the steps in extracting template information
from a part. This chapter also details the steps involved in modifying the extracted templates.
Chapter 15, “Creating VHDL Wrappers and Map Files,” details the steps involved in creating
and verifying a VHDL wrapper and map file.
Chapter 16, “Creating Verilog Wrappers and Map Files,” details the steps involved in creating
and verifying a Verilog wrapper and map file.
January 2002
16
2
Library Basics
Objective
In this chapter, you will:
■
Understand the physical organization of a library
■
Understand the different views of a part
Overview
Libraries are a collection of parts. To enable you to understand the library storage and its
organization, a sample lsttl library containing the ls00 and ls01 parts are provided. This
sample library is stored in the tutorial_project_data location.
January 2002
17
Library Basics
Library Concepts
Physical Organization of Libraries
Each library is a directory and each part of a library is a directory. The part directories are
stored under the library directory. For example, the library lsttl is stored in a directory
called lsttl. The part ls00 and ls01 are subdirectories in the lsttl directory.
Information about a part, such as packaging and graphical information, are stored in different
views. A view is nothing else, but a directory under the part. Each part can have many views
like chips, entity, sym_1 etc. The information about a view is stored in one or more files
under the view directory. For example, the chips view (the chips directory under the part)
contains the chips.prt file. This file has the information about the physical packages
associated with the part.
Note: You can see the set of Cadence-supplied libraries in <your_install_dir>/
share/library.
The following section describes the views in more detail.
January 2002
18
Library Basics
Lib-Cell-View Architecture
Views
Symbol (sym) View
The sym_1 and the sym_2 directories represent the symbol view of the part. The symbol
view is the graphical representation of a part in a Concept-HDL drawing. Each part can have
one or more symbol views that are in effect different graphical representations.
January 2002
19
Library Basics
Figure 2-1 Examples of Symbol Views
lsttl
ls00
sym_1
master.tag
symbol.css
sym_2
master.tag
symbol.css
Different symbol views are stored under directories named sym_1, sym_2 and so on. The
actual information about each symbol is stored in the symbol.css file stored within the
sym_n subdirectories.
Package (chips) View
The package view or the chip view stores the package information, such as pin names, pin
numbers, footprints and electrical information, for a part. This view connects the logical view
of a component to its physical view.
Pin information, such as pin names, types, loading and physical numbers, is stored in the
chips.prt file located in the chips subdirectory. To see the contents chips.prt file of
the ls00 part, open it through any text editor such as notepad or vi.
Displayed below is a partial screen shot of the chips.prt file for the ls00 component.
January 2002
20
Library Basics
Figure 2-2 The ls00 chips.prt file
The chips.prt file is divided into primitives where each primitive represents the
information for a specific package such as DIP, SOIC etc. The primitive is itself divided into a
pin and a body section.
January 2002
21
Library Basics
The pin section defines the logical to physical pin mapping. It also contains information on pin
names, pin types, pin loading values and physical pin numbers. The low asserted pins are
suffixed with either a ‘*’ , ‘_N’ or a ‘-’ sign.
Of special interest is the PIN_NUMBER property which is present for each logical pin of a
part. The general syntax is
PIN_NUMBER = (pin number,pin number,.....,pin number)
The number of comma separated entries describes the number of slots in a part. If the logical
pin has a corresponding physical pin for the slot, it is filled with the physical pin number.
Otherwise, the pin number is substituted with the value 0.
For ls00, A, B and Y are the logical pins. By looking at the PIN_NUMBER entry, you can
identify that the part has four slots. Also, since all the logical pins are present across all the
slots, the PIN_NUMBER entry for each logical pin has a physical pin in all the four slots.
The body section of the chips.prt file contains the power pins information as well as the
properties that are associated with a package, such as JEDEC_TYPE etc. These properties
are necessary and are used during different stages of the PCB Design front-to-back flow.
More information about properties is available in PCB Systems Properties Reference.
For more information on the chips.prt file, see Concept-HDL Libraries Reference.
Entity View
The entity view is stored in the entity subdirectory. This view contains a Verilog module and
a VHDL entity declaration. Both of them describe the list of ports found on the part. This view
is used when you create Verilog and VHDL wrapper and map files for simulation. For more
information about simulation views, see the Concept-HDL Libraries Reference.
Part_Table View
The Part_Table view stores the Physical Parts Table (.ptf) file. The Physical Parts Table (.ptf)
file stores the packaging properties for a part in the library. This file contains information about
parts such as package types, manufacturers, part numbers and any custom properties.
January 2002
22
Library Basics
For example, displayed below is a typical entry from a .ptf file.
FILE_TYPE = MULTI_PHYS_TABLE;
PART ‘74LVT574’
CLASS = IC
:PACK_TYPE = Part_NUMBER | JEDEC_TYPE | DESCRIPTION;
DIP = CDS123 | DIP20_3 | FLIP_FLOP
SOIC = CDS456 | SOIC20 | FLIP-FLOP
LCC = CDS789 | LCC20 | FLIP-FLOP
END_PART
END.
In the above part table file, the following things are of importance:
■
A unique part number is assigned based on package style.
■
An Allegro package symbol name is assigned based on package style.
Note: The JEDEC_TYPE property may also be defined in the chips.prt file. However, the
part_table view has the priority.
■
A part description is added
The PACK_TYPE property is a key property (it is on the left hand side of the equal sign). This
implies that every 74LVT574 in the schematic must have the PACK_TYPE property assigned.
However, if an 74LVT574 is found that does not have a PACK_TYPE property value of either
DIP, SOIC or LCC, the Packager-XL will abort. To set a default PACK_TYPE value, use the
OPT statement as follows:
:PACK_TYPE (OPT = ‘LCC’) = PART_NUMBER | JEDEC_TYPE | DESCRIPTION;
When a 74LVT574 part in the schematic fits the key property description (has a PACK_TYPE
property value of either DIP, SOIC or LCC), then the injected properties (they are all on the
right side of the equal sign) are added to the packager netlist files (specifically the
pstchip.dat file).
Each cell in a library containing logical parts should have a corresponding .ptf file. You can
place all the files in a single directory which will later be read by Packager-XL during
packaging. You should maintain packaging information such as Allegro footprint
(JEDEC_TYPE), VALUE, TOLERANCE, and PWR_RATING in this file.
January 2002
23
Library Basics
Simulation View
When a symbol view is saved to the disk, an entity view is automatically created. In the entity
view is a Verilog and VHDL file that contains the names of all the pins on the symbol (known
as a module). The simulation view maps the symbol (or module) to a simulation model. The
name of the module is mapped to the name of the simulation model. The pin names in the
module are mapped to the port names in the simulation model. The file in this view contains
only mapping data. The actual model is stored in an HDL model library (for example,
veriloglib).
During simulation, the Verilog or VHDL file in the schematic view is used as the netlist. Each
part in this netlist has an entity and a simulation view.
Verilog-XL replaces the parts in the netlist with the simulation models as defined by the
wrapper or a map file.
Depending upon whether a Verilog or a VHDL based flow is used, and whether map files or
wrappers are used, it is suggested that the following directories store the simulation views:
■
vlog_map stores the map file that is used by Verilog during simulation
■
vlog_model stores the wrapper file that is used by Verilog during simulation
■
vhdl_map stores the map files that is used by VHDL during simulation
■
vhdl_model stores the wrapper file that is used by VHDL during simulation
Note: Unlike other views, simulation views can have user-defined directory names. However,
it is suggested that you use the names mentioned above to ensure consistency and uniformity
of understanding.
Category (.cat) Files
In addition to the supported views, you can also create a category file (.cat) within each
library, to organize the parts into functional groups, such as BUFFER, CLOCKDISTRIBUTION and so on. The category files are located within each library. This is an
optional file. The file is named as library_name.cat such as lsttl.cat for the lsttl
library.
Summary
In this chapter, you learned about the physical organization of a part library. You also learned
about the different views of a part. In the next chapter, you will learn how to create and work
with a library project.
January 2002
24
Library Basics
January 2002
25
Library Basics
January 2002
26
3
Working with a Library Project
Objective
In this chapter, you will learn to:
■
Identify the types of projects.
■
Understand the library management use models.
■
Understand the library development methodology.
■
Create a library project using Library Explorer.
■
Create a new build library.
■
View the categories in which a library is categorized.
■
Import a part from the reference area to the build area.
■
Copy parts across libraries.
■
View footprints.
■
Verify parts.
■
Delete a part from a build library.
Types of Projects
There are two types of projects:
■
Design Projects
You need to create a design project to design and develop PCB boards. Design projects
are created using Project Manager.
■
Library Projects
January 2002
27
You need to create a library project to create and manage libraries of parts. These
parts are used in the design projects. The person who creates and manages a library
project is called a librarian.
Library Management Use Model
PCB Librarian suite provides you the following tools to perform library creation and
management tasks:
■
Library Explorer
■
Part Developer
■
Part Table Editor
Depending upon whether you are a librarian or a designer, you can use the tools to perform
specific tasks.
As a Librarian
Use Library Explorer to:
1. Create or open a library project which provides you with a build area where you can build
and modify libraries and parts.
2. Import reference libraries or parts you wish to modify into the build area.
3. Create any new libraries or cells.
4. Launch Part Developer to create or edit views.
5. Verify libraries.
6. Export new or modified libraries and parts to the reference library location.
7. Clean up the build area when finished.
Use Part Developer to:
1. Create or modify symbol, package, simulation views and part table views.
2. Verify the part.
Use Part Table Editor to:
1. Create or modify a part table.
January 2002
28
2. Verify a part table.
3. Add new parts to a part table.
As a Designer
As a designer, you can do the following:
1. Create a design project using Project Manager.
2. Specify the project libraries while creating the project.
Now if you want to either create a new part or modify existing parts in the project libraries,
you can launch the Part Developer tool. When you launch the Part Developer tool, it will
display the project libraries thus enabling you to modify and create new parts only in
them.
Note: Library Explorer will not be available on a project created through Project Manager as
library management oriented tasks like creating new libraries and categories, copying
libraries and so on, should only be done by a librarian.
January 2002
29
Library Project Concepts
Build Tab
Reference Tab
A library project is a project that provides you with an environment in which to build and
manage libraries and parts. A library project is created using the Library Explorer tool.
Displayed above is a typical Library Explorer window after a library project is created or
opened. Similar to the Windows Explorer, the Library Explorer window is divided into two
panes.
The left pane is further divided into two areas, namely the build area and reference area.
These two areas are accessible by the two tabs, Build and Ref. These are automatically
created when a new library project is created. The build area is the area for your private library
development needs. That is, it is the work area on which you can create, modify and manage
your libraries and parts.
The entries in the build area are controlled through a file called the cds.lib file. The
cds.lib file is a text file and contains the mapping of the library name as visible in the build
area to its actual physical location. This file is created automatically when a library project is
created. The cds.lib file is in the same location as the project file. For example, in the above
screenshot, the library project test stored in the tutorial_project_data is opened in
January 2002
30
Library Explorer. The actual lsttl library is stored in the
c:\tutorial_project_data\test\lsttl location, and the cds.lib fi;e contains the
following entry:
DEFINE lsttl c:\tutorial_project_data\test\lsttl
The Ref tab represents the reference area for the library project. The reference area stores
the parts that have been verified by the librarian and made available for use by the designers.
The list of libraries in the reference area are stored in the library list file named refcds.lib.
The refcds.lib file is similar to the cds.lib file and is stored in the same location as
the project file. As with the cds.lib file. the refcds.lib file contains the mapping of the
library name as visible in the reference area to its actual physical location.
By default, when you create a library project, the standard libraries provided by Cadence and
stored in the <your_install_dir>/share/library can be added as reference
libraries in your library project. You can also add your own libraries as reference libraries.
When you create and verify a library in the build area, you can export it to the reference area
so that other users can also use it. Usually, only the librarian should have permissions to
export the libraries to the reference area.
To create a new reference library, you must first create the library and it constituent parts in
the build area, verify them and then export the build library into the reference area.
Similarly, to modify, rename, or delete a reference library, you must import it into your build
area, make the necessary changes, and export it back to the reference area.
Using Library Explorer
Overview
Now, you will create a library project and name it tutorial_project.cpm. This library
project should be created in the tutorial_project directory. After you create the library
project, you will import a part that is categorized as a DECODER from the lcx reference
library to you build area. Then, you will copy the part from one build area library to another.
Next, you will view the associated footprint of the part from within Library Explorer. Finally, you
will verify the part.
January 2002
31
Creating a Library Project
The first step in working with libraries is to create a library project. In this section, you will learn
how to create a library project using Library Explorer.
Task Overview
Create a library project. The library project should be named tutorial_project.cpm.
This project should be created in the tutorial_project directory. The
tutorial_project_data directory contains the lcx library which will be used as the
reference library.
Steps:
1. Invoke the command shell of your computer.
2. Create a directory called tutorial_project.
3. In the command prompt, type libexp and press Enter.
The Library Explorer Product Choices dialog box appears. This dialog box displays
the product suites for which you have the licences. The availability of tools and features
of the tools are dependent on the choice of the product suite. For example, if you choose
PCB Librarian, you can access the Library Explorer and Part Developer tools, but not
their expert features such as data management and template creation.
January 2002
32
4. Select the PCB Librarian option and click OK.
The Library Explorer window appears on the background with a Getting Started dialog
box on the foreground. In this dialog box you can choose to either open an existing build
area or create a new build area.
5. Since you are going to create a new library project, select the Create a new Build Area
option and click OK.
January 2002
33
The New Project Wizard appears. This wizard enables you to quickly create a library
project. You will need to provide several information as you proceed with the wizard to
successfully create the project. First, you need to specify the project name and location.
6. Enter tutorial_project in the Project name text box and press Tab.
7. Click the Browse button and browse to the tutorial_project directory.
8. To continue, click Next.
The Select libraries page of the wizard appears. In this page, you select all the libraries
you want as reference libraries. The reference libraries will appear in the Ref tab of
Library Explorer window.
Note that by default, all the Cadence supplied libraries appear in the wizard page, and
unless you explicitly remove them, get added as reference libraries to your project.
January 2002
34
To add more libraries, either add them or import from another cds.lib file. If you import
from another cds.lib file, all the libraries listed in the cds.lib are added as reference
libraries.
For this project, you will remove the lcx library from the Cadence supplied libraries and
add the lcx library from the tutorial_project_data location.
9. To remove the lcx library from the Cadence supplied libraries, select the lcx library and
click Remove.
10. Next, to add the lcx library from the tutorial_project_data location, click Add.
January 2002
35
The Choose Directory dialog box appears.
11. To begin the process of adding the lcx library to your reference library list, browse to the
tutorial_project location.
The contents of the tutorial_project_data directory appears.
12. To add the lcx library as a reference library, double-click on the lcx folder and click OK.
The lcx library gets added to the list of reference libraries.
13. Click Next.
January 2002
36
The Summary page of the wizard appears.
14. To complete the creation of the project, click Finish.
After the project has been created, the Library Explorer message box appears.
15. Click OK.
January 2002
37
The tutorial_project library project is created and appears in the Library Explorer
window.
Caution
The tutorial_project_lib library appears in the Build tab. Do not delete this
library. This library contains the origin symbol which is required by the
Cadence tools. Physically, the library is named worklib and created in the
Library Project location. The cds.lib file displays the worklib as the
<projectname>_lib in the Build area.
Next, you will create a new library in the build area. Such libraries are called build libraries.
January 2002
38
Creating Libraries in the Build Area
You create libraries in the build area to store user created parts. You have full control over the
libraries in the build area. Other than creating new parts, you can also copy parts from other
libraries in the build area and import libraries from the reference area into your build area.
Task Overview
Create a library in the build area. Name the library my_library.
Steps
1. Before creating the build library, ensure that the Build tab is selected.
2. To begin creating a new build library, choose File > New > Build Library.
A new build library, named new_library is created.
3. To rename the library to my_library, type my_library press Enter.
The name of the library changes to my_library.
Next, you will identify decoder component in the lcx library and import it to the build area.
This is a two step process. First, you need to identify which component in the lcx library is a
DECODER and then you need to import it to the build area.
Viewing by Categories
You can categorize parts of your libraries. Normally the categorization is done as per the
functionality of the part such as FLIP-FLOP, DECODER etc.
To view library in terms of its component categories, you select the category view. This view
is available through Library Explorer.
Task Overview
View the part categories of the lcx library.
January 2002
39
Steps
1. To display the reference libraries, select the Ref tab.
2. Select the lcx library.
3. To view the categories, select View > Categories.
4. Double-click on the lcx library.
The Library Explorer view changes to show the categories into which the library is
divided.
5. To see the component that is classified as DECODER, select the DECODER folder in
the lcx library entry.
The lcx library has only one 3-TO-8 decoder is available.
6. To see the part that is classified as the 3-TO-8 DECODER, double-click on the 3-TO-8
folder.
The contents of the 3-TO-8 folder appears on the right pane. The part number is LCX138.
Now, you need to import this part to your build area.
January 2002
40
7. To import a part into the build area, you need to revert back to the part view. To revert to
the part view, select View > Categories.
The Library Explorer reverts to the part view.
8. Right-click on the lcx138 component.
9. Choose Import.
The part gets imported to the build area. It is important to remember that when you
import a part, the complete library structure is created in the build area. Therefore, in the
build area, you will see the lcx library under the Build Area Libraries, which will have
only the lcx138 part.
10. To view the imported part in the build area, click on the Build tab.
The build area of the tutorial_project library project appears.
11. Double-click on the lcx library.
The lcx138 component appears in the right pane.
You successfully imported the lcx138 component to the build area. Next, you will copy the
lcx138 part to the my_library build library.
Copying Parts
Library Explorer provides a Windows Explorer type ability to copy and paste parts from one
library to another.
Task Overview
Copy the lcx138 component from the lcx library to my_library.
Steps
1. Right-click on the lcx138 component in the Build area.
The short-cut menu appears.
2. Choose Copy.
3. Right-click on my_library.
4. Choose paste.
January 2002
41
The lcx138 part is copied from the lcx build library and copied to the my_library build
library. Similarly, using the short-cut menu, you can cut, delete, and rename components.
5. Now, rename the part to my_lcx138.
Next, you will view the footprints associated with this component.
Viewing Footprints
Using Library Explorer, you can view the footprints for a part. The footprints are used in the
Allegro design.
Task Overview
View the footprints of the my_lcx138 part.
Steps
1. Right-click on the my_lcx138 part in the my_library build area.
2. Choose View Footprint.
The Physical Properties dialog box appears. The dialog box contains the different
physical footprints for the packages in my_lcx138 part.
3. To close the dialog box, click Close.
4. Next, rename the part back to lcx138.
Next, you need to verify the part to ensure that the part can be used in a design.
January 2002
42
Verifying Parts
Overview of Types of Verifications
From Library Explorer, you can run a set of checks. These are:
View Verification
The view verification check does the following checks:
■
Symbol origin is centered.
Checks whether the origin always lies within the symbol and the symbol outline is at a
distance less than the maximum allowed offset from the origin.
■
Tristated pins have input and output loads defined.
Checks the presence of pin properties OUTPUT_LOAD and INPUT_LOAD for every tristate pin. The presence of a tri-state pin is denoted by the property OUTPUT_TYPE
=TS,TS.
■
Mandatory properties present in package file.
Checks whether the properties named BODY_NAME, PART_NAME, CLASS, and
JEDEC TYPE are present in the packages.
■
Consistent symbol name in symbol and package file.
Checks whether the cell name is the same as BODY_NAME property in the chips.prt file.
■
Consistent symbol and package in pin list.
Checks whether the pins are the same across symbol and package views.
Instantiation and Packaging
In this check, the parts are instantiated on a design sheet using Concept-HDL. One design
sheet is created for each package type. All the cells supporting a particular package type are
instantiated on the sheet of that package type. For each such created design sheet, a .cpm
file is made and saved in the working directory.
Next, Packager-XL is invoked to package each of the designs. Then, the following checks are
performed:
■
Checks the hdldir.log, pxl.log and edbconfig.log files for errors.
■
Checks whether the schematic view has non-zero verilog.v and .sir files.
■
Checks whether the packaged view has non-zero .dat files.
January 2002
43
■
If the netrev option ia checked (from the Options button), then Allegro is invoked to
create an empty board and netrev. The board is then upreved with the netlist, and a
physical view is created. After creating a physical view, the presence of the netrev.lst
and .brd files in the physical view is checked. Finally the reports of the result are
reported in a log file.
■
Reports the result of the test on the library in a report file called ftb.rep. The report file
is created in the current working directory.
■
Declares the test library as passed, if the Concept-HDL and the PXL run are successful.
■
Reports the nature of a failure in the ftb.rep file, if any errors occur in the ConceptHDL run or at the Packager-XL run.
If the Use project ptf files for verification option is checked, all the .ptf files are loaded
as specified in the ptfdirective file, and scanned for rows corresponding to the part concerned.
If the rows have the given PACK_TYPE property as the key property, then all the other key
properties get added to the part. The properties that are being added are checked to ensure
that the properties are not duplicated in the corresponding symbol.css file.
The designs are then packaged and the o/ps is checked. If the o/ps are successful, the design
is netreved from the created .pst file.
The following tasks are also performed:
■
Checks whether pack_type is present in .ptf files, but not in the chips.prt file.
■
Ensures that if the PACK_TYPE property on it is conflicting, then the symbol is not
instantiated for a particular pack type. In other words, it skips the parts if the PACK_TYPE
property on it is in conflict.
■
It checks if pack type is a part of the primitive name in the chips.prt file.
To switch on/off the options mentioned above, you have the following check boxes:
■
Use Project .ptf files for verification
If you select this rule, part table files are used in instantiation and packaging. If no part
table files are specified in the project file, the cell-level .ptf file is used by default.
■
Use allegro board (netrev)
If you select this option, the part or library is verified for the complete Front to Back flow.
■
Generate Pass/Fail report
This option is enabled only if you select a library.
January 2002
44
Note: If you select the Generate Pass/Fail option, each part is verified separately. This is
a time consuming process.
Advanced View Checks
Select this option to launch CheckPlus. You can run your own custom-defined checks using
CheckPlus.
VHDL Compilation
Note: This check is available only in the expert version of Library Explorer.
You use the VHDL Compilation option to compile the generated VHDL wrapper. You can
use either NCVHDL or CV to compile the wrapper. You can specify the tool to compile the
VHDL wrapper in the Enter command in the VHDL compilation dialog box. This dialog
box is displayed when you click the Options button in the Verifications dialog box.
Verilog Compilation
You use the Verilog Compilation option to compile the generated Verilog wrapper. You can
use NCVERILOG to compile the wrapper. You can specify the tool to compile the Verilog
wrapper in the Enter command for Verilog compilation dialog box. This dialog box is
displayed when you click the Options button in the Verifications dialog box.
Verify with Templates
You use the Verify with Templates option to verify a part against a template. The verification
is done only for those values that exist in the template file as well. The output is displayed in
a dialog box. The output is divided into two sections, Overview and Details.
In the Overview section, the overview of the differences are displayed. In the Details
section, each of the differences in the logical, physical and symbol levels are detailed.
Task Overview
For the lcx138 component in the my_library build library, run only the View Verification
check with all the options.
January 2002
45
Steps
1. Select the lcx138 part in the my_library build library.
2. Choose Tools > Verify.
The Verification dialog box appears.
3. Select the View Verification option.
4. To ensure that all the part will be checked for all the options of the View Verification
check, click Options.
The View Verification dialog box appears. Ensure that all the options are checked.
5. Click OK.
The View Verification dialog disappears.
6. To start the verification process, click OK.
The Verification Results message box appears. It should report no errors.
7. Click OK.
8. Click Close to close the Verification dialog box.
Deleting Parts
Library Explorer provides you with a Window Explorer type interface for deleting parts.
Task Overview
Delete the lcx138 part from the my_library build library.
Steps
1. Right-click on the lcx138 part.
2. Choose Delete.
January 2002
46
The Confirm Folder Delete dialog box appears.
3. Since the part is to be deleted only from the build area, click Yes.
The lcx138 part gets deleted from the my_library build library.
Summary
You covered a lot in this chapter. In this chapter, you learned about the types of projects. You
learned the library management use models and the library development methodology. You
also learned how to create a library project and work in it. In the next chapter, you will learn
to create a part with pins split across multiple symbols.
January 2002
47
January 2002
48
4
Creating Parts With Pins Split Across
Symbols
Objective
To become familiar with the methodology and steps involved in creating a part with pins split
across symbols.
■
Understand the methodology involved in creating parts.
■
Setup Part Developer to assign properties globally to all symbols and packages of a new
part.
■
Do intermediate saves while creating a part.
■
Create a part with pins split across symbols.
■
Access Allegro footprints to specify JEDEC_TYPE property.
■
Extract pin numbers from the Allegro footprint.
■
Verify parts using View Verification check.
■
Create a new reference library.
■
Export the part to the new reference library.
Part Creation Methodology
Part Developer enables you to create and modify symbol, package, and part table views of
parts in Concept-HDL libraries. You should follow the sequence of steps listed below to
ensure an effective use of the Part Developer tool.
1. Refer to the datasheet. The datasheet contain all the information that you require to
create parts.
January 2002
49
Creating Parts With Pins Split Across Symbols
2. Configure Part Developer to correctly interpret the pin names.
3. Enter the logical pin information. Logical pins are the pin names as they appear on the
datasheet.
4. Specify the values in the Setup Options for creating a part. These values are dependent
on the values in the datasheet and the standards you follow. These values include
properties that are to be placed on the symbols, pins and packages, the placement and
load values of the pins, the format of the symbols as they will appear in Concept-HDL,
the format of the low asserted pins, and the interpretation of the pin names.
5. Create the packages for the part.
This creates the chips view for the part.
6. Create the symbols for the part.
This creates the symbol views.
7. If required, create the simulation views. This involves creating the Verilog and the VHDL
wrappers and map files.
8. Verify the parts that you have created for use in the design flow.
Creating a Part
Task Overview
Create the N87C196NT part in the my_library build library. Set up Part developer to:
■
Add the property Library_Name with the value my_library to all the packages and
symbols.
■
Display the pin texts in 0.6 grid size.
January 2002
50
The relevant part of the datasheet is stored in the tutorial_projects/datasheets
location. A snapshot of the datasheet is displayed below:
Starting Part Developer
Since the part has to be created in the my_library build library, ensure that my_library is
selected in Library Explorer. To launch Part Developer:
1. Choose Tools > Part Developer.
January 2002
51
The Create/Open Part dialog box in the Part Developer window appears.
2. Since you need to set up Part Developer to add global properties, click Cancel.
The blank Part Developer window appears.
Setting up Part Developer
Task Overview
Set up Part Developer to associate and display a property Library_Name with the value
my_library for all packages and symbols. Also, all the packages should have the
BODY_NAME property with value as ? and the symbols should display pin text in 0.6 grid size.
Steps
1. Choose Tools > Options.
January 2002
52
The Part Developer Setup Options dialog box appears. By default, the Properties tab is
selected. The Library_Name property and its value will be entered in this tab.
2. Enter Library_Name in the Property Name column.
3. Click the corresponding cell in the Value column.
4. Enter my_library.
5. To display both the property name and its value in the symbol, select Both from the
Visible drop-down list box.
6. To associate the property with both symbols and packages, select Package checkbox
in the Package group box.
Note: The Symbol checkbox is selected by default.
7. Click Add.
The property will get added to all the symbols and packages created in this session of
Part Developer.
8. Next, enter BODY_NAME in the Property Name column.
9. Enter ? as its value.
10. Since the BODY_NAME property is to be added only to the packages, deselect the
Symbol check box.
11. Click Add.
12. Next, configure Part Developer to display the pin text in 0.6 grid size. Click the Symbol
tab.
January 2002
53
13. Click in the Pin Text Size text box.
14. To display the pin notes in 0.6 grids, enter 0.6.
After you configure the properties, the next step is to configure the format.
Configuring Format Options
The Format options page helps you to determine the way in which you will read and write low
asserted pins, and how the asymmetrical parts, sizeable pins and vector pins are displayed
when a part is read into Part Developer.
Following is a description of the two group boxes that constitute the Format page.
■
Low Asserted Pin Syntax.
The setting in this group box determines the pin names that Part Developer will treat as
low asserted while reading a part. You also specify the notation that Part Developer
should use to write a low asserted pin into the symbol and the chips.prt file. You can
choose to display the pins with following notations as low asserted pins on the symbol
and then write them to the symbol file in one of the following ways:
❑
Either with a asterisk (*) or _N suffix: In this case any pin which has either a * or _N
in its name is read as a low asserted pin. You can then determine whether you want
to write the low asserted pin into the symbol file with either the '*' or '_N' suffix.
❑
With a star (*) notation: In this case, the pins with a * are read as a low asserted pin.
The pin is written back to the symbol file with the * suffix.
❑
With a _N notation: In this case, the pins with _N are read in a low asserted pin. They
are written into the symbol file with the _N notation.
Note: Select the Use minus [-] sign for low asserted pins in Package
view to ensure that the pins that are considered low asserted are written into the chips
file with a minus [-] sign. If you leave this unchecked, and depending on which pins you
treat as low asserted, they will get written into the chips.prt file with the same suffix
as they are written into the symbol file (basically, either ‘*’ or ‘_N’).
Caution
You must follow a standard convention for reading and writing the low
asserted pins, otherwise the associated pin texts might get lost. For
example, while creating a part, you decide on writing the low asserted
pins with _N assertion. As a result, all the low asserted pins of the symbol
have _N appended to them. Now to modify the part, you load the part back
January 2002
54
into Part Developer and change the low assertion write back option to *.
Now when you save the part, the associated pin text will be lost. This is
because when saving, Part Developer tries to associate pin names with
pin texts and fails to find a pin with name, say A*, on the symbol (since
the symbol has A_N) and as a result it doesn’t write any PIN_TEXT
property for low asserted pins.
■
Chips File Reading Options
The options in this group box determines how Part Developer reads the chips.prt file
for displaying the following:
❑
Asymmetrical parts
Asymmetrical parts have multiple functionality. Corresponding to each functionality,
there is a pin list. All sections or slots that have the same functionality have the same
pin list. The slots that have the same functionality form one group. Depending on the
part, there may be multiple groups. You can choose to display the pin numbers in
such a way that the group numbers are also visible. You can do this by selecting the
Use group format for reading asymmetrical parts check box.
❑
Sizeable pins
Sizeable pins can be displayed in Part Developer in one of the following ways: Slot
Number-Base Name or Base Name - Slot Number. In the Slot Number - Base Name
format, the numeric part is treated as the slot number while the alphanumeric string
part is treated as the base name. For example, if the pin name given is 1A, it is taken
as base name A and slot number 1.
In the Base Name- Slot Number format, the alphanumeric string part is treated as a
base name and numeric part is treated as a slot number. For example, if the pin
name entered is A1, it is treated as a sizeable pin with base name A and slot number
1.
❑
Vector pins
Vector pins can be displayed in Part Developer in one of the following ways: Bit
Number - Base Name or Base Name - Bit Number. In the Bit Number - Base Name
format, the numeric part is treated as the bit number while the alphanumeric string
part is treated as the base name. For example, if the pin name given is 1A, it is taken
as base name A and bit number 1.
In the Base Name - Bit Number format, the alphanumeric string part is treated as a
base name and the numeric part is treated as a bit. For example, if the pin name
entered is A1, it is assigned the base name A and the bit number 1.
January 2002
55
Task Overview
Configure Part Developer to write low asserted pins with ‘*’ suffix.
Steps
1. Select the Format tab.
The Format property page appears.
2. Ensure that the Suffix ‘*’ and Suffix ‘_N’ option for reading and Suffix ‘*’ for writing is
selected. This is the default selection and suffices for most of the part creation scenarios.
After you configure the Format options, you need to configure the pin name
interpretations.
January 2002
56
Configuring Pin Name Interpretation
Overview
Logical pin names appear in the datasheets in following four patterns:
■
Alphanumeric String (for example, A, B, and EN)
■
<Alphanumeric String><Numeral> (for example, A0, A1)
■
<Numeral><Alphanumeric String> (for example 0A, 1A)
■
<Numeral><Alphanumeric String><Numeral> (for example 1A1, 1A2)
Note: Any string that is flanked by alphabets on both sides is treated as an alphanumeric
string. For example, A, A1A.
Alphanumeric String
Usually, scalar pin names, such as A, B, EN, A1A and so on appear in data sheets as
alphanumeric strings. Any alphanumeric string that is not flanked by numerals falls into the
Alphanumeric string category. These pins are always treated as scalar pins.
<Alphanumeric String>< Numeral>
Data sheets use the alphanumeric string numeral names for representing vector bits or
sizeable pins. For example, the names A0, A1, A2..A7 specify an 8-bit vector bus. Here,
A is the base name and 0-7 is the bit range. Similarly, the names B1, B2, B3, B4 specify
the sizeable pin B in a part with four slots. The pins can be interpreted in the following ways:
Base Name: The entire alphanumeric string is treated as the base name and it is treated as
a scalar pin.
Base Name-Bit: The alphanumeric string part is treated as a base name and the numeric part
is treated as a bit number. For example, if the pin name entered is A1, it is assigned the base
name A and the bit number 1.
Base Name-Slot: The alphanumeric string part is treated as a base name, and the numeric
part is treated as a slot number. For example, if the pin name entered is A1, it is treated as a
sizeable pin with the base name A and the slot number 1.
January 2002
57
Numeral Alphanumeric String
Sometimes data sheets may also use numeral alphanumeric string names for representing
vector bits, sizeable pins, or a scalar pin belonging to a slot group. For example, the names
0A, 1A, 2A..7A specify an 8-bit vector bus or the names 1B, 2B, 3B, 4B specify a
sizeable pin B in a part with four slots. Similarly, the scalar pins 1OE and 2OE are used to show
that the pin is in two slot groups. The pins will be interpreted in one of the following ways:
Base Name: The entire alphanumeric string is treated as a base name and taken as a scalar
pin.
Bit-Base Name: The numeric part is treated as the bit number while the alphanumeric string
part is treated as the base name. For example, if the pin name given is 1A, it is taken as the
base name A and the bit number 1.
Slot-Base Name: The numeric part is treated as the slot number while the alphanumeric
string part is treated as the base name. For example, if the pin name given is 1A, it is taken
as the base name A and the slot number 1.
Group-Base Name: The numeric part will be treated as group number while alphanumeric
string part will be treated as base name. For example, if the pin name given is 1A, it will be
taken as the base name A and the group number 1.
<Numeral>< Alphanumeric String>< Numeral>
Usually, data sheets use the <numeral>< alphanumeric string>< numeral> notation for
representing sizeable pins belonging to different groups. For example, if a part has 8 slots
with slots 1 to 4 in one group and 5 to 8 in another group, then a sizeable pin A of that part
appears on the data sheet as following:
1A1, 1A2, 1A3, 1A4
2A1, 2A2, 2A3, 2A4
You can enter these pins in two steps:
■
enter 1A1- 1A4 and
■
enter 2A1-2A4
These pins can be interpreted in the following ways:
Base Name: The entire alphanumeric string is treated as a base name.
January 2002
58
Slot-Base Name: The starting numeral is treated as the slot number while the rest of the
name is treated as base name. For example, if the name is 1A1, it is taken as pin A1 in the
slot as1.
Bit-Base Name: The starting numeral is treated as bit number while the rest of the name is
treated as a base name. For example, if the name is 1A1, it is taken as pin A1 and the bit
number 1.
Group-Base Name-Slot: The starting numeral is taken as a group number and the end
numeral is treated as a slot number in that group. So, if the pin name is 1A1, it is taken as
base pin A, slot 1, and group 1.
Group-Base Name-Bit: The starting numeral is taken as the group number and the end
numeral is treated as the bit number. Therefore, if the pin name is 1A2, it is taken as base pin
A, bit 2, and group 1.
Base Name-Slot: The end numeral is treated as slot number while rest of the alphanumeric
string is taken as the base name. For example, if the pin name is 1A1, it is treated as base
pin 1A in slot 1.
Base Name-Bit: The end numeral is treated as bit number while rest of the alphanumeric
string is treated as base name. For example, if the pin name is 1A1, it is treated as base pin
1A, and bit 1.
Group-Base Name: The starting numeral is taken as the group number while the rest of the
name is treated as a base name.
Task Overview
The N87C196NT has scalar pins. You will configure the pin interpretation to accept all pins
as scalar pins. For this, you need to setup the pin interpretation defaults as Base Name.
Steps
1. Click Edit in the Pin Name Interpretation group box in the Logical Pins dialog box.
January 2002
59
The Pin Name Interpretation tab of the Part Developer Setup Options dialog box
appears.
2. Select Base Name in all the three sections.
3. Click OK.
This will set up Part Developer to interpret all pins as scalar pins.
After you set up Part Developer, you begin the process of creating the parts.
January 2002
60
Entering Part Properties
Task Overview
The N87C196NT part should have the following properties:
■
Part Name should be N87C196NT
■
Physical Part Name should be the same as part name.
■
Part Type should be IC.
Steps
1. Click Create New in the Create/Open Part dialog box.
The New Part Properties dialog box appears. Notice that the my_library build library
is selected by default.
2. Enter N87C196NT in the Part Name field.
Note: The Physical Part Name field also gets filled in automatically as you enter the part
name field. This field is used as the PART_NAME property in the chips.prtfile.
3. Click OK.
January 2002
61
The Logical Pins dialog box appears.
Entering Logical Pins
Task Overview
Enter the pin information as given in the datasheet into Part Developer. Open the datasheet
and go to the pin descriptions table. The datasheet is located in the tutorial_project/
January 2002
62
datasheets location. The pins will be entered in the same sequence as they appear in the
datasheet.
Steps
1. The first few pins in the Pin Descriptions table are power pins. To enter a power pin,
select POWER from the Pin Type drop-down list box.
2. Enter Vcc, Vss,Vss1, VREF, VPP, ANGND in the Pin Name text box.
Important
Note that the Pin Descriptions table has multiple entries for the Vss1 power pin. In
Part Developer you need to enter the name only once in the logical pins list. Later
when creating packages, you can associate multiple physical pins to a power pin.
3. To add the pin to the logical pin list, click Add.
The power pins gets added to the logical pins list.
4. Next, to enter an input pin, select INPUT from the Pin Type drop-down list box.
5. Enter XTAL1 in the Pin Name text box and click Add.
6. The next couple of pins in the Pin Descriptions table are output pins. To enter an output
pin, select OUTPUT from the Pin Type drop-down list box.
7. Enter XTAL2, P2.7 in the Pin Name text box and click Add.
8. The next pin in the table RESET which is an active low input pin. Select INPUT from the
Pin Type drop-down list box.
9. Enter RESET in the Pin Name text box.
10. To make an pin active low, select the Active Low check box and click Add.
11. The next couple of pins are input pin, but not active low. Therefore deselect the Active
Low check box.
12. Enter P5.7, NMI in the Pin Name text box and click Add.
13. Next, to enter the P5.1 output pin, select OUTPUT from the Pin Type drop-down list
box.
14. Enter P5.1 in the Pin Name text box and click Add.
15. The next two pins in the table are active low input pins. Select INPUT from the Pin Type
drop-down list box.
January 2002
63
16. Enter EA, HOLD in the Pin Name text box.
17. Select the Active Low check box and click Add.
18. The next two pins in the table, HLDA and BREQ are active low output pins. Therefore,
select OUTPUT from the Pin Type drop-down list.
19. Enter HLDA, BREQ in the Pin Name text box and click Add.
20. The next four pins in the table are active high output pins. Therefore, deselect the Active
Low check box.
21. Enter P5.0, P5.3, P5.2,P5.5 in the Pin Name text box and click Add.
22. The next pin (P5.6) in the Pin Descriptions table is an input pin. Therefore, select INPUT
from the Pin Type drop-down list box.
23. Enter P5.6 in the Pin Name text box and click Add.
24. Next few pins in the table are bidirectional pins. To enter a bidirectional pin, select BIDIR
When creating large parts, it is a good idea to keep saving pin information every once in
a while. For this, you do an intermediate save.
Intermediate Saving of Parts
When you save a part in Part Developer, several pre-save checks are run. So if you try to save
an incomplete part, you might get some errors and the part will not get saved.
Therefore, to save a work-in-progress part, you should use the intermediate save feature of
Part Developer.
To save the part information in an intermediate save file:
1. Close the Logical Pins dialog box.
2. Choose File > Intermediate Save.
The Save As dialog box appears.
3. Enter n87c196ntin the File Name field and press Enter.
You successfully saved the part in an intermediate file.
After you do an intermediate save, you can continue entering more pins.
January 2002
64
Continuing Pin Entry
1. Right-click on the Logical Pins entry in the tree view.
2. Choose Edit Pin List.
3. Enter P5.4,P6.2,P6.3, EPA0-EPA9 in the Pin Name text box and click Add.
4. The next four pins are input pins. Select INPUT from the Pin Type drop-down list box.
5. Enter ACH4-ACH7 in the Pin Name text box and click Add.
6. The next four pins in the datasheet are bidirectional pins. Select BIDIR from the Pin
Type drop-down list box.
7. Enter P6.4-P6.7 in the Pin Name text box and click Add.
8. The next few pins are output pins. Select OUTPUT from the Pin Type drop-down list
box.
9. Enter P2.0-P2.1,P4.0-P4.7 in the Pin Name text box and click Add.
10. Next four pins in the table are bidirectional pins. To enter a bidirectional pin, select BIDIR
11. Enter A16-A19in the Pin Name text box and click Add.
12. The next pin is an active low output pin. Select OUTPUT from the Pin Type drop-down
list box.
13. Enter INTOUT in the Pin Name text box.
14. Select the Active Low check box and click Add.
15. The final eleven pins in the table are bidirectional pins. To enter a bidirectional pin, select
BIDIR from the Pin Type drop-down list box.
16. Enter P2.2, SLP0-SLP7 in the Pin Name text box.
17. Deselect the Active Low check box and click Add.
18. To accept the entries and close the Logical Pins dialog box, click OK.
After the logical pins have been entered, you create the packages.
January 2002
65
Creating Packages
Task Overview
Create the PLCC package for the N87C186NT part.
Steps
1. To begin the process of creating packages, choose File > New > Package.
January 2002
66
The New Package dialog box appears. By default, the General tab is selected.
2. Since the N87C196NT part comes in PLCC package, enter PLCC in the Specify
Package Type text box.
3. Click Specify Footprint.
January 2002
67
The Physical Property dialog box appears.
You need to specify the JEDEC_TYPE value for the package. The value for the
JEDEC_TYPE property will be picked up from the Allegro footprints of standard
packages provided by Cadence.
4. Click in the cell under the Value column next to the JEDEC_TYPE entry.
5. To select the appropriate value for the JEDEC_TYPE property, click Browse.
January 2002
68
The Footprints dialog box displays. This has the complete list of footprints supplied by
Cadence.
6. Select plcc68 and click OK.
You selected the value for the JEDEC_TYPE property.
7. To close the Physical Properties dialog box, click OK.
Next, you need to update the value of the BODY_NAME property to be the same as the
part name. This is a standard requirement for your parts to be usable in the design flow.
8. To change the value of the BODY_NAME property, double-click on the Value column.
9. Enter N87C196NT as the value for the BODY_NAME property.
10. Next, you need to enter the physical pins and map them to the logical pins that you
entered earlier. To get to the page where you enter physical pins, click the Physical Pin
Mapping tab.
You can either add the physical pins manually, or extract them from the footprint. To
ensure correctness of the entered physical pins, you should always extract the pins from
the footprint.
11. To extract the pins from the footprint, select the Extract from Footprint option.
January 2002
69
12. Click Pin Numbers.
The Part Developer message box appears. This message box states that all pin numbers
extracted from the footprint will be added as unmapped pins to the package.
13. Click OK.
The 68 physical pins listed in the footprint get added as physical pins. Note that the pin
numbers are not in a sorted order.
14. To sort the physical pins, click on the Number column heading.
Next, the physical pins need to be mapped to the logical pins. The general method to
map a physical pin with logical pin is to select both the pins and click on the Map button.
January 2002
70
15. As per the datasheet, physical pin 1 is mapped to logical pin P5.4. Therefore, select 1 in
the Physical Pins list, and select P5.4 in the Logical Pins list.
16. To map the selected pins, click Map.
The physical pin 1 is mapped to the logical pin P5.4.
Note: Whenever you map a physical pin to a logical pin, the pin number moves from the
Physical Pins list to the Logical Pins list and the next pin number in the list gets selected
in the Physical Pins list. This eases the pin mapping as you do not explicitly need to select
a physical pin to map to a logical pin. You can select the logical pin that you want the
automatically selected physical pin to be mapped to, and map it.
17. To map pin number 2 to logical pin P5.6, select P5.6 in the Logical Pins list.
18. Click Map.
19. Similarly, see the datasheet and map the first 10 physical pin numbers.
Note: Other than single pin mappings, you can also select multiple physical pins to be
mapped to multiple logical pins. To ensure that pin mappings are done correctly, you may
need to sort the pins in either ascending or descending order.
The physical pins 11-14 will be mapped to the logical pin A19-A16 by using this method.
To select multiple pins, press CTRL + Click on the pins to be selected.
Currently, the logical pins are listed in the order of A16-A19. If you multi-select the pins
and do the mapping, the pin number 11 will get mapped to logical pin A16 and so on.
However, what is required is that the pin number 11 be mapped to logical pin A19.
Therefore, first the order of the logical pin needs to be reversed.
20. To change the sorting order of the pins 11-14, select the pins and right-click.
21. Choose Sort Descending.
The pins 11-14 are sorted in descending order.
22. To map pin number 11 - 14 to logical pins A19-A16, first select the pin numbers 11,12,13
and 14 in the Physical Pins list.
23. Next, select A19,A18,A17,A16 in the Logical Pins list.
24. Click Map.
25. Similarly map the other physical pins to their corresponding logical pins.
26. When you get to pin number 68, you will get an error message saying that this pin has
already been mapped. This is situation where there are two physical pins (34 and 68) for
January 2002
71
a power pin (VSS1) of the same name. To handle such situation, Part Developer allows
you to replicate the power pin.
27. To replicate the VSS1 power pin, right-click on VSS1.
28. Select Replicate.
The Replication Factor dialog box displays. In this dialog box you can determine the
number of replicated power pins. The default value is one.
29. Since only one more VSS1 power pin is required, click OK.
30. Map the physical pin 68 to the replicated VSS1 power pin.
31. To complete the creation of the package, click OK.
After you create a package, the next step is to create symbols for the part.
Creating Split Symbols
You can create symbols with pins split across them for reasons such as:
■
Reflect the way the parts functionality is used in a schematic.
■
Enable a more manageable display for large pin count parts.
Task Overview
Create two symbols for the N87C196NT part where the pins are split across the symbols.
Symbol 1 should have the following pins:
■
XTAL1, XTAL2, RESET*, NMI, EA*, P4.0 - P4..7, A16-A19, SLP0-SLP7, Power Pins
Symbol 2 should have the remaining pins.
January 2002
72
Steps
Part Developer provides a Symbol Creation Wizard which enables you to efficiently and
correctly create symbols.
1. To begin creating the symbols, choose File > New > Symbol.
The Split Symbol page of the Symbol Creation Wizard appears. By default, the All
Pins option is selected.
2. To create two symbols, select the Split Pins across symbols option.
3. By default, the value in the Number of symbols is two. Since the pins are to be splitted
into two symbols, there is no change required for the Number of symbols field. To
continue, click Next.
January 2002
73
The Pin Selection page of the Symbol Creation Wizard appears. This page displays
the list of available logical pins and gives the choice to associate a logical pin with a
particular symbol.
The following pins should be added to the first symbol:
■
XTAL1, XTAL2, RESET*, NMI, EA*, P4.0 - P4..7, A16-A19, SLP0-SLP7
The remaining pins should be on the second symbol.
4. To add the above mentioned list of pins on the first symbol, select the corresponding
check box under the sym_1 heading for each pin. For example, to add the XTAL1 pin on
the first symbol, select the checkbox under sym_1 heading next to XTAL1 entry.
5. Similarly, associate the other pins to the second symbol.
January 2002
74
The Summary page of the Symbol Creation Wizard appears. This page displays the
list of symbols and the pins associated with each symbol.
7. Check the summary page and click Finish.
The Symbol Creation Wizard creates the two symbols by splitting the pins across the
symbols.
Saving Parts
Task Overview
Save the N87C196NT part.
January 2002
75
Steps
➤
To save the part, choose File > Save.
The Part Developer Errors dialog box appears. It should show no errors.
Next, you will verify the part for its validity.
Verifying Parts
The parts that you created should be error free and usable in the design flow. Part Developer
provides you with robust verification tools which ensure that the parts are correct and usable.
Task Overview
Verify the N87C196NT part for cross view errors and instantiation and packaging errors. This
is done by running the View Verification and Instantiation and Packaging
checks.
View Verification Check
The view verification check does the following checks:
■
Symbol origin is centered.
Checks whether the origin always lies within the symbol and the symbol outline is at a
distance less than the maximum allowed offset from the origin.
January 2002
76
■
Tristated pins have input and output loads defined.
Checks the presence of OUTPUT_LOAD and INPUT_LOAD pin properties for every tristate pin. The presence of a tri-state pin is denoted by the OUTPUT_TYPE =TS,TS pin
property.
■
Mandatory properties present in package file.
Checks whether the BODY_NAME, PART_NAME, CLASS, and JEDEC_TYPE
properties are present in the packages.
■
Consistent symbol name in symbol and package file.
Checks whether the symbol text is the same as BODY_NAME property in the
chips.prt file.
■
Consistent symbol and package in pin list.
Checks whether the pins are the same across symbol and package views.
Instantiation and Packaging
In this check, the parts are instantiated on a design sheet using Concept-HDL. One design
sheet is created for each package type. All the cells supporting a particular package type are
instantiated on the sheet of that package type. For each such created design sheet, a .cpm
file is made and saved in the working directory.
Next, Packager XL is invoked to package each of the designs. Then, the following checks are
performed:
■
Checks the hdldir.log, pxl.log and edbconfig.log files for errors.
■
Checks whether the schematic view has non-zero verilog.v and .sir files.
■
Checks whether the packaged view has non-zero .dat files.
■
If the netrev option is checked (from the Options button), then Allegro is invoked to
create an empty board and netrev. The board is then upreved with the netlist, and a
physical view is created. After creating a physical view, the presence of the netrev.lst
and .brd files in the physical view is checked. Finally, the reports of the result are
reported in a log file.
■
Reports the result of the test on the library in a report file called ftb.rep. The report file
is created in the current working directory.
■
Declares the test library as passed, if the Concept-HDL and the Packager-XL run are
successful.
■
Reports the nature of a failure in the ftb.rep file, if any errors occur in the ConceptHDL run or at the PXL run.
January 2002
77
If the Use project ptf files for verification option is checked, all the .ptf files are loaded
as specified in the ptf directive file, and scanned for rows corresponding to the part
concerned. If the rows have the given PACK_TYPE property as the key property, then all the
other key properties get added to the part. The properties that are being added are checked
to ensure that the properties are not duplicated in the corresponding symbol.css file.
The designs are then packaged and the o/ps is checked. If the o/ps are successful, the design
is netreved from the created .pst file.
The following tasks are also performed:
■
Checks whether pack_type is present in ptf files, but not in the chips.prt file.
■
Ensures that if the PACK_TYPE property on it is conflicting, then the symbol is not
instantiated for a particular pack type. In other words, it skips the parts if the PACK_TYPE
property on it is in conflict.
■
It checks if pack type is a part of the primitive name in the chips.prt file.
To switch on/off the options mentioned above, you have the following check boxes:
■
Use Project ptf files for verification
If you select this rule, part table files are used in instantiation and packaging.
If no part table files are specified in the project file, the cell-level ptf is used by default.
■
Use allegro board (netrev)
If you select this option, the part or library is verified for the complete Front to Back flow.
■
Generate Pass/Fail report
This option is enabled only if you select more than one part or when you select a library that
has more than one part.
Note: If you select the Generate Pass/Fail option, each part is verified separately. This is a
time consuming process.
Steps
1. To begin the process of verifying the part, choose Tools>Verify.
January 2002
78
2. To do the verification of the stand-alone views and cross-view checks, select the View
Verification option. This is selected by default.
3. To ensure that all the checks that View Verification does are selected, click Options.
The View Verification dialog box appears.
By selecting the options in this dialog box you can determine which of the View
Verification checks will be run on a part. Since for N87C196NT all the checks should be
run, ensure that all the checks are selected.
4. Click OK.
January 2002
79
The View Verification dialog box closes.
5. To run the View Verification check on the part, click OK.
The Verification Results dialog box appears. It should show that all the checks have
passed.
Next, check the part for instantiation and packaging errors.
6. Select the Instantiation and Packaging radio button.
7. To run this check to verify the packaging of the parts, click Options.
The Instantiation and Packaging dialog box appears.
8. Ensure that the Use project ptf files for verification and Upto allegro board (netrev)
options are unchecked.
9. Click OK.
The Verification Results dialog box appears. It should show that all the checks have
passed.
Congratulations. You have successfully created the N87C196NT part.
January 2002
80
Viewing the Part in Concept HDL
After you create the part, you can view it in Concept HDL by launching Concept HDL from
within Part Developer.
Task Overview
View the N87C196NT in Concept HDL.
Steps
1. Select the symbol sym_1 in the tree view.
2. Choose Tools > ConceptHDL.
An error message pops-up informing you that Concept HDL is not part of the PCB
Librarian tool suite. Click OK to destroy the message box.
The Concept-HDL Product Choices dialog box appears. This dialog box lists all the
product suites that have Concept-HDL licence.
3. For this example, select the PCB Librarian Expert suite.
4. Click OK.
January 2002
81
Concept-HDL launches displaying the selected symbol and its properties.
A partial view of the symbol with the properties is also displayed below
:
After you create a part and verify it, you should export the part back into the reference area.
January 2002
82
Exporting Parts to the Reference Area
Task Overview
Export the N87C196NT part which you created in the my_library build library to the
reference area.
Steps
1. Since parts (and libraries) can only be exported from within Library Explorer, go to the
Library Explorer window.
2. Right-click on the n87c196nt part in the my_library build library.
3. Select Export from the pop-up menu.
The Export Destination dialog box appears.
4. Notice that although you selected only the N87C196NT part for export, the Source
Library column displays the build library name in which the part is stored. This is
because when you select to export a part, the complete library structure is exported.
That is why you need to specify the destination library. You need to determine the
destination library into which you want to export the part. The destination library can
either be one of the existing reference libraries or you can create a new reference library
altogether. In this example, you will create a new reference library called
my_reference_library and store it in the c:\my_reference_libs directory. You
will need to create this directory outside Library Explorer.
5. To create a a new reference library, click New Ref Lib.
January 2002
83
The New Reference Library dialog box appears.
In this dialog box you enter the name of the reference library and its location.
6. Enter my_reference_libs in the Name of the new library field.
7. To change the reference library location, click Browse.
8. Select the my_reference_libs location and click OK.
The New Reference Library dialog box disappears.
Now, you need to select the my_reference_libs from the Destination Library drop
down list box in the Export Destination dialog box.
9. To see the list of available reference libraries, click the down arrow in the Destination
Library list box.
10. Select my_reference_libs and click OK.
The Library Explorer dialog box appears. It should show that the export was
successful.
11. Click OK.
12. To verify that the new reference library and the exported part shows up in the Ref area,
click the Ref tab.
January 2002
84
13. Browse and view the contents of the my_reference_libs reference library. It should
show the N87C196NT part that you exported from the my_library build library.
Once you export a part to the reference library, you can delete the part from the build
library.
14. To begin the process of deleting the N87C196NT from build area, click the Build tab to
view the build area.
15. Select N87C196NT in the my_library build library.
16. Press Delete.
The Confirm Folder Replace dialog box appears.
17. Click Yes to delete the part from the build area.
You deleted the part from the build area.
Summary
In this chapter you learned about the methodology and steps involved in creating a part with
pins split across symbols. In the next chapter, you will learn to modify the part that you created
in this chapter.
January 2002
85
5
Modifying a Split Part
Objective
To become familiar with the steps involved in modifying a split part.
■
Import a part.
■
Setup Part Developer to view the part data in the same format as you had entered.
■
Add/delete logical pins.
■
Add/remove power and NC pins.
■
Modify packages and symbols by resplitting the pins across symbols.
■
View the symbols in Concept-HDL and snap the new pins to the boundary of the symbol.
■
Verify the part.
■
Export the part after modification.
Importing a Part
When you want to modify a part in the reference library, you need to import the part into your
build area. After the part has been imported, you can use Part Developer to modify the part
as required.
Task Overview
Import the N87C196NT part from the my_reference_library reference library into the
build area.
January 2002
86
Steps
1. To begin the process of importing the N87C196NT part into the build area, you need to
select the part in the reference area. Click Ref tab to display the reference area.
2. Browse the reference area libraries and select the my_reference_library reference
library.
The contents of the my_reference_library appear in the right-pane of the Library
Explorer window.
3. To import the N87C196NT part, right-click on N87C196NT and select Import from the
pop-up menu.
The Library Explorer message box appears. It should report that the import operation
was successful.
Setting Up Part Developer
The settings in the Format tab of Tools > Setup options in Part Developer determines how
the information about a part is interpreted when it is read into Part Developer. It determines
whether the pins that have the suffix * or _N or both are to be interpreted as low asserted pins.
It also determines the format in which different kind of pins, such as scalar, sizeable, and
vector, are shown when a saved part is read in Part Developer. Therefore, it is necessary to
ensure that the format options are set up properly for the part that you want to open.
Task Overview
Open the N87C196NT part in Part Developer. Ensure that the pins with suffix * are read in as
low asserted since that is how you had configured Part Developer to represent low asserted
pins while creating the part. Since for the N87C196NT part, the logical pins are all scalar, the
other options in the Format page will have no effect.
January 2002
87
Steps
1. Launch Part Developer by choosing Tools > Part Developer.
2. To verify and set up the values of the Format option before opening the part, click Cancel
in the Create/Open Part dialog box.
The Part Developer Setup Options dialog box appears.
4. Click Format.
The Format page appears.
5. Ensure that under the Reading option, the check box next to the Suffix ‘*’ and Suffix
‘_N’ is selected. This ensures that the pins with the suffix * and _N will be read in as low
asserted pins.
6. Click OK.
Next, you need to open that part.
Opening an Existing Part
Task Overview
Open the N87C196NT part stored in the library named my_library.
Steps
1. Choose File > Open.
The Open Part dialog box appears.
2. Choose my_reference_libs from the Library drop-down list box.
3. Choose N87C196NT from the Cell drop-down list box and click OK.
The part will open in Part Developer.
Next, you will add some logical pins and NC pins to the part.
January 2002
88
Modifying Pins List
Task Overview
Remove the scalar pin P2.2 and add the vector pins ZZ1-ZZ16 to the part. Ensure that the
pins ZZ1-ZZ6 are interpreted as vector pins.
Steps
1. To modify the logical pin list, right-click on the Logical Pins entry in the tree view.
2. Choose Edit Pin List.
The Logical Pins dialog box displays.
3. To modify the pin interpretation, click Edit in the Pin Pattern Interpretation group box.
The Pin Name Interpretation page of the Part Developer Setup Options dialog box
appears.
4. To ensure that the pins ZZ1-ZZ16 are interpreted as bits of a vector pin, select the
BaseName-Bit option.
5. Click OK.
6. Enter ZZ1-ZZ16 in the Pin Name field.
7. Click Add.
The pins ZZ1-ZZ16 will get added to the logical pins list as vector pins. Next, you need
to delete the pin P2.2.
8. Right-click on the pin P2.2.
9. Select Delete.
The P2.2 pin will get deleted from the logical pins list
10. To accept the changes, click OK.
Next, you need to update the package to synchronize it with the modified pin list.
January 2002
89
Modifying Packages
Task Overview
Modify the plcc package to reflect the changes done in the logical pins list. Mark the physical
pin that was associated with the deleted logical pin P2.2 as NC. Also, change the value of the
JEDEC_TYPE property from plcc68 to plcc84.
Steps
1. Right-click on the N87C196NT_PLCC package in the tree view.
2. Choose Properties.
The Package Properties dialog box appears.
3. Since more pins have been added, the value of the JEDEC_TYPE property needs to be
updated.To select a new value for the JEDEC_TYPE property, click Specify Footprint.
The Physical Properties dialog box appears.
4. To modify the value of the JEDEC_TYPE property, click Browse.
The Footprints dialog box appears.
5. From the displayed list of footprints, select plcc84 and click OK.
The value of the JEDEC_TYPE property changes from plcc68 to plcc84
Next, you need to update the physical to logical pin mapping for the package.
6. Click Physical Pin Mapping.
January 2002
90
Notice that the physical pin 43 which was mapped to the logical pin P2.2 is now
unmapped and moved under the physical pins list. You need to mark this pin as NC.
7. To mark the physical pin number 38 as NC, select the NC check box next to the pin.
Next, you need to add the physical pin numbers for the logical pins ZZ1-ZZ16. For this,
you will again extract the physical pins from the footprint.
Note: When you re-extract pin numbers from a footprint for an existing package, then all
the pin numbers present in the package, but not present in the footprint are removed from
the package. The mappings for pin numbers present on the package, and also present
on the footprint are preserved. The rest of the pin numbers on the footprint are added as
unmapped pins.
January 2002
91
8. To extract the physical pin information, click Pin Numbers.
A confirmation box appears.
9. Click Yes.
January 2002
92
The additional pin numbers get extracted from the footprint and added to the physical
pins list.
Next, you need to map the physical pins 69-84 to the logical pins ZZ1-ZZ16.
10. To map the physical pins 69-84 to the logical pins ZZ1-ZZ16, multiselect the physical
pins.
Note: To ease the pin mapping procedure, you can sort the physical pin list by either
clicking on the Numbers column heading in the Physical Pins list or by right-clicking on
the multiselected physical pins and then choosing either the Sort Ascending or Sort
Descending option.
11. Next, multiselect the logical pins ZZ1-ZZ16 and click Map.
January 2002
93
This maps the physical pins 69-84 to the logical pins ZZ1-ZZ16.
12. To accept the changes, click OK.
Next, you need to modify the symbols.
Modifying Symbols
Overview
Modify split symbols, implies one of the following tasks:
1. Creating new symbols.
To create additional symbols, you need to resplit the pins across a larger number of
symbols. For example, if you have two symbols for a part and want to create a third one,
you will need to specify that you need three symbols and resplit the pins across them.
Part Developer provides you with a Symbol Modification Wizard to enable you to resplit
the pins across the symbols.
2. Copying symbols.
You may want to make copies of a symbol to create a flat symbol from a sizeable symbol.
However, for parts with split symbols, you cannot simultaneously have both sizeable and
flat symbols. You can have either a symbol with all the vector pins/sizeable pins
expanded or a symbol with the vector/sizeable pins contracted.
3. Deleting Symbols
When deleting split symbols, one of the following is possible:
❑
Deleting all the symbols.
❑
Decrease the number of symbols by resplitting the pins across a smaller number of
symbols. A Symbol Modification Wizard helps you in effortlessly decreasing the
number of symbols and resplitting the pins across the smaller number of symbols.
4. Adding Logical Pins
If you add pins to the logical pins list, you cannot globally add them to all the symbols.
You need to run the Symbol Modification Wizard to add the logical pins to the required
symbol.
Note: You should map the added logical pins to physical pin numbers in the package
before you run the Symbol Modification Wizard.
January 2002
94
5. Modifying/ Deleting Logical Pins
If you add or delete a logical pin and then try to save the part, it will ask you whether you
want to regenerate the symbols on which the pins have been added or from where the
pins have been deleted. If you choose to regenerate the symbols, they will lose their
existing shape and get saved as rectangular symbols.
Task Overview
Modify the split symbols of the N87C196NT part. Create a third symbol and modify the
existing symbols so as to have the vector pins ZZ1-ZZ16 on sym_1 and the power pins and
NC pin on sym_3.
Steps
1. To begin the process of modifying the split symbols, right-click on any one of the existing
symbols.
2. Select Modify Pin List.
The Split Symbol Modification wizard appears.
3. Since you need to create three symbols, specify the value in the Number of split
symbols field as 3 and click Next.
The second page of the Split Symbol Modification Wizard appears. Notice that the
logical pin P2.2 which was deleted from the logical pins list is automatically deleted from
the symbols. Also, the pin ZZ1-ZZ16 are added to the pin list. Since they are bits of a
vectored pin, there is a single entry ZZ in the matrix corresponding to the vectored pin.
January 2002
95
The pins that are currently present in the symbols sym_1 and sym_2 are checked
appropriately.
4. Modify the pin list to add the pin ZZ to sym_1 and move the power and the NC pins to
the sym_3.
5. Click Next.
The Summary page of the Symbol Modification Wizard appears.
January 2002
96
6. To complete the symbol modification, click Finish.
You successfully modified the symbols and created the third symbol. From sym_1 you
deleted the pin P2.2 and added the vector pin ZZ1-ZZ16. From sym_2, you moved the
power pin to sym_3, and you created the third symbol sym_3 that has the power and the
NC pins.
7. Save the part by choosing File > Save.
A message box appears asking you whether new rectangular symbols should be created
for the modified symbols or whether the existing shape of the symbols should be
preserved. The second option implies that new pins will be added away from the
boundary of the symbol. You will need to manually snap the pins to the symbol boundary
January 2002
97
in Concept HDL. This functionality is provided to enable addition of pins to existing parts
without destroying the symbol graphics.
8. To retain the shape of the symbols, click OK.
January 2002
98
9. Click OK.
Next, you need to view the symbols in Concept-HDL.
10. To view sym_1 in Concept HDL, select sym_1.
11. To launch Concept HDL on sym_1, choose Tools > ConceptHDL.
January 2002
99
Concept HDL launches on sym_1. Notice that the vector pins ZZ1-ZZ16 is added away
from the symbol graphics.
Next, you need to attach the ZZ vector pins to the symbol outline.
12. Click on pin name ZZ <16 1> on the symbol.
The ZZ<16 1> will be surrounded by a rectangle displaying that it has been selected.
13. Next, press Ctrl and click on the dot, the signal and the pin text ZZ <16 1> entries. This
will select all the entries.
January 2002
100
14. Right-click on the selection.
15. Select Group of Objects.
This will group the pin name, dot, signal, and pin text together.
16. Right click on the group, and select Move.
17. Move the selected object to wherever you want to place it on the symbol body and click
once.
You successfully moved the vector pins to the symbol graphics.
18. Close Concept HDL.
Next, you need to ensure the validity of the parts by running the View Verification check
on the part.
19. To run the checks, choose Tools > Verify.
20. Choose View Verification and click OK.
The View Verification check should pass. Next, you will view the bits of the vector pin
ZZ1-Z16.
Viewing the Bits of a Vector Pin
When you add a vector pin, by default, it appears as pin_name<n..1> format in the
symbols. For example, the vector pins ZZ1-Z16 will appear as ZZ<16..1> in the tree view.
However, you can expand the vector pins to view all the bits of the vector pins.
Task Overview
Expand the bits of the ZZ<16..1> of the N87C196NT part.
Steps
1. Expand the sym_1 symbol in the tree view.
2. Right-click on the vector pin ZZ<16..1>
3. Select Expand to Bits.
January 2002
101
The vector pins gets expanded to display all the pins of the vector pin ZZ<16..1>
Summary
In this chapter you learned about the steps involved in modifying a split part. In the next
chapter, you will learn to create a multi-section symmetrical part.
January 2002
102
January 2002
103
6
Creating a Multi-Section Symmetrical
Part
Objective
To become familiar with the methodology and steps involved in creating a multi-section
symmetrical part.
■
Set up Part Developer to apply properties globally to all symbols and packages and
interpret the logical pins in a manner that is most appropriate for the part that is to be
created.
■
Create packages by using the different methods supported in Part Developer.
■
Create symbols.
■
Create a HAS_FIXED_SIZE symbol.
■
Verify the part.
■
Export the part.
Overview
A part in which the pin list that appears in the datasheet (called the logical pin list) is the same
across the packages and sections (or slots) is known as a symmetrical part. The generic
component LS00 (a quadruple 2-input positive-NAND gates symmetrical part) present in the
SN5400, SN54LS00, SN54S00, SN7400, SN74LS00, and SN74S00 components will be
used as an example while detailing the steps to create a symmetrical part. This will be created
in a build library named my_ library. This part has four independent 2-input NAND gates and
January 2002
104
Creating a Multi-Section Symmetrical Part
comes in DIP, SOIC, Ceramic Chip Carrier (CCC) and Ceramic Flat Packages (CFP). The
pinouts for the specific packages are displayed below:
Note: In the diagram displayed above, the following representations are used for the
packages.
J Package
DIP Package
W Package
Ceramic Flat Package (CFP)
N Package
SOIC Package
FK Package
Ceramic Chip Carrier (CCC)
Starting Part Developer
Task Overview
Create the LS00 part in the my_library build library.
Steps
Since the part has to be created in the my_library build library, ensure that my_library is
selected in Library Explorer. To launch Part Developer:
January 2002
105
2. Since you need to set up Part Developer before you create the part, click Cancel.
Setting Up the Part Developer
The first step in creating parts using Part Developer is to set up Part Developer to ensure that
the pin names are interpreted correctly. To know more about pin name interpretations, see
Configuring Pin Name Interpretation on page 57.
Task Overview
LS00 is a four-slot part. The datasheet for LS00 has the pin names in
<Numeral><Alphanumeric> pattern. Therefore, configure Part Developer to interpret the pins
in the Slot-BaseName format.
Steps
2. Click Pin Name Interpretation.
The Pin Name Interpretation property page appears.
January 2002
106
3. Since the pin name is represented in LS00 as <Numeral><Alphanumeric> and the part
has four slots, select the Slot-Base Name option in the Pin Name Interpretation tab
in the Part Developer Setup Options dialog box.
4. Click OK.
The next step is to enter the part properties such as the part name, and the logical pin
information.
Entering Part Properties and Logical Pins Information
Task Overview
Create the LS00 part and enter the part properties and the logical pins for the part. You will
create the SN5400 implementation of LS00.
Steps
1. Choose File > New > Part.
The New Part Properties dialog box appears. You need to specify the properties for the
new part in this dialog box.
2. Select the library name as my_ library.
3. Specify the part name as LS00.
4. Specify the physical part name as SN5400.
5. Specify the part type as IC.
January 2002
107
The completed dialog box should look appear as following:
6. Click OK.
January 2002
108
7. Select the pin type as INPUT.
Note: This is selected by default.
8. Enter the logical pin names for input pins as 1A-4A, 1B-4B.
9. Click Add to add the specified pin names to the logical pin list.
10. Repeat the step 8 and 9 for the different pin types. For LS00, to enter output pins, select
pin type as OUTPUT, enter 1Y-4Y as the pin names, and click Add. Repeat for GND
and VCC pins.
The loaded Logical Pins dialog box for LS00 should appear as following:
11. Click OK to accept the entries of the Logical Pins dialog box.
A Part Developer Warnings message box appears. The warning message states that
when you enter logical pins, they are entered in the slot range 1 to n, but when you
reopen the part, the slot ranges will appear as 0 to n-1. For example, for LS00, the slot
January 2002
109
ranges entered was 1-4. However, after you create the part and reopen it in Part
Developer, the slot ranges will appear as 0 to 3. Therefore, pins 1A-4A will appear as 0A3A and so on.
12. Click OK.
The next step is to create the packages for the part. But, before you create the packages you
will save the information that you have so far entered.
Intermediate Saving of Parts
When you save a part in Part Developer, several pre-save checks are run. So if you try to save
an incomplete part, you might get some warnings and the part will not get saved.
Therefore, to save a work-in-progress part, you should use the intermediate save feature of
Part Developer.
To save the part information in an intermediate save file:
1. Choose File > Intermediate Save.
The Save As dialog box appears.
2. Enter ls00 in the File Name field and press Enter.
You successfully saved the part in an intermediate file.
Creating Packages
Task Overview
Create the packages for the LS00 part.
January 2002
110
Steps
1. Choose File > New > Package.
The New Package dialog box appears. The General tab is selected by default.
Note: Alternately, the New Package dialog box can be displayed by the RMB menu
option on a “Packages” tree item.
2. Select the Specify Package Type field.
3. Enter the package type as DIP.
4. Enter the equivalent packages, as CFP and click Add.
5. To enter the value for the JEDEC_TYPE property, click Specify Footprint.
The Physical Properties dialog box displays.
6. Click Browse.
January 2002
111
The Footprints dialog box appears. The footprints are displayed from the
<your_intall_dir>/share/pcb/pcb_lib. The footprint information itself is
contained in the *.dra and *.psm files.
7. Select dip14_3 as the JEDEC_TYPE value.
8. Click OK.
9. Click OK.
You entered the value for the JEDEC_TYPE property. Next, you need to update the
BODY_NAME property.
Tip
You can also enter your own footprint information. This can be done either by
manually typing in the value of the JEDEC_TYPE property or by updating the
environment variable PSMPATH, or by adding new directories which Part Developer
will scan for displaying the footprints. The environment variable PSMPATH stores the
path to the footprint files. To set up the PSMPATH environment variable:
a. Click Allegro Setup.
The User Preferences Editor dialog box appears.
January 2002
112
b. Click the Design_paths entry in the Categories list.
c. Click the browse button (the button with three dots) next to the psmpath entry under
Preference.
The Physical Paths dialog box appears. You can set up your preferences for location of
footprints in this dialog box. You can see the current value of the PSMPATH environment
variable by selecting the Expand check box.
a. To add new footprints, click on the New button. It is the button with a dotted outline.
A new blank line is added with a browse button.
b. Browse and select the footprints directory in the tutorial_project_data directory.
c. Click OK.
January 2002
113
The new footprints are added.
a. Click OK.
b. Click OK again to close the Allegro Setup dialog box.
c. To verify, click Browse button in the Physical Properties dialog box.
January 2002
114
The Footprints dialog box appears. Notice that the first entry in the footprints list is
plcc84. This entry is coming from the plcc84.dra file located in the
c:\tutorial_project_data\footprints directory.
Footprint information from
c:\tutorial_project_data\foot
print location
10. Click on the value column of the BODY_NAME property in the Additional Properties
section.
11. Enter LS00 and click on the Physical Pin Mapping tab.
January 2002
115
The Physical Pin Mappings page appears. This page enables you to add physical pins
and map them to the logical pins.
.
12. To get the physical pin list from the footprint, ensure that the Extract from Footprint is
selected, and click Pin Numbers.
A message box appears informing you that all pin numbers extracted from the footprint
will be added as unmapped pins to the package.
13. Click OK.
This lists all the extracted physical pins under the Physical Pins list in the Physical Pin
Mapping property sheet.
January 2002
116
Note that the Physical Pins list is not sorted. To sort it on numeric order, click the
Number column heading.
Next, you need to map the physical pins to the logical pins.
14. As per the datasheet, physical pin 1 is mapped to the logical pin 1A. Therefore, select
1A in the Logical Pins list and 1 in the Physical Pins list and click Map.
January 2002
117
This maps the physical pin 1 to the logical pin 1A. Similarly, map the other logical pins to
the respective physical pins. After the mappings, the Physical Pin Mapping sheet
should appear as following:
15. Click OK to complete the creation of the package.
Next, you need to create the CCC package.
January 2002
118
Creating Multiple Packages
Using Part Developer, you can easily and quickly create multiple packages. You can make
copies of an existing package and then make the necessary changes to quickly get the new
packages.
Task Overview
Create the CCC package for the LS00 part.
Steps
1. Right-click on the SN5400_DIP package in the tree view.
2. Select Copy.
3. Right-click on the Packages entry in the tree view.
4. Select Paste.
A copy of the SN5400_DIP package gets created with the name SN5400_DIP[1]. You
need to modify the properties of this package to create the CFP package.
5. Right-click on the SN5400_DIP[1] entry in the tree view.
6. Select Properties.
The Package Properties dialog box appears. You need to make the following changes
to the current information:
❑
Package Type name
❑
JEDEC_TYPE value
❑
Physical Pin Mappings
First, you will change the package type value.
7. Change the Package Type value from DIP[1] to CCC.
Next, since the CFP package has 20 pins, you need to change the value of the
JEDEC_TYPE property from dip14_3 to dip20.
8. To change the footprint information, click Specify Footprint.
January 2002
119
9. Click Browse.
10. Select dip20 and click OK.
11. Click OK.
Next, you need to update the pin mappings.
12. To update the pin mappings, click Physical Pin Mapping.
The Physical Pin Mapping property page appears. The DIP package has 14 pins.
However, the CCC package has 20 pins. Therefore you need to add the additional 6 pins.
You can either add the pins manually or extract it from the footprint.
13. To extract the pin list from footprint, ensure that the Extract from Footprint option is
selected and click Pin Numbers.
A message box appears informing that all the pin numbers present in the package, but
not present on the footprint, will be removed from the package. The mappings for pin
numbers present on the package, and also present on the footprint, will be preserved.
Rest of the pin numbers on the footprint will be added as unmapped pins.
14. Click Yes.
The added pin numbers get added to the Physical Pins list. Next, you need to modify
the pin list for the CFP. Modification of pin list involves unmapping and remapping the
changed pins.
15. To unmap the pins, click Unmap All.
16. Click Yes.
The physical pins get unmapped and move back to the Physical Pins list. Next, you
need to map the physical pins to the logical pins as per the datasheet.
17. Physical pin 1 is marked as NC in the datasheet. To mark it as NC in Part Developer, click
the NC check box next to physical pin 1 in the Physical Pins list.
January 2002
120
18. Map the physical pin 2 to logical pin 1A.
19. Similarly, map the physical pins to the logical pins as per the datasheet.
The completed pin mappings should appear as following:
20. After you complete the mappings, click OK.
You successfully created the CFP package for the LS00 part. After you create the packages
for a part, you need to create the symbols for the part.
January 2002
121
Creating Symbols
To enable you to create symbols effectively, Part Developer provides a Symbol Creation
Wizard. The Symbol Creation Wizard guides you through the process of creating symbols.
Task Overview
Create symbols for the LS00 part.
Steps
1. Choose File > New > Symbols.
The Power/NC Pin Selection page of the Symbol Creation Wizard appears. The
Symbol Creation Wizard detects that one package has NC pins whereas the other
package does not. The Wizard asks you to determine whether you want to put the power
and NC pins on them. In case you choose to do so, you will need to specify the package
group on which you want to base your symbol.
January 2002
122
A package group is a collection of packages which have the same logical to physical pin
mappings. In this example, you will put the power and the NC pins on the symbol.
2. Choose Yes.
3. Click Next.
January 2002
123
The Package Selection page of the Symbol Creation Wizard appears. In this page
you need to determine on which package group you want to base the symbols.
4. To base the symbol on the SN5400_CCC package, choose SN5400_CCC.
5. Click Next.
January 2002
124
The Symbol Kinds page of the Symbol Creation Wizard appears.
6. To create a symbol with logical pins and a symbol with logical and NC pins, check the
Logical and Logical + NC check boxes.
Note: Notice that there are options in the Symbol Kinds page that are separated by
either by commas or a + sign. The difference between the two types is that if you select
an option with comma, then two different symbols are created. For example, if you select
the Logical, NC check box, then two symbols, one with logical pins and another with NC
pins gets created. If you select an option with the + sign, then only one symbol gets
created. For example, if you select the Logical +Power option, then only one symbol
with both logical pins and power pins gets created.
7. Click Next.
January 2002
125
The Package Types page of the Symbol Creation Wizard appears.
Important
The Package Types page enables you to specify the package type for the symbols
that you are creating. Depending on the symbols that you have chosen to create,
you may face a situation where the logical pin list in the package is not the same as
the logical pin list of the symbol.
For example, for a symbol to contain NC pins (Logical + NC in our case), there must be
a package which contains the NC pins as logical pins. This implies that there should be
a primitive in the chips.prt file which should have the NC pins in its pin section.
However, when you create packages, Part Developer always puts all the power and NC
pins in the body section. Therefore to have Power/NC pins as logical pins, you need to
explicitly move the Power/NC pins upto the pin section.
The Symbol Wizard solves this requirement by letting you create new packages which
contain the Power/NC pins in the pin section. The information from existing packages is
January 2002
126
used to create the new packages. You may choose to follow certain conventions while
naming your packages, such as L_NC for logical+NC pins on the symbol.
8. To create the corresponding packages, for the Logical + NC symbol, specify the package
type as L_NC and the Source Package as CCC.
9. Choose Next.
This displays the Summary page. Check the summary to ensure its correctness.
10. Choose Finish to create the symbols.
By default, when you create symbols for a symmetrical part, the symbol is created for
only one section or slot. For LS00, the Symbol Wizard will create a symbol which will
represent only one section of the four possible sections. However, Part Developer
provides the ability to create symbols which represent more than one section. Such
symbols are called HAS_FIXED_SIZE symbols. Next, you will make a copy of a symbol
and make it a HAS_FIXED_SIZE symbol.
January 2002
127
Copying Symbols
Task Overview
Make a copy of the symbol sym_1.
Steps
1. Right-click on the symbol sym_1 in the tree view.
2. Select Copy.
3. Right-click on the Symbols in the tree view.
4. Select Paste.
A new symbol sym_3 is created in the tree view. This symbol is a copy of the symbol
sym_1.
Next, you will make this symbol a flat symbol.
Creating HAS_FIXED_SIZE Symbols
Normally when you create a multi-section symmetrical part, only one of the section is
displayed in the symbol. For example, for LS00, only one section containing the logical pins
A, B and Y is displayed in the symbol. However, you may need to create symbols that show
more than one section. You can create such parts by modifying the HAS_FIXED_SIZE
property of a symbol. Such symbols are called HAS_FIXED_SIZE symbol.
Task Overview
Display all the four sections of LS00 in sym_3 by make the symbol sym_3 a
HAS_FIXED_SIZE symbol.
Steps
1. Right-click on sym_3 in the tree view.
2. Select Fixed Size.
January 2002
128
The Fixed Size Symbol dialog box appears.
3. To make this symbol represent all the four sections of LS00, change the Size entry to 4.
4. Click OK.
You successfully created a HAS_FIXED_SIZE symbol.
After you complete creating the symbols, you should verify the part to ensure that it us
usable and then export it to the reference area. See Verifying Parts on page 76 and
Exporting Parts to the Reference Area on page 83 for details.
Summary
In this chapter you learned about the methodology and steps involved in creating a multisection symmetrical part. In the next chapter you will learn to modify the part that you created
in this chapter.
January 2002
129
7
Modifying Multi-Section Symmetrical
Parts
Objective
To become familiar with the methodology and steps involved in modifying a multi-section
symmetrical part.
■
Import a part from the reference library.
■
Set up Part Developer to view the part data as you had entered it.
■
Delete a package.
■
Delete a symbol.
■
Add a logical pin.
■
Delete a power pin.
■
Modify the packages.
■
Modify the symbols.
■
Verify the part.
■
Export the part.
Importing a Part
When you want to modify a part in the reference library, you need to import the part into your
build area. After the part has been imported, you can use Part Developer to modify the part
as required. For details, see Importing a Part on page 86.
January 2002
130
After you import the part into the build area, you open it in Part Developer and make the
necessary changes.
Launching Part Developer
2. Since you need to set up Part Developer before you create the part, click Cancel.
Setting Up the Part Developer
LS00 is a four-slot part. The datasheet for LS00 has the pin names in
<Numeral><Alphanumeric> pattern. When creating the part, you had configured the pins to
be interpreted as Slot-BaseName format. Therefore, when reading the part, you should
ensure that the pins are interpreted in the Slot-BaseName format.
Task Overview
Setup Part Developer to interpret the pins in the Slot Number - Base Name format.
Steps
January 2002
131
2. Select the Slot Number - Base Name option.
3. Click OK.
You setup Part Developer to read pins of LS00 in Slot-BaseName format. This is the
same format in which you had entered the pin names whine creating the part. Next, you
will modify the pin list.
Modifying Pin List
Task Overview
Add a scalar pin Z to the part. Also, delete the power pin GND from the part.
January 2002
132
Steps
1. Right-click on the Logical Pins entry in the tree view.
2. Select Edit Pin List.
3. Enter Z in the Pin Name field.
4. Click Add.
5. To complete the process, click OK.
Next, you need to delete the power pin GND.
January 2002
133
6. Expand the Logical Pins entry in the tree view.
7. Right-click on the GND entry in the tree view.
8. Select Delete.
You successfully deleted the GND power pin from the part. Next, you need to modify the
packages and the symbols to reflect that changes in the pin list.
Deleting Packages
Task Overview
Delete the SN5400_L_NC package.
Steps
1. Right-click the SN5400_L_NC package in the tree view.
2. Select Delete.
The SN5400_L_NC package is deleted from the LS00 part. Next, you will delete a
symbol of the LS00 part.
Deleting Symbols
Task Overview
Delete the symbol sym_2.
Steps
1. Right-click on the symbol sym_2 in the tree view.
2. Select Delete.
The sym_2 symbol of ls00 part is deleted. Next, you will modify the remaining packages
to add the scalar pin Z.
January 2002
134
Modifying Packages
Task Overview
Modify the DIP, CFP packages of the LS00 part.
Steps
1. Right-click on the SN5400_DIP entry in the tree view.
January 2002
135
The Physical Pin Mapping property page appears. Note that the power pin GND is
removed from the logical pins list and the physical pin that was mapped to it is moved
back to the Physical Pins list.
4. Map the physical pin 7 to the logical pin Z.
5. Click OK.
You successfully updated the DIP package. Similarly update the CFP package. After you
modify the packages, you need to updates the symbols.
January 2002
136
Modifying Symbols
Task Overview
You added a scalar pin Z and remove the power pin GND from the part. Modify the symbol to
reflect the changes.
Steps
First, you will add the scalar pin to all the symbols. To enable you quickly add a logical pin to
all symbols in a sizeable part, do the following:
1. Right-click on the Symbol entry in the tree view.
2. Select Add Logical Pins.
The Add Logical Pins dialog box appears. It displays the logical pin that you can add
to all the symbols.
3. Select the pin Z and click OK.
The logical pin Z gets added to all the symbols of the LS00 part.
4. Save the part by choosing File > Save.
January 2002
137
in Concept-HDL. This functionality is provided to enable addition of pins to existing parts
without destroying the symbol graphics. See Modifying Symbols on page 94 for details.
5. To regenerate the symbols, select all the two symbols and click OK.
January 2002
138
6. Click OK.
After you modify the symbols, you should verify that the part is error free.
7. To verify the part, select Tools > Verify.
8. Choose View Verification and click OK.
The View Verification check should pass.
Summary
In this chapter, you learned the methodology and steps involved in modifying a multi-section
symmetrical part. In the next chapter, you will learn to create an asymmetrical part.
January 2002
139
8
Creating Asymmetrical Parts
Objective
To become familiar with the methodology and the steps involved in creating an asymmetrical
part.
■
Understand the definition of an asymmetrical part.
■
Understand the methodology involved in creating asymmetrical parts.
■
Manually enter the physical pin information.
■
Create multiple packages.
■
Create multiple symbols.
■
Verify parts.
■
Export a part into the reference area.
Overview
When creating parts, you may come across parts in which the logical pin lists across
packages or slots are different. These are called asymmetrical parts. LS241 is such an
asymmetrical part.
January 2002
140
■
Different logical pin list across slots: Consider the part LS241. The pins appear in the
datasheet as follows:
As displayed, LS241 is an 8-slot part with a low asserted enable signal (G*) and a high
asserted enable signal (G). The high asserted enable signal G is present in four slots and
low asserted enable signal G* is present in the remaining four. This divides the part into
two groups. The first group has G as the enable pin and the second group has G* as the
enable pin. Because the functionality of each section in a group is the same and because
January 2002
141
of the different assertion signals across the sections, the logical pin list across the section
or slots are different. The pin entries created will be as follows:
DIfferent pin
list across
slots
Notice that the pin number G is present in the first four slots and not in the next four. The
slots in which G is not present have 0 as pin numbers.
In this chapter, you will learn to create an asymmetrical part where the asymmetry arises due
to different pin list across slots.
January 2002
142
Create the LS241 part. It is an eight slot part with two slot groups, one with low asserted
enable signal 1G* and the other with high asserted enable signal 2G. This part comes in DIP,
SOIC and CFP packages. The diagram of the LS241 part is displayed below.
.
Entering Part Properties
1. Choose File > New > Part.
The New Part Properties dialog box appears.
2. Select my_library from the Library Name drop-down list box.
3. Enter LS241 in the Part Name field.
Note: The Physical Part Name field also gets filled in automatically as you enter the a
part name field. This field is used as the PART_NAME property in the chips.prt file.
4. Click OK.
The Logical Pins dialog box appears. Next, you need to configure the pin name
interpretation for the logical pins.
January 2002
143
Configuring Pin Name Interpretation
Need for Configuring Pin Name Interpretation
As displayed, the LS241 component is an eight slot part with two slot groups, one with low
asserted enable signal 1G* and the other with high asserted enable signal 2G. In the
datasheet the pins are present in <Numeral><Alphanumeric String><Numeral> format such
as 1A1, 1A2 and in <Numeral><Alphanumeric String> format such as 1G* and 2G. Here the
leading numeral represents the group, the alphanumeric string represents the base name
and the trailing numeral represents the slot number. Therefore the pins need to be interpreted
as Group-Base Name-Slot and Group-Base Name respectively.
Alternately, you can also enter the pins in the BaseName-Slot format, that is, as A1-A8, B1B8 etc. See Alternate Method of Creating an Asymmetrical Part on page 162 for details.
Task Overview
Configure the pin interpretation to interpret <Numeral><Alphanumeric><Numeral> pins as
Group-BaseName-Slot and <Numeral><Alphanumeric> as Group-BaseName.
Steps
1. Click Edit in the Pin Name Interpretation group box in the Logical Pins dialog box.
January 2002
144
The Pin Name Interpretation tab of the Part Developer Setup Options dialog box
appears.
January 2002
145
2. Select Group-Base Name [G-BN] and Group-Base Name-Slot [G-BN-S].
3. Click OK.
You successfully setup Part Developer to interpret pins as Group-BaseName-Slot and
Group-Base Name. Next, you need to enter the logical pins as they appear in the
datasheet.
Entering Logical Pins
Task Overview
Enter the pin information as displayed in the diagram into Part Developer. The pins will be
entered in the same sequence as they appear in the diagram.
January 2002
146
Steps
1. Select INPUT from the Pin Type as Input.
2. Enter 1A1-1A4, 2A1-2A4 in the Pin Name text box.
3. Click Add.
4. Enter 1G in the Pin Name text box.
5. Click Add.
6. Enter 2G in the Pin Name text box.
7. Select the Active Low check box.
8. Click Add.
January 2002
147
9. Similarly, add the 1Y1-1Y4, 2Y1-2Y4 as the output pins and VCC and GND as the power
pins.
The filled up Logical Pins dialog box for LS241 part is displayed below:
10. To accept the entries and close the Logical Pins dialog box, click OK.
After the logical pins have been entered, you need to create the packages.
January 2002
148
Creating Packages
Task Overview
Create the DIP package for the LS241 part. Modify the value of the BODY_NAME property
to LS241. The logical to physical pin mappings are as following:
Steps
1. To begin the process of creating packages, choose File > New >Package.
The New Package dialog box appears. By default, the General tab is selected.
2. Enter DIP in the Specify Package Type field.
3. To update the value for the JEDEC_TYPE property, click Specify Footprint.
January 2002
149
The Physical Property dialog box appears. You need to specify the value of the
JEDEC_TYPE property for the package. The value for the JEDEC_TYPE property will
be picked up from the Allegro footprints of standard packages provided by Cadence.
4. To select the appropriate JEDEC_TYPE, click Browse.
The Footprints dialog box appears. This has the complete list of footprints supplied by
Cadence.
5. Select dip20.
6. Click OK.
7. Next, click in the Value column next to the ALT_SYMBOLS property.
8. Click Browse.
9. Select dip20_3.
10. Click OK.
You selected the value for the JEDEC_TYPE and ALT_SYMBOLS properties.
11. To specify the value for the BODY_NAME property, enter LS241 as the value.
12. Next, you need to enter the physical pins and map them to the logical pins that you
entered earlier. To get to the page where you enter physical pins, click the Physical Pin
Mapping tab.
You can either add the physical pins manually, or extract them from the footprint.
Extracting the pins from footprint is useful when you are dealing with large pin count
parts. For this example, you will add the pins manually.
January 2002
150
13. To add the pins manually, select the Add Manually option.
The Add Physical Pin Numbers dialog box appears. You add the physical pin numbers
through this dialog box.
15. Since the part has 20 pins, enter 1-20 in the Numeric field and click OK.
January 2002
151
The physical pins get added to the Physical Pins list in the New Package dialog box.
Next, the physical pins need to be mapped to the logical pins. The general method to
map a physical pin with logical pin is to select both the pins and click on the Map button.
16. As per the datasheet, physical pin 1 is mapped to logical pin 1G. Therefore, select 1 in
the Physical Pins list, and select 1G in the Logical Pins list.
17. To map the selected pins, click Map.
The physical pin 1 is mapped to the logical pin1G
Note: Whenever you map a physical pin to a logical pin.The pin number moves from the
Physical Pins list to the Logical Pins list and the next pin number in the list gets selected
in the Physical Pins list. This eases the pin mapping effort as you do not need to explicitly
January 2002
152
select a physical pin to map to a logical pin. You can simple select the logical pin that you want
the automatically selected physical pin to be mapped to, and map it.
18. To map pin number 2 to logical pin 1A1, select 1A1 in the Logical Pins list.
19. Click Map.
Similarly, map the remaining pins.
January 2002
153
After the mappings are done, the New Package dialog box should appear as displayed
below.
20. Click OK to complete the process of creating the DIP package.
January 2002
154
Creating Multiple Packages
Task Overview
Create the CCC package for LS241. The package information is displayed below:
You can create multiple packages in two ways:
■
By creating a fresh package.
■
By making a copy of an existing package and then making the necessary changes. This
method helps you save time while making multiple packages for a part. For this example,
you will make a copy of the DIP package and then make the necessary changes for the
CCC package.
Steps
1. Right-click on the LS241_DIP package in the tree view.
2. Select Copy.
3. Right-click on Packages.
4. Select Paste.
January 2002
155
A copy of the LS241_DIP is made with the name as LS241_DIP[1]. You need to change
the properties of this package.
5. Right-click on LS241_DIP[1].
7. Enter CCC in the Specify Package Type field.
8. To specify the correct footprint for CCC type package, click Specify Footprint.
9. To display the list of available footprints in Allegro, click Browse.
The Footprints dialog box displays.
10. Select flat20 and click OK.
11. Since there are no alternate symbols for the CCC package, remove the value for the
ALT_SYMBOLS property.
January 2002
156
12. Click OK.
Next, you need to change the logical to physical pin mapping information for the CCC
package.
13. Click the Physical Pin Mapping tab.
The Physical Pin Mapping tab page appears. This page displays the current logical to
physical pin mappings. You need to update the mapping information for the CCC
package.
Notice that there is no difference in the pin mappings between the DIP and the CCC
package, therefore there is no need to make any changes in the Physical Pin Mapping
property page.
14. To complete the creation of the CCC package for LS241, click OK.
After you create the packages, the next step is to create symbols for the part.
Creating Symbols
Part Developer provides a powerful Symbol Creation Wizard which enables you to quickly
and efficiently create symbols for a part.
Task Overview
Create symbols for the part.
Steps:
1. To begin creating the symbols, select File > New > Symbol.
The Select Sections page of the Symbol Creation Wizard appears. This page
informs you that there are two groups which exist for the packages. You need to
January 2002
157
determine the groups for which you want to create the symbols. You can select either one
of the groups or both. You will create a symbol based on both the slot groups.
2. Click Select All and click Next.
The Symbol Kinds page of the Symbol Creation Page appears. In this page you can
determine the types of symbols you want for the part. For this example, you will create
the following symbols:
❑
A symbol with only logical pins
January 2002
158
❑
A symbol with logical and power pins
3. Note that, by default the Logical option is selected. This will create the symbol with only
logical pins. To create the symbol with both logical and power pins, select the
Logical+Power option and click Next.
The Package Types page of the Symbol Creation Page appears. This page displays
the symbols that you want to make and the packages that correspond to the symbols.
You will notice that the value of the Package Type field next to the Logical symbol is
filled with the DIP,CCC values whereas next to the Logical + Power symbol, the value
of the Package Type field is empty.
This happens because when you create a package using Part Developer, the power and
NC pins are always put in the body section of the chips.prt file. However, when you
want a symbol to show the power and/or NC symbol, the power/NC pins must
necessarily be in the pin section of the chips.prt file. Since currently there are no
January 2002
159
packages that have the power/NC pins on the pin section, the value of the Package
Type next to the Logical + Power symbol appears blank.
To enable the creation of a symbol which can display both the logical and power/NC pins
on the symbol, you need to create a new package that will have the logical as well as the
power/NC pins on the pin section. You can do this by entering a package name in the
Package Type field next to the Logical + Power symbol and specify a source package
from which this package will be created. When you specify the source package, Part
Developer uses the information from the source package and creates the section for the
package in the chips.prt file.
4. Enter lp in the Package Type field next to the Logical + Power symbol entry.
5. Select DIP as the source package and click Next.
January 2002
160
The Summary page of the Symbol Creation Wizard appears. Notice that four symbols
will be created. This is because Symbol Wizard creates one symbol for each of the slot
groups in the part.
6. To complete the process of creating the symbols, click Finish.
Saving Parts
Task Overview
Save the LS241 part.
January 2002
161
Steps
➤
To save the part, choose File > Save.
Verifying Parts
The parts that you created should be error free and usable in the design flow. Part Developer
provides you with robust verification tools which ensure that the parts are correct and usable.
Task Overview
Verify the LS241 part for errors across the different views.
Steps:
1. To begin the process of verifying the part, choose Tools > Verify.
2. To do the verification of the stand-alone views and cross check view, select the View
Verification option.
3. Click OK.
The Verification Results dialog box appears. The verification should not report any
errors.
Congratulations. You have successfully created the LS241 part.
After you create a part and verify it, you should export the part into the reference area and
then delete it from the Build area. See Exporting Parts to the Reference Area on page 83 for
details.
Alternate Method of Creating an Asymmetrical Part
In parts such as LS241, if you choose to use the BaseName-Slot notation for entering the
logical pins then there has to be a mechanism to determine to which slot groups do the scalar
pins G and G* belong. This ability is provided by the Expand to Slots function. To do so:
1. Setup Part Developer (Tools > Options > Pin Name Interpretation) to interpret
<Alphanumeric String><Numeral> logical pins as BaseName-Slot.
January 2002
162
2. Enter the logical pins, as A1-A8, B1-B8, Y1-Y8, G, and G*.
Note: Note the difference in the logical pin naming. If you had chosen the GroupBaseName-Slot interpretation instead of the BaseName-Slot interpretation, the pins
would have been entered as 1A1-1A4, 2A1-2A4, 1B1-1B4, 2B1-2B4, 1Y1-1Y4, 2Y1-2Y4,
1G and 2G*.
3. Create a new package.
4. Enter/extract the required physical pins.
5. Associate the logical pins to the physical pins except G and G*.
6. Right-click on G.
7. Select Expand to slots.
This will expand the scalar pin G across all the slots in the part. For LS241, the scalar
pin G will get expanded to all the eight slots, G<1>..G<8>.
Similarly, expand the other scalar pin G*.
8. Since G is common across the first four slots, map the physical pin 1 to G<1>..G<4>.
Leave the remaining slots empty.
Similarly, map the physical pin 19 to the G*<5>..G*<8> slots.
9. To complete the process, click OK.
After you create the packages, the remaining steps in creating an asymmetrical parts are the
same as described in the example before.
Summary
In this chapter you become familiar with the methodology and steps involved in creating
asymmetrical parts. In the next chapter, you will learn to modify the part that you created in
this chapter.
January 2002
163
9
Objective
To become familiar with the methodologies and steps involved in modifying asymmetrical
parts.
■
Import a part from the reference library.
■
Set up part developer to read-in asymmetrical parts as they were entered.
■
Add logical pins.
■
Modify the packages.
■
Modify the symbols.
■
Add package pin properties.
■
Add symbol pin properties.
■
Change the blank pin spacings for a symbol pin.
■
Verify the part.
Overview
In this chapter, you will import the LS241 part into the build area and modify it.
Importing a Part
The first step in modifying a part in a reference area is to import it into the build area. To see
the steps, see Importing a Part on page 86.
After you import the part, open the part in Part Developer to modify it.
January 2002
164
Setting up Part Developer
Before opening a part, you should configure Part Developer to ensure that the part is read in
correctly. The Format tab is divided into two group boxes:
■
Low Asserted Pin Syntax.
The setting in this group box determines the pin names that Part Developer will treat as
low asserted while reading a part. You also specify the notation that Part Developer
should use to write a low asserted pin into the symbol and the chips.prt file. You have
the following options:
❑
Either with a asterisk (*) or _N suffix: In this case any pin which has either a * or _N
as a suffix in its name is read as a low asserted pin. You can then determine whether
you want to write the low asserted pin into the symbol file with either the '*' or '_N'
suffix.
❑
With a star (*) notation: In this case, the pins with a * suffixed in their names are read
as a low asserted pin. The pin is written back to the symbol file with the *.
❑
With a _N notation: In this case, the pins with _N as suffix are read in a low asserted
pin. They are written into the symbol file with the _N notation.
Note: Select the Use minus [-] sign for low asserted pins in Package
view to ensure that the pins that are considered low asserted are written into the
chips.prt file prefixed with a minus [-] sign. If you leave this unchecked, then the low
asserted pins are written into the chips.prt file with the same notation as they were
written into the symbol.css file.
■
Chips File Reading Options
The options in this group box determines how Part Developer reads the chips.prt file
for displaying the following:
❑
Asymmetrical parts
Asymmetrical parts have multiple slots which have different functionality.
Corresponding to each functionality, there is a pin list. All sections or slots that have
the same functionality have the same pin list. The slots that have the same
functionality form one group. You can choose to display the pin numbers in such a
way that the group numbers are also visible. You can do this by selecting the Use
group format for reading asymmetrical parts check box.
January 2002
165
If this option is checked, you can see the groups to which each of the pin in a package
belongs. For example, displayed below is the expanded pin list of the SOIC package of
the LS241 part, where the group format is used to read the asymmetrical part.
Group Number
January 2002
166
The same part is displayed again. This time, the group format has not been used to read
the asymmetrical parts (the Slot-Base Name format has been used). Notice that the
group information is not displayed in the expanded package pin list.
f
Slot Number
❑
Sizeable pins
Sizeable pins can be displayed in Part Developer in one of the following ways: Slot
Number-Base Name or Base Name - Slot Number.
In the Slot Number - Base Name format, the numeric part is the slot number while
the alphanumeric string part is the base name. For example, if a pin A is present in
slots 1,2,3,4, it will be displayed as 1A, 2A,3A,4A.
January 2002
167
In the Base Name- Slot Number format, the alphanumeric string part is base name
and numeric part is treated as a slot number. For example, if a pin A is present in
slots 1,2,3,4, it will be displayed as A1, A2,A3,A4.
❑
Vector pins
Vector pins can be displayed in Part Developer in one of the following ways: Bit
Number - Base Name or Base Name - Bit Number. In the Bit Number - Base Name
format, the numeric part is the bit number while the alphanumeric string part is the
base name. For example, if a vector pin A has two bits, it is displayed as A<Size
2..0>.
In the Base Name - Bit Number format, the alphanumeric string part is the base
name and the numeric part is the bit.
For reading in the LS241 part, ensure that the Use group format for reading asymmetrical
parts is selected. This is required because you had used the group format while creating the
part.
Task Overview
Set up Part Developer to read in the LS241 part in the same format as you had created it.
Steps
1. Launch Part Developer.
2. Select Tools > Options.
3. Click Format.
The Format property page appears.
4. Ensure that the following options are selected:
❑
In the Low Asserted Pin Syntax group box, Suffix ‘*’ and Suffix ‘_N’ is selected.
This will ensure that the pins in the symbol file which have either * or _N as the suffix
are read in as low asserted pin.
❑
Use minus [‘-’] for low asserted pins in Package view is selected. This will
ensure that the low asserted pins are written back into the chips file with the ‘-’ sign.
❑
Use group format for reading asymmetrical parts is selected. This ensures that
the part is loaded with the group information.
January 2002
168
5. Click OK.
Next, you need to open the part to modify it.
Opening the Part
Task Overview
Open the LS241 part.
Steps
1. Select File > Open
The Open Part dialog box appears.
2. Select my_reference_libs from the Library drop-down list.
3. Select ls241 from the Cell drop-down list.
4. Click OK.
The LS241 part launches in Part Developer. Next, you will add a logical pin to the part.
Modifying Logical Pin List
Task Overview
Add logical pins 1K and 2K to the LS241 part.
Steps
1. To add the logical pins 1K and 2K to the LS241 part, right-click on the Logical Pins entry
in the tree view.
2. Select Edit Pin List.
3. Enter 1K, 2K in the Pin Name field.
January 2002
169
4. Click Add.
5. Click OK.
This adds the logical pins 1K and 2K to the logical pins list. Next, you need to update the
packages and symbols to reflect this change.
Modifying Packages
Task Overview
Update the packages to add the new logical pin. Also add a property my_prop with the value
ABCD to the packages. Updating the packages involves the following tasks:
■
Adding the physical pins for the new logical pins
■
Mapping the physical pins to the new logical pins
■
Updating the footprint information, i.e. the JEDEC_TYPE and ALT_SYMBOL values.
■
Adding the additional properties
■
Saving the packages
Note: Although in this section you will be adding the physical pins manually and then
updating the value for the JEDEC_TYPE property, it is not the recommended way. This style
is covered only to show the possible ways in which you can use Part Developer. The
recommended way to modify packages is to first update the value of the JEDEC_TYPE
property, then extract the footprint information and change the pin mappings if required.
Steps
1. Right-click on the LS241_DIP package in the tree view.
January 2002
170
The Physical Pin Mapping property page appears. Note that the logical pins 1K and
2K appear in the Logical Pins list.
Next, you need to add the physical pins for the added logical pins.
4. To manually add the pins, select the Add Manually option.
January 2002
171
The Add Physical Pin Numbers dialog box appears. Since the package already
contains 20 pins, you need to add 2 more pins for the additional two logical pins.
6. Enter 21-22 in the Numeric field.
7. Click OK.
January 2002
172
The physical pins get added to the Physical Pins list.
Next, you need to map the physical pins to the logical pins.
8. To map the logical pin 1K to the physical pin 21, select the pins and click Map.
9. Similarly, map logical pin 2K to physical pin 22.
Next, you need to update the value of the JEDEC_TYPE property for the package.
10. Click General.
The General property page appears.
11. Click Specify Footprint.
January 2002
173
12. To update the JEDEC_TYPE property value, click Browse.
13. Select dip22_3 and click OK.
Next, you need to update the ALT_SYMBOLS value.
14. Click on ALT_SYMBOLS.
15. Click Browse.
16. Select dip22_4 and click OK.
17. Click OK.
You successfully modified the footprint information. Next, you need to add the my_prop
property to the package and add ABCD as its value.
18. Double-click in the blank cell under the BODY_NAME property in the Additional
Properties section.
19. Enter my_prop and click on the column under Value.
20. Enter ABCD as the value.
21. To complete the process of updating the package, click OK.
You successfully updated the DIP package of the LS241 part. Similarly update the other
packages. After you update the packages, you need to update the symbols.
Updating Symbols
Task Overview
Update the symbols to add the new logical pins to the symbol drawing.
Steps
For asymmetrical parts, you need to update the symbols individually.
1. To update sym_1, right-click on the sym_1 entry in the tree view.
January 2002
174
2. Select Modify Pin List.
The Symbol Modification Wizard appears.
This page informs you that the selected symbol is based in the DIP, CCC packages and
asks you whether you want change the package association for the symbol. By default,
No is selected.
3. Since you do not need to change the package association, click Next.
January 2002
175
The next page of the Symbol Modification Wizard appears.
This page displays the different slot groups that exist for the package. You need to
determine the slot group on which you want to base the symbol.
4. To update the symbol for the first slot group, select Groups 1 and click Next.
January 2002
176
The Summary page appears.
The Summary page displays the pins that will be visible in sym_1 and the package the
symbol is associated with.
5. Click Finish to complete the process of updating the symbol.
Similarly update the other symbols for the part. After you update the packages and the
symbol, you need to save the part.
Saving Modified Part
Task Overview
Save the modified LS241 part.
January 2002
177
Steps
1. Choose File > Save.
in Concept-HDL. This functionality is provided to enable addition of pins to existing parts
without destroying the symbol graphics.
2. To regenerate symbols, select the regenerate option for all the symbols.
3. Click OK.
The Part Developer Errors dialog box appears. It should show no errors. Next, you will
add some properties to the symbol and package pins.
January 2002
178
Adding Symbol Pin Properties
Task Overview
Add the property my_pack_pin_prop to the pin 1G in the LS241_DIP package. The value
for the property should be my_prop_value.
Steps
1. To associate a pin property to the LS241_DIP package, expand the package in the tree
view.
The expanded view of the LS241_DIP package appears.
2. Right-click on the pin 1G.
January 2002
179
The Package Pin Properties dialog box appears. You can set the pin specific
properties for a package through this dialog box.
4. To enter the my_pack_pin_prop property, click Additional.
January 2002
180
The Additional property page appears. You enter the additional properties for a package
pin in this property page.
5. Enter my_pack_pin_prop under the Name column and click under the Value column.
6. Enter my_prop_value and click OK.
You successfully entered a package pin property. Next, you will add a symbol pin
property.
January 2002
181
Changing Symbol Pin Properties
Task Overview
Do the following changes to the pin G of symbol sym_1:
■
Change the blank pin spacing of pin G to leave 5 stub pin stubs before the pin G.
■
Add a symbol pin property my_symbol_pin_prop to the logical pin G in sym_1. The
value of the property should be my_symbol_prop_value. Set up the property so that
both the pin property name and its value is visible and left-aligned.
Steps
1. To associate a pin property to the sym_1 symbol, expand sym_1 in the tree view.
2. Right-click on G.
January 2002
182
The Symbol Pin Properties dialog box appears. You specify all the symbol pin specific
properties through this dialog box.
4. Enter 5 in the Before field of the Blank Pin Spaces group box. This will result in 5 pin
stubs being left blank before the pin G in the symbol sym_1. This feature is useful in
cases where you want to keep a certain amount of gap between two types of pins such
as an address bus and a scalar pin in a symbol.
5. To enter the my_symbol_pin_prop property to the symbol pin, click Additional.
January 2002
183
The Additional property page appears. You enter all the symbol pin related properties
through this page.
6. Enter my_symbol_pin_prop under the Name column and click under the Value
column.
7. Enter my_symbol_pin_prop_value.
8. Select Both from the Visible column.
9. Click OK.
You successfully added a symbol pin property. Now save the part.
After you modify a part, you should verify the part for correctness. See Verifying Parts on
page 76 for details. After you verify the part, you should export it to the reference area.
See Exporting Parts to the Reference Area on page 83 for details.
Note: After you export a part to the reference area, you should delete the part from the build
area.
January 2002
184
If you view the symbol in Concept-HDL, it should display as following:
Summary
In this chapter you learned to modify an asymmetrical part. In the next chapter you will how
Part Developer handles pin texts.
January 2002
185
10
Handling Pin Texts
Objectives
In this chapter, you will be able to:
■
Understand the methodology involved in handling pin texts.
Methodology
In parts created in earlier versions of Part Developer, the pin text was stored as a note in the
symbol file and not as a pin property. Therefore, there was no direct association of the pin text
with the pin. In the new release of Part Developer, pin texts are stored as properties on the
pin.
In the new Part Developer, the following methodology is implemented:
■
For new parts, the pin text is stored as the PIN_TEXT property. This property is
associated with the pin.
■
When parts created in an earlier version of Part Developer or Concept-HDL are loaded
in Part Developer, it is likely that the pin texts on symbols are not stored as properties on
the pin. In this case, Part Developer will automatically assign the pin texts to the pins and
you will be prompted to save the part. However, before saving the part, you should verify
that the pin texts are mapped correctly by launching the Associate Pin Text dialog box
and checking the pin texts corresponding to the pins.
■
In case there are some texts that are still unassociated, you should decide whether you
want to retain or remove the text. In case there are any unassociated pin text left on the
symbol, a warning will be given during the saving of the part. You can choose to either
retain the unassociated text in the symbol or remove them from the symbols. You may
want to retain the unassociated texts if they are symbol texts and not pin texts.
The next time you load such parts, the pin texts will be associated with the pins as pin
properties.
January 2002
186
Handling Pin Texts
To understand this feature, you will open the parts provided in the old_parts library
under the tutorial_project_data directory. To open the parts of the old_parts
library, you need to do the following:
❑
Add the old_parts library to the tutorial_project library project.
❑
Launch Part Developer on the parts of the old_parts library.
Adding Libraries to a Library Project
You can add your own libraries to an existing library project by modifying the cds.lib file of
the project. You can modify the cds.lib file from within Library Explorer.
Task Overview
Add the old_parts library to the tutorial_project library project.
Steps
1. Launch Library Explorer and open the tutorial_project library project.
2. Choose Edit > Modify Library List.
The cds.lib file appears.
3. Add the following line:
DEFINE old_parts c:\tutorial_project_data\old_parts
4. Save the file and close it.
5. Choose View > Refresh.
The old_parts library gets added to your library project. Next, you will launch Part
Developer on the parts of the old_parts library to understand how Part Developer
works with parts where the pin texts on symbols are not stored as properties on pins..
Working with Unassociated Pin Texts
To understand the how Part Developer deals with older parts, you will open the following parts
of the old_parts library:
■
3807
January 2002
187
Handling Pin Texts
This is a part with a 10 bit vector pin O and a scalar pin IN. Each bit of the vector pin
has a pin note associated with it, such as O1, O2 etc. The original symbol is
displayed below:
■
803237_50hz
This is a part with 20 logical pins, 4 power pins and two ground pins. The sym_1 is
displayed below:
January 2002
188
Handling Pin Texts
Note that some of the pins have two pin texts associated with them, such as LOW
BATTERY and EXTERNAL ADJ is associated with the BATT_EXT pin.
Task Overview
Open the 3807 part in the old_parts library and associate the pin texts as pin properties.
Steps
1. In the Library Explorer window, select the 3807 part in the old_parts library.
Part Developer launches on the 3807 part with a message box saying that the pin texts
in the symbol are not stored as properties of the pin. This happens because currently the
pin texts are not associated to the pins as pin properties.
3. Click OK.
The part opens in the Part Developer with the warning that some text in sym_1 could not
be associated with any pin. You should use the Associate Pin Text option to associate
January 2002
189
Handling Pin Texts
the text properly. This happens because part Developer tries to associate the pin texts to
the existing pins of the part and finds some text that it fails to associate with any pin.
4. Click OK.
5. To display the Associate Pin Text dialog box, right-click on sym_1 in Part Developer
tree view.
6. Select Associate Pin Text.
The Associate Pin Text dialog box appears. Since Part Developer has the limitation
that for a vectored pin, bit specific property values are not allowed. So the pin texts for all
the bits are constrained to be the same. Therefore, in the Associate Pin Text dialog box,
January 2002
190
Handling Pin Texts
only pin O10 gets associated with the vector pin O and rest of the notes are left as
unassociated text.
7. Change the pin text associated to the vector pin O from O10 to O. This is required
because Part Developer follows the convention of always adding the range notation (<0>
etc.) for pin texts for a vectored pin.
8. Click OK.
Next, you need to remove the unassoicated text as they have no relevance for the
symbol. To remove the unassociated pin texts, you need to save the part.
January 2002
191
Handling Pin Texts
The Retain Unassociated Text dialog box appears.
10. To remove the unassociated text, select the Remove Unassociated Text checkbox.
11. Click OK.
A message box appears. It should show no errors.
12. Click OK.
13. Launch Concept HDL on the sym_1.
Note that the bits of the vector pin now have O<n> as the pin text associated with
them.For example, bit 1 has the pin text O<1>.
14. Close Concept-HDL and Part Developer.
Next, you will open the 803237_50hz part.
Task Overview
Open the 803237_50hz part in Part Developer.
January 2002
192
Handling Pin Texts
Steps
1. In Library Explorer, select the 803237_50hz part.
Part Developer launches on the 803237_50hz part with a message box saying that the
pin texts in the symbol are not stored as properties of the pin.
3. Click OK.
The part opens in the Part Developer with the warning that some text in sym_1 and
sym_2 could not be associated with any pin. You should use the ‘Associate Pin Text’
option to associate the text properly.
4. Right-click on sym_1 in the Part Developer tree view.
5. Select Associate Pin Text.
The Associate Pin Text dialog box appears. It is important to remember that although
Part Developer tries to associate pin texts to pins, three things could happen:
❑
Wrong pin text is associated with a pin.
❑
Some pin texts are left unassociated
❑
Pin with multiple pin texts have only one pin text associated with them. The
remaining stay as unassoicated.
Therefore after the Associate Pin Text dialog box is opened the first time, you should
verify the pin texts against the symbol and fix the inconsistencies.
In the 803237_50hz, all the three inconsistencies are present. Note that the pins 5VA,
8VA, 5VB and 8 VB have incorrect pin texts. Pins such as Z_AMP_IN have no pin texts
associated with them. And pins such as BATT_EXT which had multiple pin texts have
January 2002
193
Handling Pin Texts
only one pin text associated with them. The remaining pin texts are left as unassoicated.
Therefore, you need to fix these inconsistencies.
First, fix the incorrect pin text issue.
6. Edit and change the pin text entry next to pin 5VB from VB to 5VB.
Similarly change the other incorrect pin texts. Next, map the pin texts to the pins which
have been left blank.
7. Select Z_AMP_IN in the Pin Name column and Z AMP IN in the Pin Text column and
click Map.
This maps the Z AMP IN pin text to the Z_AMP_IN pin. Similarly, map the GAIN BLOCK
INPUT, EXTERNAL BIAS, V REF IN, LOOSE LEAD and LOW BATTERY pin texts.
Finally, you need to determine whether you want to add the pin texts to the pin that had
multiple pin texts.
8. The pin BATT_EXT had two pin texts, LOW BATTERY and EXTERNAL ADJ. Part
Developer only associated LOW BATTERY pin text to the BATT_OUT pin and left the
other pin text as unassociated pin text. In case you want to add it, you will have to edit
the LOW BATTERY pin text and type the remaining pin text by hand.
January 2002
194
Handling Pin Texts
After you have completed updating the pin text association for sym_1, you should verify
and update the pin texts for sym_2.
Note: It is important to remember that the part name that appears in the symbol is the
symbol text stored in the symbol file and can be edited only through the Symbol
Properties dialog box.
Next, you need to delete the unassoicated pin texts. To remove the unassociated pin
texts, you need to save the part.
The Retain Unassociated Text dialog box appears.
10. To remove the unassociated text, select the Remove Unassociated Text checkbox.
11. Click OK.
A message box appears. It should show no errors.
12. Click OK.
13. Launch Concept HDL on the sym_1 and verify that the pin texts are associated properly
as pin properties.
14. Close Concept HDL and Part Developer.
Summary
In this chapter you learned how Part Developer handles pin texts. This chapter also concludes
the functionality that is available in Library Explorer and Part Developer if you have the PCB
Librarian licence. In the next chapter you will learn to create and work in data-managed
projects.
January 2002
195
11
Data-Managed Projects
Objective
To become familiar with the methodologies and steps in creating and working with datamanaged projects.
■
Understand the methodology of a data-managed project.
■
Setup the environment variables necessary to launch Library Explorer in the datamanaged mode.
■
Execute the script to setup areas needed to work in data-managed mode.
■
Create the data-managed project using Library Explorer.
■
Join a data-managed project.
■
Checkout a part and modify it.
■
Checkin the modified part.
Overview of Data-Managed Project
Overview
You can create data-managed (DM) projects in Library Explorer only if you have the PCB
Librarian Expert licence. DM projects allow teams of library developers to work on projects.
The Project Leader can create a new DM project and the team members can then join in.
Version control of data is supported. The Library Explorer tool provides the interface for
managing library data through checking-in and checking-out of data.
A project comprises of the following storage areas:
January 2002
196
■
Vault or Repository
This is the location where all checked-in data resides. Users (team members and the
Project Leader) can check out data, work on it, and check in data back into the repository.
Each project has its own repository. Multiple projects cannot share a repository.
■
Integration area (Integ area)
This is the location where all the verified libraries and parts are stored. The Project
Leader checks out data from the repository, validates it, and updates the integration area
with libraries for the designers. This area serves as the access point for designers.
■
Local work areas/build areas
These are the local work areas owned by individual team members. The team member
can check out data from the repository into the local work area, work on it, and check the
data back in to the repository. Team members can also create new libraries and cells and
check them into the repository.
The creation of a new project would typically be a one time operation because all the
libraries can be managed by one project. For specific reasons such as to have separate
team members for different projects, the Project leader might decide to create more than
one project, and distribute the libraries to be managed among these projects.
January 2002
197
The following figure illustrates the use model of a DM project
Leader
ProjectProject
Leader
■
Create Project
■
Modify Project
Repository
■
Update integ area
■
Create work area (optional)
If work area is created:
■
Check out from repository
■
Check in to repository
PL updates
the integ area
Team Members
Integ Area
■
Join Project
■
Check out from repository
■
Check in to repository
Designers
January 2002
198
Pre-requisites for Creating a DM Project
Library Explorer enables you to create a DM project. However, before creating a project, the
following needs to be done by the Project Leader. They are:
1. In UNIX, set the umask appropriately, by running the command umask 002. This is
required so that everybody in the group has permissions to make modifications in the
repository. For NT, set up the appropriate share permissions (i.e. read, write) on the
folders corresponding to the repository and the integration area. This permission is
required for all users.
2. Set the following variables:
❑
TZ = GMT
This sets the time zone. This is required by VersionSync to execute properly.
❑
GDM_MAIL_HOSTNAME = <your_mailserver_name>
This setting is required for Part Developer to send mails to team members asking
them to join the project.
3. Decide on the libraries that need to be managed and the integration area.
4. Decide on the location of the vault or the repository for the project.
5. Decide on the location of the local workarea.
6. After you have decided the libraries to be managed and the locations, you need to run
the vssetvault script in a command window. This script sets up the vault, integration
area, and local workarea appropriately. Currently, data-managed functionality is being
provided with the version control system called VersionSync. The script that needs to be
run for setting things up is called vssetvault and for UNIX, should exist in
<install_dir>/tools/bin (if the VersionSync kit has been installed).
Before you create or join a DM project in NT, you should do the following:
1. Provide write access to the repository and the integration area to all the members of the
project team.
2. Put the following entry as the first entry in your PATH environment variable:
<your_install_dir>/vs_nt
This entry ensures that the diff executable in the vs_nt directory is the one that is
picked up by the tool.
January 2002
199
The vssetvault script takes two parameters, the path to your repository and the path to
your integration area or the local build area.
The vssetvault script has to be run twice. In the first instance, the script prompts for the
paths to the repository and the integration area. The syntax for running the command for the
first time is:
vssetvault <path of the repository> <path of the integ area>
In the second instance, specify the path for the repository and the local work area. When you
run it the second time, the syntax is:
vssetvault <path of the repository> <path to your local build area>
For example, if you want to create the repository in x:\gdm_projects\repository
and the integration area in x:\gdm_projects\integ, you will have to specify the
following command at the command prompt:
vssetvault
x:\gdm_projects\repository x:\gdm_projects\integ
This will create the repository and integ folders under x:\gdm_projects and
populate the integration area with the two files, .VSVAULT and cdsinfo.tag. The
.VSVAULT file contains the path to the repository, and the cdsinfo.tag file contains the
entry for the type of version control tool used. In case of vssetvault, the entry will be
DMTYPE vs
To create a local build area, for example localbuildlib under x:\gdm_projects, give
the command:
x:\gdm_projects\repository
x:\gdm_projects\localbuildlib
vssetvault
This will create a folder named localbuildlib under x:\gdm_projects and populate it
with the .VSVAULT and cdsinfo.tag files.
For the librarian and the members, ensure that mapping to the repository and the integration
area is the same. For example, if the project leader creates the repository and the integration
area in F:\rep and F:\integ respectively, then all the team members should also have
the mapping to repository and integration area as F:\rep and F:\integ respectively.
Once you have run the vssetvault script, you are ready to create a DM project. When you
create a new project, you are the project leader for that project. You create a new project to
specify the integration area, repository, and work area. You should also define the reference
libraries that are to be managed and the team members who will work on the project.
You can define the libraries that are to be managed by specifying the paths to these libraries
or by including cds.lib file that has the paths to these libraries.
January 2002
200
Creating a Data-Managed Project
Task Overview
Create a new DM project as a project leader and name the project my_dm_project.
Note: All the screenshots are based on the assumption that the data-managed project is
created in D:\gdm_projects
Steps
The first task in creating a DM project is to set the environment variables.
1. Set the following environment variables:
❑
TZ=GMT
❑
GDM_MAIL_HOSTNAME = <your_mailserver_name>
Next, you need to create the necessary directory to create and store the project.
2. Create the gdm_projects directory under D:\.
After you create the directory, you need to run the vssetvault script to set up the
environment for creating a DM project.
3. Run the vssetvault script to mark the respective directories as integration area,
repository and local work area. The commands are:
vssetvault d:\gdm_projects\repository d:\gdm_projects\integ
vssetvault d:\gdm_projects\repository d:\gdm_projects\local_area
This sets up the following project directory:
Directory Name
Purpose
d:\gdm_projects\integ
The location of the integration area
(reference area) for the tutorial.
d:\gdm_projects\repository
The location of the repository for the
tutorial.
d:\gdm_projects\local_area
The location of the project leader’s local
work area for the tutorial.
January 2002
201
Next, the library project needs to be created.
4. If you are in UNIX, launch Library Explorer by typing the following command in the
command window
libexp &
If you are in NT, launch Library Explorer by doing the following steps:
a. Choose Start > Run.
The Run dialog box appears.
b. The executable for Library Explorer is libexp. To run the executable, type libexp
in the Run dialog box.
The Library Explorer Product Choices dialog box appears.
5. To launch Library Explorer from the PCB Librarian Expert suite, select PCB Librarian
Expert.
6. Click OK.
The Getting Started dialog box appears.
7. To create a new managed library project, select the Create a new Managed Library
Project radio button.
8. Click OK.
January 2002
202
The Project Type page of New Project Wizard appears. In this page, you determine
whether or not to create a managed project.
9. To create a data-managed project, ensure that the DM option is selected.
10. Click Next.
The Create Options page of New Project Wizard appears. In this page, you
determine whether to join an existing DM project as a team member or to create/manage
a project as the project lead. If you select the team member option, you can join an
existing DM project. If you decide to join as a project lead, you need to determine whether
you want to create a new project from scratch or use an existing location containing your
libraries as the integration area.
For the tutorial, you will be the project lead and create a new project.
11. To create a new project as the project lead, select the Administrator/project lead radio
button.
Notice that by default the New checkbox is selected.
12. Click Next.
January 2002
203
The Project Name and Location page of New Project Wizard appears. In this page,
enter the project name and the location to the integration area.
13. Enter my_gdm_project in the Project name field.
Next, the location of the integration area needs to be specified.
14. Browse and select the D:\gdm_projects\integ as the integration area.
15. Click Next.
The Libraries page of New Project Wizard appears. In this page, you can add the
libraries that you want to manage to your project. You can add the libraries by either
physically selecting the library folders, or by importing a cds.lib file. If the libraries are
January 2002
204
not in the integration area, then the selected libraries will get copied into the integration
area.
For the tutorial, a sample library lcx is provided under the
x:\tutorial_project_data\lcx folder.
16. To add the lcx library, click Add.
The Choose Directory dialog box appears.
17. Select the lcx library from x:\tutorial_project_data\lcx.
18. Click OK.
January 2002
205
The selected library is added.
19. Click Next.
January 2002
206
The Project Team page of New Project Wizard appears. In this page enter the
information pertaining to the project team members. A mail is sent out to each member
whose email has been provided in the E-mail column.
20. Enter the team member’s details. For demonstrative purposes, we have used Vishal
Kumar as team member.
The Create Work Area page of New Project Wizard appears. In this page you need
to specify the path to the local work area for yourself. This is optional. You may choose
not to create a local work area for yourself.
For the tutorial, the local work area which was created in the beginning of the tutorial will
be used.
January 2002
207
22. To select the local_area as the local work area, click the Browse button and select the
D:\gdm_projects\local_area directory.
23. Click Next.
January 2002
208
The Summary page of New Project Wizard appears.
#
24. Click Finish.
A message box will appear informing you that mail have been sent.
25. Click OK.
The project will be created, and displayed in the Library Explorer window.
Next, you will checkout the lcx00 component from the reference area into the build area.
26. Choose File > Check Out.
The Check Out (Read Only) dialog box appears. You can select the parts that you want
to checkout through this dialog box. Note that, by default the checkout is read-only.
However, you can also checkout parts in a read/write mode. For completing the task in
this chapter, you need to checkout the lcx00 part in read\write mode.
27. To checkout the part in read/write mode, click Options.
January 2002
209
The Checkout Options dialog box appears.
28. Select the Check out Read/Write option.
29. Click OK.
You configured Library Explorer to checkout the parts in read/write mode. Next, you need
to select the part that you want to check out.
30. Click on the lcx00 checkbox.
31. Click OK.
The Library Explorer message box appears informing that the check-out operation was
successful.
32. Click OK.
Important
You can see the DM status of any library or part by right-clicking on the library/part
and selecting the GDM Status option.
January 2002
210
A GDM Status message box appears (sample shown below) appears informing you the
DM status of the part.
Next, modify the part and add a symbol property my_prop with value my_val.
33. You use Part Developer to modify parts. See the earlier chapters to know more about
modifying a part.
Next, you need to checkin the part.
34. To checkin the part, select File > Check In.
January 2002
211
The Check In dialog box appears.
35. To simultaneously update the integration area so that the modified part is also available
to the designers, select the Update integ area checkbox.
Note: When you checkin a part, Part Developer automatically increments the version number
of the part.
36. Click OK.
A message box appears informing that the check-in was successful. This creates the
version 1.2 of the part.
37. Click OK.
38. Next, you will check-out the version 1.1 of the part. It is important to remember that you
can only checkout older versions in read-only mode.
39. To check-out an older version, select File > Check Out
40. To checkout the part in read/write mode, click Options.
January 2002
212
The Checkout Options dialog box appears.
41. Select the Update with tag option.
42. To checkout the version 1 of the part, enter 1 in the Repository Tag Name field.
43. Click OK.
44. Click OK.
A message box appears informing that the check-in was successful. The first version of
the part is checked out. Remember that it is checked out in read-only mode.
Summary
In this chapter you learned about the methodology of a data-managed project. You also
learned the steps involved in creating and working in a data-managed project. In the next
chapter, you will learn to create a part from an XML datasheet.
January 2002
213
12
Using XML to Create Parts
Objective
To become familiar with the steps involved in using XML datasheets to create parts.
■
Import data into Part Developer from an XML file.
■
Implement post-import corrections.
■
Update the package information.
■
Create symbols.
Importing Part Data from an XML Datasheet
Task Overview
Import the part information for the LS244 component from the XML datasheet named
74ls244.zip. It is stored in the tutorial_project_data/datasheets location.
Steps
1. Launch Part Developer and open the tutorial_project.cpm project.
The Create/Open Part dialog box appears.
2. To begin the process of importing form an XML file, Click Cancel.
3. Choose File > Import XML.
The Import from XML to Concept HDL dialog box appears.
January 2002
214
4. Select 74ls244.zip from the tutorial_projects/datasheets location and click Open.
Next, you need to decide whether you want to convert only the master component, or
each alias as individual primitive or each alias as individual cell.
If you choose to convert only the master component, then one Concept HDL part is
created. The chips.prt file will have only one primitive section with the master
component name as its only entry.
If you choose to convert each alias as individual primitives, then one Concept HDL part
is created with each alias appearing as a primitive entry in the chips.prt file. For
example, if a part has four aliases, the resultant chips.prt file will have four primitives.
If you choose to convert each alias as an individual cell, then as many number of parts
as there are aliases will be created. For example, if a part has four aliases, then four
separate Concept HDL parts will be created.
5. You need to create only the master component. By default, this option is selected.
6. Click OK.
The LS244 part appears in the Part Developer tree view.
After you read-in the part information from the XML datasheet, you need to take care of the
following issues:
PIN_TYPE Property
The PIN_TYPE property gets filled in as per the following rules:
January 2002
215
■
Passive is interpreted as ANALOG.
■
Rest of the pins are mapped to their corresponding types in Part Developer.
CLASS Property
The CLASS property gets filled in as per the following rules:
■
CLASS property gets the value IC if the Designator element in the XML datasheet had
the value U.
■
CLASS property gets the value IO if the Designator element in the XML datasheet had
the value J, JP or SW.
■
CLASS property gets the value DISCRETE for all other values of the Designator element
type. These values are: C, D, ISO, L, LS, Q, R, T, U, VR, and Y.
Therefore, you may need to check the value of the CLASS property after the data has been
imported from the XML datasheet. If required, change the value of the CLASS property. The
steps are:
1. Right-click on the part name in the tree view.
2. Select Properties from the shortcut menu.
3. Change the value of the Part_Type field.
DUPLICATE PINS
Often a part may have duplicate pins names such as multiple collector pins in transistor,
programmable IO pins in FPGAs etc. In such cases, Part Developer appends an index with
‘_’ to the pin name starting from the second occurrence. For example, if there are two
collectors with name C, they will be read-in as C and C_1.
Pins With ‘>’ or ‘<‘
Certain pins have either a ‘>’ or a ‘<‘ symbol in their pin names, such as P>Q or P<Q in
comparators. Such pins will be read in with the ‘>’ symbol converted to ‘_GT_’ and the ‘<‘
symbol converted to ‘_LT_’ in the pin names. For example, a pin name P>Q will get converted
to P_GT_Q.
January 2002
216
Partnames with ‘/’
Some part may have ‘/’ symbol in their part names. The ‘/’ in such part names will get
converted to ‘_’ in the primitive entry of the chips.prt file.
JEDEC_TYPE
When a part information is imported from an XML datasheet, the value of the JEDEC_TYPE
property is not seeded. You will need to manually specify the value of the JEDEC_TYPE
property for a part.
NC Pins
E-tools XML datasheets do not contain information about the NC pins. Therefore, when you
import the data from the XML datasheets, NC pins would be absent from the packages. You
can follow one of the two methods to add the NC pins to the packages:
1. Use the Extract From Footprint option in the Physical Pin Mapping tab of the Package
Properties dialog box, and then mark the required unmapped pins as NC pins.
2. Manually add the pin numbers and mark them as NC pins.
Note: If you use the Extract From Footprints option, you will lose the mappings for those
pins that are mapped to logical pins but not present in the list of extracted pin numbers.
Symbol Interpretation
After you create a part from an XML datasheet, you need to be aware of the following:
■
The origin of the symbol will be at the top left corner of the symbol bounding box and the
PART_NAME will be displayed just above the origin.
■
Pin text will appear outside the symbol graphic.
■
In data sheets, the multi-assertion pin names appears as name/name. When such pins
are read into Part Developer from XML, each character in the low asserted part of the
name is followed by a ‘\’. For example, RD/WR will be written as RD/W\R\.
■
Sometimes, some of the symbols may appear to have additional height. This is because
when a part data is imported from XML, all the power pins are moved to the body section
of the chips.prt file. This results in the removal of power pins from the symbols.
However, the space reserved by the symbol for power pins is not adjusted after the power
pins are moved to the body section.
January 2002
217
Once you have taken care of the above mentioned issues, you should verify the part. Only
after the verification of the part is complete, you should check-in the part.
Summary
In this chapter you learned to create a part from an XML datasheet. In the next chapter you
will learn to create a part template and apply the template to create parts.
January 2002
218
13
Creating Templates
Objective
To become familiar with the methodologies and steps involved in creating and using Part
Templates.
■
Create a new template.
■
Apply the template.
■
Create a part with the applied template values.
■
Verify the part against the template.
Overview
Part Developer provides you the ability to set up the part construction rules and property
setup through the use of Part Templates. Using the templates, you can quickly create parts
that follow your company standards and yet have the flexibility to add properties and
behaviors specific to the part.
Using Part Developer, you can:
■
Create a template.
A template can be created with data such as property names and values, pin positions
and symbol display characteristics. The template is then used to create multiple parts.
■
Create parts using a template.
A template can be selected from the existing list of available templates and parts created
based on the information stored in the template.
■
Verify parts against a template.
January 2002
219
Creating Templates
Parts can be verified against a selected template or the original template from which the
part was created.
Creating and Applying a Part Template
Overview
Part Developer enables you to create part templates. While creating part templates, you can
specify the following information:
In Packages
■
Package properties
■
Pin load properties
In Symbols
■
Grid size
■
Symbol outline
■
Pin text orientation
■
Pin text size
■
Whether to use pin names for pin text
■
Minimum symbol height
■
Minimum symbol width
■
Symbol properties
■
Symbol pin spacing, both top/bottom and left/right
■
Position of symbol pin types
After you specify the information, you save the information in a .tpl file. This file can then
be used as a template in later sessions of Part Developer to create parts.
January 2002
220
Creating Templates
Task Overview
Create a template with the symbol property PART_NAME, a package property
CREATED_ON . Save the template in mytemplate.pl and apply it.
Steps
1. Launch Part Developer and open the tutorial_project.cpm project.
The Create/Open Part dialog box appears.
2. Click Cancel.
The empty Part Developer window appears.
3. Choose Templates > New.
January 2002
221
Creating Templates
The New Template dialog box appears. Note that the properties that were set up in the
Tools > Options appear as template properties.
Next, you need to enter the new template properties.
4. Enter the property name as PART_NAME.
5. Enter the property value as ?.
This will ensure that the property is annotated to the symbol and the value for this
property has to be specified by you in Concept-HDL.
6. Select the value of the Visible field as Both.
7. Specify the alignment as Center.
8. Since the PART_NAME property has to appear only on the symbols and not packages,
deselect the Package option.
Next, you need to specify the package property CREATED_ON for the packages.
9. Select the next blank line under Property_Name, and enter CREATED_ON as the
property name.
10. Enter ? as its value.
11. Since the CREATED_ON property is to be applied only to packages, deselect the
Symbol checkbox.
12. Click Save.
The Save Part Template dialog box appears.
13. Enter the file name as mytemplate. tpl
January 2002
222
Creating Templates
14. Click Save.
A Part Developer message box appears.
15. To apply the template, click Yes.
The blank Part Developer window appears with the template applied on it. Basically, the
Setup options properties are updated. You can now create parts. The new parts will
automatically contain the properties that you set up through the templates.
In case you want to see the properties that you added using templates, choose Tools >
Options.
Using Part Template to Create Parts
You use a part template as the building block in creating one or more parts. To create parts
using a part template, you need to open the part template and apply the template values to
the current session of Part Developer. This overrides the default values specified through
Tools > Options. Once you have applied the template, proceed with the creation of parts as
detailed in Chapter 4, “Creating Parts With Pins Split Across Symbols” and Chapter 6,
“Creating a Multi-Section Symmetrical Part” and Chapter 8, “Creating Asymmetrical Parts”.
For this chapter, create a simple part with two input pins A, B and an output pin Y. Name the
part mypart and create one package DIP and one symbol with logical pins for it. Enter ? as
the JEDEC_TYPE value.
Next, you will verify the part against the template that you created.
Verifying Parts Against Templates
To ensure that the parts are conforming to your standards, Part Developer enables you to
verify a part against a template. The verification is done only for those values that exist in the
template file. The output is displayed as a report that can be saved as a .rep file. The
verification is done as per the following rules:
January 2002
223
Creating Templates
Property Checks
The property check is done on all packages for the following:
■
All properties listed in the template for a package must exist in each package of the part.
■
The value of the property in each package must match the value in the template unless
the value in template is "?" or blank.
Pin Load Checks
This is done on all pins in all packages as per the following rules:
■
If PINUSE="UNSPEC" exists for a pin, all checks are bypassed on that pin.
■
If a pin type is not determined, it is an error.
■
If a pin type is determined, its load value is checked against the load value of that pin
type in the template. An error is generated if the load values don’t match.
■
Error is shown if any of the loads for a pin type is missing.
Symbol Checks
All Symbols are checked for a given part as per the following rules:
■
All symbols must have at least one connection with a line stub or a bubble else an error
stating that check cannot proceed is shown.
■
All lines are assumed to be vertical or horizontal. Arcs are not supported in this release.
■
Each Bubble is interpreted to have two virtual stub lines - horizontal and vertical.
■
No two connections can have the same X, Y coordinates, else error is shown to the user.
■
Location of connections is derived based on the direction of the stubs attached to the
connection. Therefore, only connections that have a stub or a bubble on them are
checked.
■
Stub length is calculated based on the integer average of all stub lengths.
■
The outline of the body is derived by searching for the perpendicular line from the end of
stub. As the stub size varies, the search is made within the range of the stub size
variance. After getting a single outline, the rest are traced as the ones connected the
outline end points. The procedure is executed recursively for each detected outline.
■
Minimum pin spacing are calculated for all sides (Top, Left, Right, Bottom).
January 2002
224
Creating Templates
■
For pin texts, the property PIN_TEXT is used. If it is not found, pin texts are searched
for within 1/3 of the average stub length from the end of the stub for each connection.
Also the location (x,y) of the pin note must not be mis-aligned by more than 1/2 pin
spacing.
■
Grid is derived by taking the highest common factor of all differences of values of X and
Y on respective coordinates. Only the connection (Logic) grid is derived. The symbol grid
is not derived even though the template mentions it as Symbol Grid.
■
All properties listed in the template for symbols must exist on each symbol in the part.
■
The value of the property in each symbol must match the value in the template unless
the value in template is "?" or blank.
■
The alignment of the property must match the one specified in template.
■
The visibility of the property must match the one specified in template.
Pin Checks
Each pin is checked as per the following rules:
■
Each pin based on the type as defined in the template must be at the location area in
symbol as defined in the template for that type.
■
The text size of the pin must match the size specified in the template.
■
The Use Pin Names For Text is checked only if the template sets it to true.
■
The text style for pin text is checked with value in template. If the style is vertical for top
and bottom pins and horizontal for pins on left and right then the style is considered to
be Automatic. The angles of 90 and 270 are considered equivalent and vertical and 0
and 180 are considered equivalent and horizontal.
■
All pins with spacing less than the spacing specified in the template are marked as
errors.
Grid Checks
Grid checks are done with the following rules:
■
Conversions are done for calculating and matching the grid values for Inches and
Fractional (Fractional is currently not supported in Part Developer). This is then matched
with the template value.
January 2002
225
Creating Templates
Outline Checks
The outline checks are done with the following rules:
■
All detected Outlines are checked to match the thickness specified in template.
Minimum Size Checks
■
The minimum pin spacing values on the left and right is read for each symbol and verified
against the minimum pin spacing left and right value stored in the template. An error is
generated if the value in the symbol is less than that of the value stored in the template.
■
The minimum pin spacing values on the top and bottom is read for each symbol and
verified against the minimum pin spacing top and bottom value stored in the template.
An error is generated if the value in the symbol is less than that of the value stored in the
template.
■
The minimum symbol height value is read for each symbol and verified against the
minimum symbol height stored in the template. An error is generated if the value in the
symbol is less than that of the value stored in the template.
■
The minimum symbol height width is read for each symbol and verified against the
minimum symbol width stored in the template. An error is generated if the value in the
symbol is less than that of the value stored in the template.
The output of the verification is displayed in a dialog box. The output is divided into two
sections, Overview and Details.
In the Overview section, the overview of the differences are displayed. In the Details section,
the differences are detailed.
Task Overview
Verify the part mypart against the mytemplate.tpl template.
Steps
1. Choose Tools > Verify.
2. Select the Verify with Templates option.
3. Click OK.
January 2002
226
Creating Templates
The Select Part Template dialog box appears. You need to select the template file
against which the verification will be done.
4. Select mytemplate.tpl and click Open.
The verification is run and the differences found are displayed in the Part verification
with Template dialog box.
Notice that one difference has been found with relation to the symbol properties.
Summary
In this chapter you learned to create a template and apply the template to create new parts.
In the next chapter you will learn to extract and modify templates.
January 2002
227
Creating Templates
January 2002
228
14
Extracting Templates
Objective
To become familiar with the methodologies and steps involved in extracting and modifying
part templates.
■
Extract a template from a part.
■
Modify the extracted template.
■
Save the template.
■
Apply the template on a part.
If you have a part which has been built in compliance with your company standards, you can
extract information from it and create a template. After the template information is extracted,
the part is verified against the extracted template information. A verification report is
generated listing the differences with the extracted values. Template information is extracted
as per the following rules:
From Packages
■
All properties found in any of the packages are added to the template with their values.
■
If the property name matches with any of the properties listed below then the value is
replaced with "?":
❑
JEDEC_TYPE
❑
POWER_PINS
❑
NC_PINS
January 2002
229
❑
BODY_NAME
❑
PART_NAME
❑
TECH_FAMILY
Pin Load Extraction
Pin Load is extracted from the different pin types. If a pin type is not found on one of the
packages, it is searched in the next package and so on. If a pin type is not found on any of
the packages, its load is not added to the template. If for any pin type the load extracted is not
a standard, i.e., the load is not same for all pins of a type on all packages then the first load
is used.
Symbol Data Extraction
■
All symbols are read for a given part.
■
All symbols must have at least one connection with a line stub or a bubble else an error
stating that process cannot proceed is displayed.
Symbol Property Extraction
■
All properties found in any of the symbol are added to the template with their values.
■
If a property exists both in a package and a symbol, the package property is given
precedence and its value is extracted.
■
Alignment and visibility are extracted from the symbol and added.
■
If the property differs in value across packages or across symbols to or it differs in
visibility or alignment, then the value of the property from the last instance of either the
package or symbol is extracted.
Symbol Pin Extraction
For each pin the following checks are done:
■
A search is done for the first pin of each pin type and its location value is added to the
template.
■
The Use Pin Names For Text option is set to false if a single pin is found to violate this
rule.
January 2002
230
■
The Text Style for Pin Notes is interpreted. If the style is vertical for top and bottom pins
and horizontal for pins on left and right then the style is considered to be Automatic. The
angles of 90 and 270 are considered equivalent and vertical and 0 and 180 are
considered equivalent and horizontal. If it is not consistent for all the instances for a pin
type based location then user is warned that this is not a standard.
Grid Extraction
The highest common factor of all differences in X distances and Y distances is taken as the
minimum grid unit. It is calculated into template in Inches.
Minimum Size Extraction
■
The minimum pin spacing values on the left and right are read for all the symbols and the
smallest value is extracted to the templates as the minimum spacing value for left and
right. If in a symbol, 0 or 1 pin exist on left and right, its value is not extracted.
■
The minimum pin spacing values on the top and bottom are read for all the symbols and
the smallest value is extracted to the templates as the of minimum spacing on top and
bottom. If in a symbol, 0 or 1 pin exist on top and bottom, its value is not extracted.
■
The symbol height value is read for all the symbols and the smallest value is extracted
to the templates as the of minimum symbol height.
■
The symbol width value is read for all the symbols and the smallest value is extracted to
the templates as the of minimum symbol width.
■
The outline is extracted as thick if all outlines are thick. The outline is extracted as thin if
all outlines are thin. If neither of the cases are true then no extraction is done for this
value. If a value is not extracted, a warning is displayed.
Task Overview
Extract template information from the LS244 part that you had created by importing the data
from an XML datasheet.
Steps
1. Import the ls244 part from the reference area.
2. Launch Part Developer and open the ls244 part
3. Choose Templates > Extract.
January 2002
231
The New Part Template dialog box appears. You need to enter the file name into which
you want to store the template information that will be extracted.
4. Enter fromls244.tpl as the template file name and click Save.
The Extracted Template Values dialog box appears. You can view the extracted values
in this dialog box.
5. Click OK.
The Extracted Template Values dialog box disappears.
Next, you need to modify the template values.
January 2002
232
Modifying Template Values
Overview
After the template information has been extracted into Part Developer, you can modify the
extracted information. You can modify the information by editing the template values.
Task Overview
Modify the Pin Text Size value in the fromls244.tpl template file from 0.88 grids to
0.50 grids. Save the template file after you have made the necessary changes.
Steps
1. Choose Templates > Edit.
The Load Part Template dialog box appears.
2. Select fromls244.tpl template file and click Open.
The Edit Template dialog box appears.
To make changes to the pin text size, you need to go to the Symbol property page.
3. Click Symbol.
4. Modify the Pin Text Size value to 0.50.
5. Click Save.
January 2002
233
The Save Part Template dialog box appears.
6. Enter the name of the modified template file as my_ls244.tpl and click Save.
A Part Developer message box appears asking you whether to apply the template.
7. To apply the template, click Yes.
Summary
In this chapter you learned to extract a template from a part and modify the extracted
template. In the next chapter, you will learn to create a VHDL wrappers and map files.
January 2002
234
15
Creating VHDL Wrappers and Map Files
Objective
To become familiar with the methdologies and steps involved in creating and using VHDL
wrappers and map files.
■
Create VHDL wrapper and map file for a part
Overview
Concept HDL generates a netlist that you can use to simulate your logical design using a
Verilog or VHDL based simulator. To generate the netlist, it uses the symbol pin names as the
interface ports for each component used in the design. The interface ports of a part may be
January 2002
235
different from the VHDL model’s ports. For example, for the part 74ac74, the interface ports
are:
January 2002
236
For the same part, the VHDL model’s port names are:
To successfully simulate a design, a mapping is required between the symbol pin names with
the model port names. This making is stored in wrapper and map files. The wrappers or map
files can be created using Part Developer.
January 2002
237
Creating a VHDL Wrapper/Map File
Task Overview
Create a VHDL wrapper and map file for the 74ac74 part. The VHDL model for the part is
provided in the vhdl_models directory under tutorial_project location. You will need
to import the 74ac74 part from the Cadence supplied reference libraries.
Steps
1. Launch Library Explorer and open the tutorial_project.cpm project.
2. Import the 74ac74 part from the 74ac reference library.
3. Open the part in Part Developer.
4. Choose File > New > VHDL Wrapper/Map File.
The VHDL Wrapper/Map file dialog box appears. You enter the path to the VHDL
model in this dialog box. This can be done by specifying either the actual physical path
to the VHDL model or the Lib:Cell:View structure.
For example, to access the VHDL model stored in x:⁄74ac⁄sn74ac74, you may provide
either the entire physical path or use the lib:cell:view method, i.e. specify
sn74ac:sn74ac74::vhdl_lib.
Note: To use the lib:cell:view method, there should be a library entry in the cds.lib file
of the project. For example, to use the sn74ac74 with the lib:cell:view method, the
following entry should be present in the cds.lib file:
January 2002
238
DEFINE 74ac x:⁄74ac
Since the cds.lib file entry has not been made for the VHDL model, you will use the
File method to specify the path to the VHDL model.
5. Select File.
6. Browse to the location of the VHDL file,
c:\tutorial_project_data\datasheets\vhdl_models\74ac74\entity\vh
dl.vhd
Next, you need to determine whether to bind the VHDL model and the symbol. That is,
determine whether to bind the symbol with one specific architecture (behavior). If you
decide to bind the VHDL model and the symbol, then the binding statement goes into the
wrapper. This is an optional step.
Since each view of the model is essentially a specific architecture, selecting the VHDL
model by using the lib:cell:view method automatically fills in the binding statement. If you
specify the actual physical path to the VHDL model, then you have to explicitly enter the
binding information. If you decide not to enter the binding information during wrapper
creation, then the binding information has to be specified later in the simulation flow.
However, not providing the binding information in the wrapper provides the freedom to
use the same wrapper for different architectures.
For the tutorial, you will leave the binding information empty.
January 2002
239
7. Click Port Mapping.
The VHDL Symbol Pin to Model Port Mapping dialog box appears.
8. Select the pin CLK in the Pin List column.
9. Select CLOCK in the Model Port[s] column.
10. Click Map.
The Update pin mode dialog box appears. This appears if you are mapping a symbol
pin to a model port of different modes (input to inout, in this case). Similarly, if the types
are different, then the Update pin type dialog box appears. In this dialog box you can
determine whether or not to map the pins of different types. In case you want to suppress
this dialog box, select the Automatically Update pin mode option.
11. Click OK.
Similarly, map the other pins.
12. Click OK.
January 2002
240
Next, determine the generics that should be annotated to the symbols.
13. Click Generics.
The Select VHDL Generics dialog box appears.
14. Select the Annotate on Symbol(s) check box next to Size and TP_CLK_MAX
generics to annotate both the generics on to the symbols.
15. Click OK.
16. To simultaneously create a map file, click Setup.
January 2002
241
The Setup for VHDL Wrapper/Map File dialog box appears.
17. Select the Generate Map File option to create the map file.
18. Click OK.
19. Click OK.
This completes the creation of a VHDL wrapper/map file. You should now save the part.
The vhdl_wrapper is the VHDL wrapper and vhdl_map is the VHDL map view for the
part.
After you create the wrapper, you can verify it by using any VHDL compiler such as
ncvhdl. Part Developer provides you an interface to interact with whichever VHDL
compiler you choose to use.
20. To setup a VHDL compiler to compile the wrapper files, choose Tools > Verify.
21. Select the VHDL Compilation option.
22. Click Options.
The Enter command for VHDL compilation dialog box appears.
23. Enter the command for VHDL compiler in this dialog box. By default, Part Developer
shows ncvhdl.
January 2002
242
Note: ncvhdl is not supplied with PCB Librarian Expert product suite and needs to be
purchased separately.
24. If you have a VHDL compiler, click OK.
The wrapper will be compiled and a report about the verification status will be made
available to you.
Summary
In this chapter, you learned to create VHDL wrapper and map files. In the next chapter you
will learn to create Verilog wrapper and map files.
January 2002
243
January 2002
244
16
Creating Verilog Wrappers and Map Files
Objective
To become familiar with the methodologies and steps involved in creating Verilog wrappers
and map files.
■
Create a Verilog wrapper and map file.
Overview
Concept-HDL generates a netlist that you can use to simulate your logical design using a
Verilog or VHDL based simulator. To generate the netlist, it uses the symbol pin names as the
interface ports for each component used in the design. The interface ports of a component
may be different from the Verilog model’s ports.
Therefore to successfully simulate a design, a mapping is required between the symbol pins
and the model port names. This mapping information is stored in the wrapper and map files.
Creating a Verilog Wrapper/Map File
Task Overview
Create a VHDL wrapper and map file for the 74LS00 part. The Verilog model for the part is
provided in the <your_install_dir>/veriloglib/verilogTTL/74LSTTL
directory. You will need to import the 74LS00 part from the Cadence supplied reference
libraries.
January 2002
245
Steps
1. Launch Library Explorer and open the tutorial_project.cpm project.
2. Import the 74LS00 part from the Cadence supplied reference library.
3. Open the part in Part Developer.
4. Choose File > New > Verilog Wrapper.
The Verilog Wrappers/Map File dialog box appears.
Note: The Verilog model file can be accessed by specifying either the physical path to
the model file or the lib:cell:view structure. To access the model file by using the
lib:cell:view method, ensure that the library definition exists in the cds.lib file.
5. Click browse to choose the Verilog model. For LS00, select the SN74LS00.v file from
the <your_install_dir>/veriloglib/verilogTTL/74LSTTL directory and
click Open.
Next, you need to map the pin names to the port names.
6. Click Port Mapping.
The Verilog Symbol Pin To Model Port Mapping dialog box appears.
You will notice that under the Pin List entry, there are only pins a, b, y and NCs whereas
under Model Ports there are fourteen pins. This is because the part that you have
January 2002
246
created is a sizeable part, and therefore pin names of only one section is visible, whereas
the Verilog model is a flat model and therefore all ports are displayed.
7. Select y from the pin list.
8. Select _1Y from the Model Ports list.
9. Click Map to map the pin to the port.
10. Similarly map a with _1A and b with _1B.
11. Click OK.
Next, determine the parameters to be annotated to the symbol.
12. Click Parameters.
January 2002
247
The Select Verilog Parameters dialog box appears.
13. Select the Annotate on Symbols check box for the parameters that are to be annotated
to the symbols.
14. Click OK.
15. To simultaneously create a Verilog map file, click Setup.
The Setup for Verilog Wrapper/Map File dialog box appears.
16. Select Generate Map File to create a Verilog map file.
17. Click OK.
18. Click OK.
January 2002
248
This creates the Verilog wrapper for the LS00 part. You should now save the part.
After you create the wrapper, you can verify it by using any Verilog compiler such as
ncverilog. Part Developer provides you an interface to interact with whichever Verilog
compiler you choose to use.
19. To setup a Verilog compiler to compile the wrapper files, choose Tools > Verify.
20. Select the Verilog Compilation option.
21. Click Options.
The Enter command for Verilog compilation dialog box appears.
22. Enter the command for Verilog compiler in this dialog box. By default, Part Developer
shows ncvlog.
Note: ncvlog is not supplied with PCB LIbrarian Expert product suite and needs to be
purchased separately.
23. If you have a Verilog compiler, click OK.
The wrapper will be compiled and a report about the verification status will be made
available to you.
Summary
In this chapter, you learned to create Verilog wrapper and map files. This chapter concludes
the tutorial. We hope that you would have got enough insights by now to start working with
the library development tools and develop libraries and parts for your design teams.
January 2002
249
January 2002
250
Index
B
Library Management Use Model 28
Designer 29
Librarian 28
Library Project
Concepts 30
Creating 32
Build area 30
Creating Libraries 39
C
P
Category
Viewing 39
Category File 24
cds.lib file 30
Copying Parts 41
Part Template
Creating 220
Extracting 229
Modifying extracted values 233
Using 223
PCB Librarian Expert Product Suite
Products 13
PCB Librarian Suite
Products 13
D
Build Area 197
Checking Out Parts 209
Creating 199, 201
Integ Area 197
Overview 196
Vault 197
R
refcds.lib file 31
Reference area 30
F
S
Footprints
Viewing 42
Symmetrical Part Creation
Example 104
L
T
Lib-Cell-View Architecture 19
Entity View 22
Package View 20
Part Table View 22
Simulation View 24
Symbol VIew 19
Libraries
Physical Organization 18
Library Explorer
Overview 17
Library Management
Concepts 18
January 2002
Tutorial Samples 15
Types of Projects
Design Projects 27
Library Projects 27
V
Verification
Against Part Template
View Verification 43
251
223
Verilog Wrapper/Map File 245
Creating 245
VHDL Wrapper/Map File 235
Creation 238
Views
Entity View 22
Package View 20
Part Table View 22
Simulation View 24
Symbol View 19
X
XML
Duplicate Pins 216
Importing Part Data 214
JEDEC_TYPE 217
NC Pins 217
Pins with > or 216
Post Import Issues 215
Symbol Interpretation 217
January 2002
252

Library Explorer and Part Developer Tutorial

Transcription

Similar documents

ITW Ramset 1.800.RAMSET6 (1.800.726.7386) www.ramset.com 7

Paymentez User How To Guide en

PinWall Maps Wall map diary

Sharp Triangle Beads instruction

Help Document Open the URL – www.irctc.co.in Enter your login

Mousekeeping Tip Envelopes

TF1200 - Ramset

neovisc_reimbursementassistance info_020513

Halloween Party Invitations

Atlas 5 Edition Quick Guide