OrCAD Capture SIS

Transcription

OrCAD Capture SIS

UNIVERSITI MALAYSIA PERLIS
COURSE NAME
ENGINEERING SKILLS
COURSE CODE
PCT111/ 3
LAB NO.
1-4
LAB MODULE
OrCAD
LEVEL OF COMPLEXITY
1
2
3
4
5
6
KNOWLEDGE
CEOMPREHENSION
APPLICATION
ANALYSIS
EVALUATION
SYNTHESIS
√
√
√
ENGINEERING CENTRE
CONTENTS
Table of Contents
LAB 1: Using OrCAD Capture...................................................................................... 1
LAB 2: Using OrCAD Layout ..................................................................................... 10
LAB 3: Part, Footprint And Updating Design ............................................................. 22
LAB 4: Create a Double Sided PCB ............................................................................ 35
Appendix A : PCB Footprint for LAB 1...................................................................... 38
Appendix B : PCB Footprint for LAB 4 ...................................................................... 39
Appendix C : Circuit for LAB4 ................................................................................... 41
Labaratory Manual for Engineering Skills PCT111
LAB 1: Using OrCAD Capture
OBJECTIVES:
At the end of this session you should be able to:(i)
(ii)
draw a schematic using OrCAD Capture CIS.
do the finishing to the schematic to prepare for creating a printed circuit board
(PCB)
DRAWING SCHEMATICS
1. To begin, you should consider creating a specific folder for your design. Create
the folder in “D:\OrCAD\ECT111_YOURNAME”.
2. Run your OrCAD Capture CIS. To start new project, select menu
File>New>Project as shown in the figure below.
Figure 1.1: The initial window of OrCAD Capture
3. This option will invoke the New Project dialog box, as shown in Figure 1.2 below.
You should name your project as LAB1, and create new project using PC Board
Wizard and select your own project folder as shown in Figure 1.3.
Page | 1
Figure 1.2: New Project dialog window
Figure 1.3: Select directory window
4. Then, PCB Project Wizard dialog box as shown in figure below displays, just click
Next to continue.
Figure 1.4: PCB Project Wizard
Page | 2
5. The next step is to load libraries of parts which will be available to you when you
are drawing the circuit schematics. The dialog box is for adding and removing
libraries is shown Figure 1.5 below. You might add or remove the libraries later,
now click Finish and continue to draw the schematic.
Figure 1.5: Add or remove libraries dialog box
6. Draw the circuit as shown in the Figure 1.6 below.
+9V
R2
47k
U1
NE555
7
DSCHG
OUT
CV
RST
THR
TRG
VCC
3
R3
470
D1
1
TRIGGER
C1
0.01uF
SW1
5
4
6
2
8
GND
R1
10k
LED
C2
100uF
Figure 1.6: Schematic of a 555 Timer Circuit
7. When finish draw the schematic, select all component from the Edit menu or by
pressing Ctrl+A. Then, from Edit menu, click Properties or Ctrl+E to edit the
properties of all the parts. The window as in figure below appears. Choose filter
by Layout. Select Parts tab.
Page | 3
Figure 1.7: Property Editor window
8. Refer to Table 1 given, enter the appropriate footprint for each one of the parts in
the schematic as shown in figure below. Click the PCB footprint cell for any one
of the parts, type the footprint name. Notice that you must recognize physically
how the parts look like in order to specify their correct footprint. Details of the
footprint is given in Appendix A.
Figure 1.8: Specify a PCB footprint
Page | 4
Value
Reference
PCB Footprint
NE555
U1
DIP.100/8/W.300/L.450
SW PUSHBUTTON
SW1
RAD/.300X.250/LS.200/.031
R
R3
AX/.400X.100/.034
R
R1
AX/.400X.100/.034
LED
D1
CYL/D.225/LS.100/.031
R
R2
AX/.400X.100/.034
C
C2
CPCYL1/D.200/LS.150/.031
CAP NP
C1
RAD/CK05
Table 1: Footprint List
Page | 5
FINISHING SCHEMATICS
1. Now, displays the Capture’s project manager window, click schematic page as
shown in the figure below.
Figure 1.9: Project Manager window
2. Annotate the design by choosing Tools>Annotate or by clicking
button from
the toolbar. This is for update the part reference to prepare the netlisting.
Annotate menu window will appear as shown below. Click OK to annotate.
Another dialog appears as shown in figure 1.11. Click OK to continue.
Figure 1.10: Annotating design
Page | 6
Figure 1.11
3. The design must be check for multiple parts of same reference or invalid package
or nets. Design Rules Check (DRC) will do this. Choose Tools>Design Rules
Check or click
button from the toolbar. DRC menu as shown below appear. If
there are errors, dialog box such in figure 1.13 will appear.
Figure 1.12: DRC
Figure 1.13: Error in DRC
4. If DRC does not give any error, proceed by creating netlist for PCB Layout. If
otherwise, you must identify and fix the problems.
Page | 7
5. To view error, you check the error inside your project folder. Open log file called
PCB_YOURNAME.DRC or open session log inside OrCAD capture CIS. Here
are some example shows in the message log.
Error coordinate
Figure 1.13.1: DRC log file message
6. In this log show, Checking for Unconnected Nets. You see there are two
warning. Base on that massage you can check where is the location of error is. It
given the coordinate, with this you can trace where the error is.
7. You will notice the green marker on the unconnected pin in the figure below. This
is called a DRC marker and right now it’s telling me where it found the error. You
can delete the marker by selecting it and pressing the Delete key. Then run a
wire to where it is supposed to go. Every time you fix an error make sure to rerun
the Design Rules Check
Page | 8
Figure 1.13.2: The green marker notice
8. To create netlist for PCB, choose Tools>Create Netlist or click
button from
the toolbar. Netlist menu as shown below display. Select the desired netlist type
by clicking the Layout tab. Click OK to create netlist. Save your design by clicking
OK for the next dialog box.
Figure 1.14: Create netlist for the design
9. Close and save your design.
Page | 9
LAB 2: Using OrCAD Layout
OBJECTIVE:
create a printed circuit board.
(ii)
do placement of the component, manually or automatically routing the board
INTRODUCTION
OrCAD Layout
OrCAD Layout is a powerful circuit board layout tool that has all the automated
functions you need to quickly complete you board. The chart in the figure below
illustrated Layout’s design flow.
Figure 2.1: PCB Design flow-chart
From figure above, by using OrCAD Capture, we can create a Layout-compatible
netlist. This netlist contains much of the design information that Layout uses to
produce the board. Next step is placing components by using OrCAD Layout, we can
either manually route or autoroute the board. As an output, OrCAD Layout will
produces hardcopy on printers and plotters, and also Gerber files for Gerber
Page | 10
photoplotter, and a wide variety of report files. We can preview or even edit a Gerber
files with Layout’s external Gerber editor known as GerbTool.
PCB Consideration
All PCB are divided into layers. OrCAD Layout supports up to 30 routing layers, it
displays the PCB from a top view. Layers can be a copper layers or documentation
layers. Base on this consideration, we need to clarify this particular information such
as numbers of layers, size and shape of the PCB, PCB fabrication plant
specifications that include minimum trace and space width, plating reduction and
available drills.
CREATING A PRINTED CIRCUIT BOARD
1. Run OrCAD Layout program, select options File>New as shown in figure below.
Figure 2.1: Initial window of OrCAD Layout
2. Layout window will appear with Load Template File dialog box as shown in Figure
2.2 below, choose DEFAULT template to use in this design. Template can be
found in folder OrCAD>Layout>DATA.
Page | 11
Figure 2.2: Loading template file
3. Next, Load Netlist Source dialog box appear. You need to load your netlist file
that you have created in the previous session, which is PCB1_YOURNAME.MNL
as shown in figure below.
Page | 12
Figure 2.3: Load a netlist file
4. You will be asking to save your board file, save
PCB1_YOURNAME in your own folder as described below.
your
board
as
Figure 2.4: Saving file
Page | 13
5. If there were no error during AutoECO process, your design will appear to be as
in figure below. However if there are error, Layout might abort the process and
you will need to identify and fix the problem accordingly.
Figure 2.5: View of layout design window
5.1 Resolving missing footprint
i.
If you are in the process of running AutoECO and it is unable to find a
designated footprint, the Link Footprint to Component dialog box
appears. Choose one of the options in the dialog box (described
below) to resolve the error, so that the AutoECO process can
continue.
Figure 2.5.1: Link footprint to component
Page | 14
ii.
Displays the Select Footprint dialog box, within which you can locate
and select the desired footprint, then choose the OK button to return
to AutoECO. Choose the Add button in the Select Footprint dialog box
to add additional footprint libraries, if necessary.)
6. OrCAD design window settings are controlled by system settings and user
settings. To change system settings, select options Option>System Settings.
Dialog box as in figure below display.
Figure 2.6: System Settings dialog window
7. To change user settings, select options Option>User Preferences. Dialog box
such in figure below will appear. Modify the settings according to your
preferences and then click OK.
Page | 15
Figure 2.7: User Preferences dialog window
8. Now, you can start to place the component manually by clicking
button.
Sample of complete placement of the component is shown the figure below.
Figure 2.8: Sample of placed component
Page | 16
9. Choose Obstacles tool using
button, right click in the window and choose
New. Draw the obstacle as shown in figure below.
Figure 2.9: Draw obstacle
10. Left click and then right click on the obstacles, choose Properties. Edit Obstacles
dialog box display as shown in figure below. Select Obstacles Type to Board
Outline.
Page | 17
Figure 2.10: Edit Obstacles dialog window
11. Now, click on the
button to view the spreadsheet and select Layers. A dialog
box such in figure 2.11 appear.
Figure 2.11: Layers dialog box
12. Click on the layer type column of layer name TOP, right click and choose
properties. Select Layer Type to Unused Routing as shown in figure below. Do
the same modification to INNER1 and INNER2 layers. As routing will be on the
bottom layer only, the PCB is a single layer board (single-sided PCB). Click OK
and close Layers dialog box.
Page | 18
Figure 2.12: Edit Layer dialog box
13. In order to begin routing, you need to set net properties, choose the spreadsheet
toolbar again and select Nets. The Nets spreadsheet displays as shown in figure
below.
Figure 2.13: Nets spreadsheet
14. Double click on net you want to edit, the Edit Net dialog box displays as shown in
figure below. Modify the settings that you want and click OK. Try changing the
+9V and GND net width to 20 mils.
Page | 19
Figure 2.14: Edit Net dialog box
15. To route the board automatically, choose Auto>Autoroute>Board. The board will
be route automatically as shown in the sample below. The default color for
bottom layer route is red.
Page | 20
Figure 2.13: Sample of a routing board
16. Next, after the routing is done, choose Auto>Cleanup to smoothes the route on
the board.
17. If there any modification that need to be done to route, you can click on the
button and click on the particular net and do manual routing.
18. Save and close your work.
Page | 21
LAB 3: Part, Footprint And Updating Design
OBJECTIVE:
create new schematic part
(ii)
create new footprint
(iii)
updating design of printed circuit board
Creating New Schematic Part
1. OrCAD capture has more than 20,000 parts available in the library, we may never
need to create our own part. But, however, if we need to, there is a way of
creating our own part in OrCAD Capture. We begin by creating a new library to
store our new part.
Figure 3.1:The Initial Window of Creating Library in OrCAD Capture
2. Run your OrCAD Capture software and create new library by clicking
File>New>Library. A Project Manager Window will appear indicating new
library has been created. Maximize your Project Manager Window if necessary.
Page | 22
Figure 3.2: Project Manager Window
3. Our library need to be saved in our preferred location, therefore, click on the
library name as indicated in figure 2 above, then click File>Save As. A Save As
dialogue box popped-out
Figure 3.3:Save As Dialog Box
Page | 23
4. In the ‘Save As’ dialogue box, select the location and give name to the library as
‘Libary1.olb’. Choose ‘D:\Orcad\your_name\Lab3’ as your destination folder.
Ensure that in ‘save as type’ combo box, ‘capture library (*.olb)’ is selected. Click
‘save’ to save the library. You have created a blank library named as library1 at
this point.
Figure 3.4: Creating New Part Menu
5. In order to create a new part in the library, click the library name in the Project
Manager Window to highlight it, then click Design>New Part. A New Part
properties window will popped-out
Figure 3.5 :New Part Property Window
Page | 24
6. Key in Name and Part Reference of the part as shown in Figure 5 above. Click
OK when finished.
Figure 3.6 :New Part Editing Window
7. Blank part editor as Figure 6 above appears. The dotted line shows the area that
you can use to draw your part. You may adjust its size by clicking at any corner of
it, and drag it to the size you want. Next, click Place>Rectangle and draw the
body outline of your part.
Figure 3.7 :Place Pin Window
8. Click Place>Pin to add pins to the part. When adding pins, dialogue box as in
figure 7 appears. You have to add 2 pins named ‘1’ and ‘2’ to the part, ensure
that the pin shape configured to ‘Dot’ and pin type configured to ‘Passive’. Note
Page | 25
that after adding pin, the pin name appears above the pin line, and the pin
number appears next to its line.
Figure 3.8: Finished Part Design
9. After completion of your work, your part should look like this. Close the part editor
window to go back to project manager window. Ensure that you save your work
when prompted.
Figure 3.9: Orcad Capture Library with the New Part in the list
Page | 26
10. Your project manager window will show that your library now has one part in it.
Click File>Save to save it. At this point you have finished creating your part with
CONN_2 as its name.
CREATING FOOTPRINT
1. Previously you have created a schematic part named CONN_2, this time you
have to create the PCB footprint for the part. In order to do that, you have to
know the exact details of the part, such as the dimension of the body, or the drill
size of the holes. Those information can be found in the datasheet produce by
the manufacturer of the parts. For CONN_2 parts that you have created, use the
following details presented in figure below as your reference in creating the
footprint.
Figure 3.10:CONN_2 Parts Details
2. Run OrCAD Layout program, select Tools>Library Manager. The dialog window
as shown in figure below will appear.
Page | 27
Figure 3.11: Library Manager
3. To create new footprint, click on tab Create New Footprint…, the dialog box as
shown in figure below display. Put CONN_J1 to the Name of Footprint and
choose English as Units. Click OK.
Figure 3.12: Create New Footprint
4. Check your system setting by clicking options>system settings. Ensure that the
following are selected.
Page | 28
Figure 3.13: System Setting
5. At first, you will be given a pin and a few text in your footprint design window. At
first we have to modify the padstack. Click the pin and press escape to release it
back. This is to make the pin to be the current focus object. Open the
spreadsheet>padstacks, a pad stack table appears, with the padstack in use for
pad 1 is highlighted. Modify the pad height and pad width of DRILL and
DRLDWG to the correct drill size of Ø1.3mm
Figure 3.14: Padstack Window
Page | 29
6. Now, you have to add another pin to it. Click spreadsheet on your toolbar, and
click footprint, a footprint window appears. Right-click on ‘Pad 1’ and click new to
add new pin. An ‘Add Pad’ window appears for adding the details of the new pad.
Key in as indicated in the following figure. When you click OK, the pad list and the
footprint design will be updated to reflect the changes you have made.
Figure 3.15: Add Pad Window
7. Next you have to draw the physical border of the part, you use obstacle to draw
them. Click on the obstacle toolbar, right-click on any part of your drawing area,
click new to begin drawing new obstacle. But, before you begin, right-click once
again and choose properties to set properties of your obstacle. Key in the details
as in the following figure.
Page | 30
Figure 3.16: Edit Obstacle Window
8. When finish, click on Save As tab to save your footprint. Dialog box as in Figure
3.4 below display. Click on Create New Library… tab. Create a library name LIB
under your_name folder as shown in Figure 3.5.
Figure 3.17: Save Footprint Dialog Window
Page | 31
Figure 3.18: Create New Library
UPDATING DESIGN
1. Now, run OrCAD
PCB1_yourname.
Capture
program.
Open
your
previous
project,
2. Click Place part and choose Add Library button to add your previously design
part library. Select the library file that have been created before. You may have to
browse to your previous folder to access the file.
3. Select part CONN_2 within your library and place at the input and the output as
shown as figure below.
Page | 32
Figure 3.19: Place Part Window
Page | 33
+9V
+9V
J1
1
2
R2
47k
CONN_2
U1
NE555
7
DSCHG
OUT
CV
RST
THR
TRG
VCC
3
R3
470
D1
1
TRIGGER
C1
0.01uF
SW1
5
4
6
2
8
GND
R1
10k
LED
C2
100uF
Figure 3.20: Place connector to the circuit
4. Edit the properties of both of the connectors, use the same PCB footprint that
you’ve already created as its footprint. For updating purpose, you’ll need to once
again annotate the design and create its new netlist.
5. Using OrCAD Layout, open board from the previous session, the dialog window
as in figure below appear, click Yes to continue.
Figure 3.21: Dialog window that inform changing occurrence in board netlist
6. Your design now has been updated, start placing component and routing as
usual, but this time configure your PCB to be a double layer PCB. Change Layer
Type of layer INNER 1 and INNER 2 to Unused Routing but leaving TOP and
BOTTOM Layer Type to Routing. Start routing the board by choosing autoroute
mode. Save and close your work.
Page | 34
LAB 4: Create a Double Sided PCB
OBJECTIVE:
This lab is an exercise for you. After performing this lab exercise you should be able
to:(i) Create a double-sided printed circuit board
(ii) Produce Gerber files
PROCEDURE
1. Run OrCAD Capture program, draw a circuit as in Appendix B, save the project
as PCB2_yourname into your own folder. List of all the component involve are as
follows.
Table 4. 2: Bills of Materials for circuit in Appendix B
Item
Quantity
Reference
Part
1
8
C1,C3,C8,C9,C10,C11,C12,C13
CAP NP
2
5
C2,C4,C5,C6,C7
C
3
1
J1
CON12
4
3
J2,J3,J4
CON8
5
1
J5
CON2
6
1
P1
CONNECTOR DB9
7
1
R1
R
8
1
SW1
SW PUSHBUTTON
9
1
U1
8051
10
1
U2
2764
11
1
U3
74LS373
12
1
U4
8255
13
1
U5
MAX232
14
1
U6
74LS138
15
1
Y1
CRYSTAL
2. Find the correct footprints for each one of the part by referring to Library Manager
of OrCAD Layout. Verify with instructor before proceed to the next step.
3. When finish, start annotating and create netlist for the schematic.
4. Open OrCAD Layout program, load netlist file and save the board as
PCB2_yourname.
5. Do the placement of the component.
Page | 35
6. When finish, view the spreadsheet and select Layers. Change Layer Type of the
layer INNER1 and INNER2 to Unused Routing but leaving TOP and BOTTOM
layer type to Routing.
7. Start routine the board by choosing autoroute mode.
8. When finish, select Auto>Design Rule Check. Dialog box as in figure below
appear. Click OK to run DRC.
Figure 4.1: Check Design Rules
9. If there are no errors, proceed with creating Gerber files for the board. Select
Options>Gerber Setting…to view the settings, for post process settings select
Options>Post Setting…
10. To produce Gerber files for the board, select Auto>Run Post Processors. Click
OK to both of the dialog boxes that appear as shown below.
Figure 4.2
Page | 36
Figure 4.3
11. To view a Gerber file of the design, from OrCAD Layout window, select
Tools>GerbTool>Open. Choose file PCB2_YOURNAME and click OK. Show the
PCB2_YOURNAME-GerbTool window to the instructor for verification.
12. Save and close your work.
Page | 37
Appendix A : PCB Footprint for LAB 1
Page | 38
Appendix B : PCB Footprint for LAB 4
SM/C_0805
BLKCON.100/VH/TM1SQ/W.100/12
CPCYL1/D.200/LS.100/.031
BLKCON.100/VH/TM1SQS/W.100/8
DSUB/VS/TM/9
SM/R_0805
Page | 39
DIP.100/40/W.600/L2.025
SOJ.050/28/WB.450/L.700
SOJ.050/20/WB.450/L.500
SOJ.050/16/WB.450/L.400
RAD/.400X.150/LS.200/.034
Page | 40
Appendix C : Circuit for LAB4
VCC
C1
U1
31
19
CAP NP
SW1
SW PUSHBUTTON
C2
C
Y1
CRY STAL
C3
18
9
CAP NP
R1
R
P0.0
P0.1
P0.2
P0.3
P0.4
P0.5
P0.6
P0.7
EA/VP
X1
X2
RESET
P2.0
P2.1
P2.2
P2.3
P2.4
P2.5
P2.6
P2.7
J1
1
2
3
4
5
6
7
8
9
10
11
12
CON12
1
2
3
4
5
6
7
8
12
13
14
15
P1.0
P1.1
P1.2
P1.3
P1.4
P1.5
P1.6
P1.7
INT0
INT1
T0
T1
RD
WR
PSEN
ALE/P
TXD
RXD
39
38
37
36
35
34
33
32
D0
D1
D2
D3
D4
D5
D6
D7
21
22
23
24
25
26
27
28
A8
A9
A10
A11
A12
A13
A14
A15
17
16
29
30
11
10
RD
WR
PSEN
ALE/P
U2
A0
A1
A2
A3
A4
A5
A6
A7
A8
A9
A10
A11
A12
10
9
8
7
6
5
4
3
25
24
21
23
2
ROM
PSEN
20
22
27
1
VCC
3
4
7
8
13
14
17
18
1
11
VCC
1
2
3
6
4
5
A
B
C
G1
G2A
G2B
Y0
Y1
Y2
Y3
Y4
Y5
Y6
Y7
15
14
13
12
11
10
9
7
ROM
IO
5
36
9
8
35
6
IO
Q0
Q1
Q2
Q3
Q4
Q5
Q6
Q7
A0
A1
A2
A3
A4
A5
A6
A7
2
5
6
9
12
15
16
19
OC
G
74LS373
D0
D1
D2
D3
D4
D5
D6
D7
PA0
PA1
PA2
PA3
PA4
PA5
PA6
PA7
RD
WR
A0
A1
RESET
CS
PB0
PB1
PB2
PB3
PB4
PB5
PB6
PB7
PC0
PC1
PC2
PC3
PC4
PC5
PC6
PC7
74LS138
D0
D1
D2
D3
D4
D5
D6
D7
4
3
2
1
40
39
38
37
1
2
3
4
5
6
7
8
18
19
20
21
22
23
24
25
1
2
3
4
5
6
7
8
14
15
16
17
13
12
11
10
1
2
3
4
5
6
7
8
J2
CON8
VCC
C6
C4
C
J3
CON8
C5
C
C7
U5
1
3
2
C+
C1V+
C2+
C2V-
4
5
6
C
C
11
10
12
9
J4
CON8
T1IN
T2IN
R1OUT
R2OUT
T1OUT
T2OUT
R1IN
R2IN
14
7
13
8
MAX232
1
6
2
7
3
8
4
9
5
A13
A14
A15
U6
RD
WR
A0
A1
D0
D1
D2
D3
D4
D5
D6
D7
CE
OE
PGM
VPP
U3
D0
D1
D2
D3
D4
D5
D6
D7
8051
U4
34
33
32
31
30
29
28
27
11
12
13
15
16
17
18
19
O0
O1
O2
O3
O4
O5
O6
O7
2764
ALE/P
D0
D1
D2
D3
D4
D5
D6
D7
A0
A1
A2
A3
A4
A5
A6
A7
A8
A9
A10
A11
A12
8255
P1
CONNECTOR DB9
VCC
J5
C8
CAP NP
C9
CAP NP
C10
CAP NP
C11
CAP NP
C12
CAP NP
C13
CAP NP
1
2
CON2
Title
<Title>
Size
Document Number
Custom<Doc>
Date:
Wednesday , August 12, 2009
Rev
<Rev Code>
Sheet
1
of
1
Page | 41

OrCAD Capture SIS

Transcription

Similar documents

shark pocket knives - Hardware Merchandisers

OrCAD Sigrity ERC Datasheet

The Sustainability Crisis

Printed Circuit Board Design Manual

Read More - RedRibbon Days

TARGET 3001! CrashCourse2

Assembly Instruction

Water Footprint - Universidade Federal de Santa Catarina

PJSIP - eLinux.org

Orcad Tutorial - NED University of Engineering and Technology

Cadence OrCAD 16.6 Release

An OrCAD Tutorial

OrCAD Capture CIS - EMA Resource Center