What`s New in Mastercam X4

Transcription

What’s New
in Mastercam X4
May 2009
Be sure you have the latest information!
Information might have been changed or added since this document
was published. The latest version of this document is installed with
Mastercam or can be obtained from your local Reseller. The ReadMe
file (ReadMe.htm) includes the latest information about new
features and enhancements.
II • WHAT’S NEW IN MASTERCAM X4
Mastercam® X4 WHAT’S NEW IN MASTERCAM X4
Date: May 2009
Copyright © 2009 CNC Software, Inc.— All rights reserved.
First Printing: May 2009
Software: Mastercam X4
Part Number: X4-Pack-WN
TERMS OF USE
Use of this document is subject to the Mastercam End User License
Agreement. A copy of the Mastercam End User License Agreement
is included with the Mastercam product package of which this
document is part. The Mastercam End User License Agreement can
also be found at:
www.mastercam.com/legal/licenseagreement/
III
Contents
Introduction ................................................................................................. 1
Before You Begin ..................................................................................... 1
 If You Need More Help ............................................................................ 2
 Additional Documentation ...................................................................... 2

General System Enhancements......................................................... 3
Dynamic Planes ....................................................................................... 3
 Tutorial: Using the dynamic gnomon to set a plane .......................... 4
 Dynamic Xform ...................................................................................... 11
 Tutorial: Moving geometry using Dynamic Xform............................ 11
 Wireframe Feature Recognition in Chaining ....................................... 17
 Tutorial: Chaining geometry using wireframe feature recognition ... 17
 User-Defined Setup Sheet .................................................................... 22
 Level Manager Improvements .............................................................. 23
 Managing Levels on the Status Bar..................................................... 25
 Viewsheet Enhancements .................................................................... 25
 File Translator Updates ......................................................................... 26

Design Enhancements .......................................................................... 27
Translate 3D Improvements .................................................................27
Trim Divide/Delete .................................................................................28
 New Visual Cues for Trimming............................................................. 28


Mill Level 1 Enhancements ................................................................ 29
New Tree-Style Dialogs for 2D Toolpaths ........................................... 29
 Dynamic Mill .......................................................................................... 30
 Holder Definition in 2D Toolpaths ........................................................ 31

IV • WHAT’S NEW IN MASTERCAM X4
FBM Drill .................................................................................................32
 Tutorial: Machining a large hole with FBM Drill ..............................32
 Tutorial: Mapping hole sizes to drill cycles .....................................36
 FBM Mill .................................................................................................41

Mill Level 3 Enhancements ................................................................45
Multi-Threading Support .......................................................................45
 Toolpath Refinement..............................................................................47
 Tutorial: Adjusting toolpath results using Toolpath Refinement .......47
 Minimum Tilt in Multiaxis Toolpaths ...................................................54
 New Tree-Style Dialogs for Curve 5-axis and Drill 5-axis ..................54
 Circle Mill 5-axis Toolpath ....................................................................55

Router Enhancements ..........................................................................57
Bump Nesting.........................................................................................57
 Tutorial: Adjusting nesting results using Bump Nesting...................57
 Vertical and Horizontal Cutoff in Nesting .............................................63

Lathe Enhancements .............................................................................65
Grooving Enhancements .......................................................................65
 Create Turn Profile .................................................................................69
 New Tree-Style Dialogs for C-axis Toolpaths .....................................70
 Round Boring Bar Display in Verify ......................................................71

Wire Enhancements ..............................................................................73

Agievision Workflow .............................................................................73
Post Enhancements ...............................................................................75
Updating Posts for Mastercam X4 .......................................................75
 Support for Lathe Tool Inspection ........................................................76
 Agievision Support.................................................................................77
 New Operation Parameters ..................................................................78
 Post Debugger Improvements ..............................................................78

Introduction
Welcome to Mastercam X4! Mastercam X4 features a new suite of CAD/CAM tools
focused on delivering speed and efficiency for your machining jobs. We are sure that
you will benefit from what Mastercam X4 has to offer you and your shop.
You can quickly access some of Mastercam X4’s new and exciting features through the
What’s New toolbar and menu. Go to Help, What’s New in the Mastercam menu to
view some of the new functions that Mastercam X4 offers.
Notes:
• If you migrate your toolbar settings from a previous version of Mastercam, the
What’s New in X4 toolbar will not be available.
• Some of the options on the What’s New toolbar are only available if you have
certain products enabled on your Mastercam SIM.
Before You Begin
What’s New in Mastercam X4 outlines the new features in each Mastercam product
level. Each chapter’s title corresponds to the Mastercam product that contains the
features. For example, the Mill Level 1 Enhancements chapter discusses new
functionality that you can access in Mastercam X4 Mill Level 1 or higher.
Tutorial Requirements
Many chapters in this book contain short tutorials on new features in Mastercam X4.
To complete these tutorials, you should meet the following requirements:
 You must be comfortable using the Windows® operating system.
 You must have installed your Mastercam X4 products. All tutorial files are
located in the ..\Documentation\ExampleParts folder of your
Mastercam installation.
 Start Mastercam using your preferred method:
 Double-click Mastercam’s desktop icon.
Or
 Launch Mastercam from the Windows Start menu.
2 • WHAT’S NEW IN MASTERCAM X4
If You Need More Help
There are many ways to get help with Mastercam, including the following:
 Mastercam Help—Access Mastercam Help by selecting Help, Contents from
Mastercam’s menu bar or by pressing [Alt+H] on your keyboard. Also, most
dialog boxes and ribbon bars feature a Help button
Help directly to related information.
that opens Mastercam
 Online help—You can search for information or ask questions on the
Mastercam Web forum, located at www.emastercam.com. You can also find a
wealth of information, including many videos, at www.mastercam.com and
www.mastercamedu.com.
 Mastercam Reseller—Your local Mastercam Reseller can help with most
questions about Mastercam.
 Technical Support—CNC Software’s Technical Support department (860-8755006 or [email protected]) is open Monday through Friday from 8:00
a.m. to 5:30 p.m. USA Eastern Standard Time.
 Documentation feedback—For questions about this or other Mastercam
documentation, contact the Technical Documentation department by e-mail
at [email protected].
 Mastercam University—CNC Software sponsors Mastercam University, an
affordable, online learning tool with more than 180 videos to let you master
your skills at your own pace. For more information on Mastercam University,
please contact your Authorized Mastercam Reseller, visit
www.mastercam.com, or email [email protected].
Additional Documentation
You can find more information on using Mastercam in the following materials, located
in the \Documentation folder of your Mastercam installation:







Mastercam X4 Installation Guide
Mastercam X4 Administrator Guide
Mastercam X4 Quick Start
Mastercam X4 Reference Guide
Mastercam X4 Transition Guide
Mastercam X4 Quick Reference Card
Mastercam X4 Wire Getting Started Guide
General System Enhancements
Mastercam X4 introduces several features to improve your productivity, no matter
what level of Mastercam you own.
Dynamic Planes
Dynamic Planes is a new method for defining construction planes (Cplanes), tool
planes (Tplanes), planes, and work coordinate systems (WCS) in Mastercam X4. You
can now define the desired plane using an interactive graphical gnomon to establish
the plane's origin and orientation.
Everything centers on using the gnomon and its position-sensitive functionality. The
gnomon is made of an Axis Origin and three axes, each consisting of a First Leg, Axis
Label, Second Leg, and Axis Arrowhead. Each piece has its own functionality.
1 Axis Origin - Select to place the origin of the gnomon in 3D space. You can use
AutoCursor positions, type in XYZ values, or sketch a point. Generally, this is
the first manipulation of the dynamic gnomon.
2 First Leg - Select to move the gnomon along the selected axis. Move the
gnomon along the scale displayed in the graphics window. You can also use
AutoCursor positions, type in XYZ values, or sketch a point.
3 Axis Label - Select to rotate around a perpendicular axis. Rotate the gnomon
along the scale displayed in the graphics window. You can also use AutoCursor
positions, type a rotation angle, or sketch a point.
Selecting the axis label for rotation follows these rules:
 X axis label = rotate around Y
 Y axis label = rotate around X
 Z axis label = rotate around X
4 Second Leg - Select to rotate around a perpendicular axis. Rotate the gnomon
along the scale displayed in the graphics window. You can also use AutoCursor
positions, type a rotation angle, or sketch a point.
Selecting the axis second leg for rotation follows these rules:
 X second leg = rotate around Z
 Y second leg = rotate around Z
 Z second leg = rotate around Y
5 Axis Arrowhead - Select to align the gnomon to existing geometry. You can also
use AutoCursor positions to place the gnomon on an entity. You may align the
gnomon to:
 a line or solid edge
 tangent to a spline or arc
 normal to a surface or solid face
TIP: You can modify the behavior of the gnomon with the Gnomon Settings
dialog box. Access this dialog box by clicking the Settings button on the ribbon bar
or dialog box or by holding the [Ctrl] key and right-clicking anywhere in the
graphics window.
 Using the dynamic gnomon to set a plane
1 From the Mastercam menu, choose File, Open.
2
Go to ..\Documentation\ExampleParts and select
DYNAMIC_PLANES.MCX.
3 Press [Alt + S] to shade the surface in the file.
GENERAL SYSTEM ENHANCEMENTS • 5
4 Choose Planes, Dynamic planes from
the status bar.
The Dynamic Plane dialog box displays
and the dynamic gnomon appears in the
graphics window. The first step is to
position the plane’s origin.
5 Move the gnomon around the graphics window. The gnomon picks up on
various AutoCursor positions on the wireframe geometry.
6 Move the gnomon to the left end of the
spline, and click once to set the origin.
Sliding the Gnomon
1 Click on the first leg of the Y axis. A sliding scale displays along the Y axis.
2 Move the gnomon back and forth along the scale. Notice that the value in the
Y field of the Dynamic Plane dialog box updates as you move the gnomon.
TIP: You may also use AutoCursor positions, type in XYZ values, or simply
sketch a point to set an axis position.
3 Click the Settings button on the Dynamic Plane dialog box to display the
Gnomon Settings dialog box. You can adjust the gnomon behavior here,
including snap increments and gnomon size.
4 Set the Linear increment to 10 and choose OK.
TIP: If you deselect the Activate Linear Snap check box, you can position the axis
anywhere along the scale, not just at the snap positions.
5 Move the Y axis along the scale again. Notice that the scale increments are now
different.
6 Move your cursor to the center point of the circle. The gnomon references the
AutoCursor position and uses it as the value for the Y position.
7 Click the right-hand end of the spline to set the gnomon.
Rotating the Gnomon
1 Click on the Y axis label. A dial displays
and you can now rotate around the X
axis.
2 Click to select a position.
Note: The red increments on the dial
indicate the rotation angle.
3 Click on the second leg of the Y axis. You can now rotate around the Z axis.
4 Enter 45 in the Rotation field on the Dynamic Plane dialog box, and press
[Tab]. This quickly rotates the Y axis by 45 degrees.
5 Click once anywhere in the graphics window to set the Y axis position.
6 Click on the second leg of the Y axis again, and move your cursor to the corner
of the shaded surface. The gnomon tilts to align with this point.
7 Click the 2D/3D switch on the status bar
at the bottom of the screen to change to
2D mode.
8 Move your cursor again to the corner of the shaded surface. The point projects
down to the flat plane you are rotating within.
9 Click again on the 2D/3D switch to return to 3D mode.
10 Click once anywhere in the graphics window to set the Y axis position.
Aligning an Axis
1 Click on the Z axis arrowhead, and move around the graphics window. The Z
axis snaps to align with each piece of geometry. Notice how the axis adjusts to
changes in the surface normal of the shaded surface.
2 Slide the Z axis along the spline and press [F] to flip the Z axis at various points
along the spline.
3 Press and hold the [Ctrl] key, and click the right button on your mouse to
display the Gnomon Settings dialog box.
4 In the Axis Alignment group box,
deselect the Line option. This section
sets what types of geometry Mastercam
considers when aligning an axis.
5 Click OK to close the Gnomon settings dialog box.
6 Move the gnomon around the graphics window. Notice that the gnomon no
longer snaps to align the Z axis with the line.
7 Select any position for the gnomon, and click once to set the axes.
8 Click OK on the Dynamic Planes dialog box to complete the function. The
New View dialog box displays.
9 Type a name in the Name field, and select the Set as WCS option.
10 Choose OK. The WCS, tool, and construction planes are now set to your new
plane.
Dynamic Xform
Imagine being able to translate and rotate geometry in a single, on-screen control.
That's what the new Dynamic Xform function offers you. It combines the ease of the
new graphical gnomon from Dynamic Planes with the power of Mastercam’s Xform
features.
 Moving geometry using Dynamic Xform
2
DYNAMIC_XFORM.MCX.
3 Press [F9] to display the world origin and axes. Notice that the part is not in a
standard Mastercam orientation.
4 Press [F9] again to clear the world axes from the graphics window.
5 Choose Xform, Dynamic Xform from the
Mastercam menu.
6 Select the solid part, and press [Enter].
7 On the Dynamic Xform ribbon bar, confirm that you are in Move mode and
are creating a single copy.
Positioning the Gnomon
The first task is to orient the gnomon to the way you want to move the part.
1 Click to place the gnomon origin on the
bottom left corner of the part.
2 Click the Manipulate axes button on the
Dynamic Xform ribbon bar. This allows
you to continue positioning the gnomon.
3 Click on the Y axis label to position the Y axis.
TIP: The icon next to the cursor indicates
whether you are in Manipulate axes mode
or Manipulate geometry mode. You can
press the [Ctrl] key to switch between modes.
4 Move the cursor to the top left corner of
the part. A Visual Cue displays when
Mastercam snaps to the endpoint.
5 Click on the endpoint to set the Y axis
position.
6 Click on the X axis label to start
positioning the X axis.
7 Move the cursor to the bottom right corner of the part. A Visual Cue displays
when Mastercam snaps to the endpoint.
8 Click on the endpoint to set the X axis position.
Moving the Geometry
1 Click the Manipulate geometry button
on the Dynamic Xform ribbon bar. This
allows you to move the selected
geometry.
2 Click on the first leg of the X axis and slide from side to side to translate the
part along the X axis.
TIP: You can also enter a translation position on the Dynamic Xform ribbon bar.
3 Click anywhere along the scale to position the X axis.
4 Click on the axes origin, and move the cursor around the graphics window to
start translating the part to a new origin.
5 Click anywhere in the graphics window to select a new origin position.
6 Click on the Z axis label, and notice that you can rotate around the X axis.
7 Enter -110 in the Angle field of the
Dynamic Xform ribbon bar, and press
[Tab] to position the Z axis.
8 Click once in the graphics window to return to the Dynamic Xform ribbon bar.
9 On the Dynamic Xform ribbon bar, select
World axes, and click the Align with
Axes button. This aligns the geometry
with the world coordinate system.
10 Select World origin from the Move to
origin drop-down list, and click the
Move to origin button.
11 Click OK on the Dynamic Xform ribbon bar to complete the transformation.
12 Right-click in the graphics window, and choose Clear Colors to return the part
to the original color.
13 Press [F9] again to see that the part is now moved to the world origin and
oriented to match the standard Mastercam views.
Wireframe Feature Recognition in Chaining
On wireframe parts with many similar chains mixed with other geometry, chaining can
become a tedious, error-prone, manual process. With Wireframe Feature Recognition,
you only chain an example of the geometry you want to use and then click a button.
Mastercam automatically finds all other occurrences of the geometry and chains them
as well. You can use this function to select specific holes for Circle Mill toolpaths or for
slots to cut with Pocket or Contour toolpaths.
 Chaining geometry using wireframe feature recognition
2
Go to ..\Documentation\ExampleParts and select WIREFRAME.MCX.
This example contains over 850 individual shapes.
3 Press [F1] and draw a zoom window around the left side of the part.
4 Choose Analyze, Contour from the Mastercam menu. The Chaining dialog
box displays.
5 Click the Chain Feature Options button
to display the Chain Feature dialog box.
This dialog lets you set criteria for
determining which geometry is similar.
6 Select Identical in the Feature Precision
group box. This option looks for chains
that are exact geometric matches. The
chains must contain the same number of
entities with the same measurements.
7 Click OK to close the Chain Feature dialog box.
8 Chain the small horizontal slot on the
left side of the part.
9 Click the Chain Feature button on the
Chaining dialog box.
Notice that Mastercam selects all of the identical geometry in the graphics
window. The prompt indicates that 72 chains are selected.
10 Click the Chain Feature Options button again.
11 Select the Shape Match option in the
Feature Precision group box. This option
looks for chains that are similar in shape.
The selected chains can have the same
features and arrangement of features but
differ by size.
12 Click OK to close the Chain Feature
dialog box.
13 Chain one of the kidney shapes on the
part.
14 Click the Chain Feature button again on
the Chaining dialog box.
Notice that Mastercam found the identical shapes, along with similar shapes
that are smaller and larger.
15 Click the Chain Feature Options button again.
16 Select the Shape Perimeter filter option
in the Feature Precision group box, and
select <= (less than or equal to) from the
drop-down list. This option looks for
chains that are the same size or smaller
than the selected chain.
17 Click OK to close the Chain Feature
dialog box.
18 Chain one of the larger circles on the
part.
19 Click the Chain Feature button again on the Chaining dialog box.
Notice that Mastercam chained all arcs that are less than or equal to the
reference arc. In total, Mastercam chained 620 shapes with just a few clicks.
TIP: You can save your Chain Feature settings and recall them for future use by
choosing the Save and Load buttons on the Chain Feature dialog box.
User-Defined Setup Sheet
There is a new setup sheet available in Mastercam X4. The new ActiveReports™ setup
sheet can be enabled in the Toolpaths page of the System Configuration dialog box.
The GUI and .SET options are also still available.
The new setup sheet lets you add project and customer information, including custom
screen captures. You can even add drafting and notes while you're capturing images.
Level Manager Improvements
In Mastercam X4, the Level Manager is easier to use and more powerful than ever. The
dialog box has been reorganized so it requires less screen space. In addition, you can
press [Alt + Z] to quickly open and close the Level Manager.
The Level Manager also allows you to perform more level manipulation inside the
dialog box by using new options on the right-click menu.
 Purge empty levels - Removes levels and level names that contain no
geometry.
 Renumber level - Moves entities to an unused level while maintaining the
level name, level set, and display status.




Cut - Removes geometry from a level and keeps it available for pasting.
Copy - Copies geometry from a level.
Paste - Places the cut or copied geometry into a level.
Delete - Removes geometry from a level. You can also press the [Delete] key.
Since this is a delete function, Undo and Redo are available.
Managing Levels on the Status Bar
The level name is now displayed along with the level number on the status bar. If you
open the drop-down list, all of the levels and descriptors are displayed using the same
List Level settings from the Level Manager.
You can enter a level name in the status bar when you define a new level by typing the
level number followed by a colon and the name. For example, to define level 10 as a
new level with the name cavity, type 10:cavity (no spaces) in the Level box on the
status bar.
Viewsheet Enhancements
In Mastercam X4, you can recall every option on the status bar (except Groups) as part
of a viewsheet. Right-click on any viewsheet tab and choose Settings to specify which
status bar functions to recall in the viewsheet and which ones to ignore. The
Automatically restore bookmark settings option resets the viewsheet to the
bookmark automatically when you switch from one viewsheet to another. All of these
options are also available on the Screen, Viewsheets page of the System Configuration
dialog box.
File Translator Updates
The following list shows which file formats are supported by Mastercam X4’s file
translators.











ACIS - R19
Alibre Design - V11
AutoCAD® DWG, DXF, DWF - 2009
Autodesk Inventor IPT, IAM, IDW - 2010
CATIA® V5 - R19
KeyCreator® - V8.5
Parasolids® - 20
Pro/E® - Wildfire4
Rhino® - 4
Solid Edge® - ST
SolidWorks® - 2009
Design Enhancements
Mastercam X4 Design makes drawing and editing your geometry more efficient than
ever before.
Translate 3D Improvements
The Xform, Translate 3D function has been revamped in Mastercam X4 to make it
faster and more efficient. If you are moving or copying geometry to a pre-defined plane,
you can just select the name from the drop-down list.
Trim Divide/Delete
This useful function now can delete any isolated entities with no intersections. Entities
with a single point of intersection at an endpoint are also automatically deleted.
New Visual Cues for Trimming
When trimming entities, Mastercam X4's auto-preview feature displays the results of
the selected function as you move the mouse over the final entity selection. A solid line
represents what geometry will be created. A dashed line represents what geometry will
be removed.
Mill Level 1 Enhancements
Mill Level 1 in Mastercam X4 features an improved interface for 2D toolpaths, new
machining strategies, and enhancements to the Feature Based Machining (FBM)
toolpaths.
New Tree-Style Dialogs for 2D Toolpaths
Mastercam X4 continues the migration to the tree-style dialogs and the 2D toolpaths
are the next to get this facelift. You will not notice any differences in the Mastercam
menus. However, when you select a contour or a drill operation, a new interface
displays. Operations that require chains are organized together and toolpaths that
require points or arcs are organized together.
The following toolpaths now use the tree-style dialogs:
 Contour
 Slot Mill
 Point
 Pocket
 Drill
 Helix Bore
 Facing
 Circle Mill
 Thread Mill
One of the benefits of this interface, beyond a unified look with other toolpaths, is the
ability to change toolpath types. If you begin a drill toolpath from the menu, select
several points or arcs, get into the interface and realize that Drill was not the correct
option but Circle Mill is better, you can simply switch styles and continue on. There is
no need to exit the toolpath and begin again — all geometry remains selected. You
enter the appropriate parameters, and process the toolpath.
Dynamic Mill
Dynamic Mill is a new pocketing routine for Mastercam X4. It has been added to the 2D
HST tree-style dialog as an additional toolpath type.
MILL LEVEL 1 ENHANCEMENTS • 31
Dynamic Mill gives you the ability to utilize the entire flute length of the cutting tool,
saving both time and money. It also offers flexible retract options to keep the tool down
in smaller parts and rapid retract on larger parts.
In addition, Dynamic Mill supports many powerful entry methods, including a custom
entry method that makes it easier to program complex pocket shapes. Micro lifts have
been incorporated from the Peel Mill toolpath to further refine the dynamic pocket
motion and avoid excessive heat build-up. Both the powerful entry methods and the
micro lifts support custom feeds and speeds to further productivity and generate safe
motion.
Holder Definition in 2D Toolpaths
All 2D toolpaths that use the new tree-style dialogs (point-based, chain-based, and 2D
high speed) include a Holder page in the tree control. This page is similar to 3D high
speed toolpaths, but the information is only used for Backplot and not for gougechecking the toolpath.
FBM Drill
Large Hole Milling
Customers asked for a better solution to the problem of machining holes larger than
their drills and for creating flat-bottom holes without using a mill for drilling. FBM
Large Hole Milling is designed to answer this need. With it, you can set thresholds for
through holes, counterbores, and flat-bottomed blind holes when FBM Drill will switch
from using a drill cycle to using Circle Mill or Helix Bore toolpaths.
 Machining a large hole with FBM Drill
2
Go to ..\Documentation\ExampleParts and select LARGE_HOLE.MCX.
This part features a one inch hole in the center that is too large to drill
effectively.
3 From the Mastercam menu, choose Toolpaths, FBM Drill.
4 Click the Detect button at the top of the
FBM Drill dialog box to find the holes in
the part.
The one inch hole appears at the bottom of the feature list and is set to be
drilled by default.
5 Select the Hole milling page from the tree control and select the Through
holes check box.
This page includes options to determine what holes are machined with either
a circle mill or helix bore toolpath instead of drilling. In this case, any through
holes one inch or larger will be machined with a circle mill toolpath.
6 In the Automatic tool selection group
box, enter 35% for the maximum tool
diameter and 20% for the minimum tool
diameter.
7 Select the Circle Mill page from the tree control. This page allows you to set
parameters for the circle mill toolpath or use the default toolpath parameters.
8 Click the Detect button again to re-detect the holes. Notice that the one inch
hole is now re-assigned as a circle mill operation.
9 Click OK to accept the Circle Mill default values and generate the toolpaths.
Mastercam creates a circle mill toolpath to machine the hole in the center of
the part.
Hole Mapping
FBM Drill now allows you to build a mapping table so that when a specific hole size is
encountered during detection, it is automatically assigned to a specific drill cycle and
tool. This can be useful on parts where holes that are intended to be tapped are created
with the pilot hole diameter rather than the finished hole diameter.
 Mapping hole sizes to drill cycles
2
HOLE_MAPPING.MCX.
The circular set of holes are all ¼-20 tapped holes drawn with a 0.201
diameter.
3 From the Mastercam menu, choose Toolpaths, FBM Drill.
4 Click the Detect button at the top of the
FBM Drill dialog box to find the holes in
the part.
5 Select the Hole Mapping page from the tree control and select the Hole
mapping check box to enable this feature.
6 Right-click anywhere in the hole mapping table and select Add to start a new
hole map entry.
7 Enter 0.201 for the diameter and press [Tab] to move to the next column.
8 Select Tap RH from the Hole type drop-down list and press [Tab] to move to
the next column.
9 Select the MCX: Tap RH tool from the Finish tool drop-down list to complete
the hole map entry.
10 Click the Detect button again to re-detect all of the features. All of the 0.201
holes are now set as Tap RH holes instead of Drill holes.
Notice that the counterbore features were not automatically assigned to a tool.
You can quickly make this adjustment.
11 Click the Select common features check box at the bottom of the feature list
and select one of the counterbore holes. All the counterbores are highlighted.
12 Right-click in the Finish tool column on the right and select Finish tool >
MCX: Drill from the flyout menu. This tool is applied to all the counterbore
holes.
13 Click OK to generate the toolpaths.
Pre-Drilling
FBM Drill now includes a simpler way for pre-drilling to only drill the pilot hole
diameter and not perform any pre-drilling up to that hole size. The Pre-drill pilot holes
only check box on the Pre-drilling page generates only pilot hole pre-drill cycles
followed by finish hole drill cycles, such as tapping or reaming.
Create Additional Geometry
This new option on the Setup page allows FBM Drill to create additional geometry
while creating the drill toolpaths. This geometry can be used to select holes for
multiaxis drilling. The Vector of drill engagement option creates a vector from the top
of the hole to the deepest depth of the hole, taking tip compensation and tool selection
into account.
FBM Mill
Slug Cutting
Users who work with wood and composite materials on large vacuum table machines
will definitely appreciate this enhancement in how FBM Mill handles through pockets.
FBM Mill now detects when a through pocket area is large enough for a vacuum table
to hold down the resulting slug. Instead of pocketing the entire area, Mastercam uses a
contour operation to cut the outermost passes of the profile, leaving behind a slug that
is held in place by the vacuum table.
Note: The Slug cutting page is available only when the Through features check box
is selected on the Feature detection page.
Large Hole Milling
In Mastercam X4 Mill, FBM Mill provides a method other than pocketing to machine
round features. The Hole Milling option lets you mill round features using pocket,
Circle Mill, or Helix Bore toolpaths. You can activate Hole Milling on the Feature
detection page.
If you select Hole milling, the Hole milling page becomes available in the tree control.
Use this page to select either Circle Mill or Helix Bore toolpaths for machining and to
set tool selection ranges. Like Large Hole Milling in FBM Drill, you can set parameters
for the Circle Mill or Helix Bore toolpaths, or use the operation defaults.
Mill Level 3 Enhancements
Mastercam X4 offers several enhancements for Mill Level 3 and Router Pro users,
including support for multi-threaded processing, new filters for improved finish
results, and an updated interface for Curve 5-axis and Drill 5-axis toolpaths.
Multi-Threading Support
Multi-threading is a special form of program multitasking that allows a single program
to execute portions of itself concurrently (as opposed to a single-threaded program,
which executes in a linear mode). This processing mode allows Mastercam to split the
programs that regenerate its largest, most complex toolpaths into smaller, separate
program threads that execute simultaneously. Programs that are multi-threaded can
process more quickly and efficiently.
In Mastercam X4, multi-threaded toolpath processing is available for all of
Mastercam's 3D surface high speed toolpaths (HST), and for the following multiaxis
toolpaths:
 Multisurface 5-axis
 Flowline 5-axis
 Port 5-axis
You can enable/disable multi-threaded toolpath processing as part of your Mastercam
configuration for all Mastercam sessions (Settings, Configuration, Toolpaths page).
Or you can use the Toggle Multi-Threading button to turn it on or off for the
current Mastercam session.This button is located on the What’s New in X4
toolbar, and in the Settings, Customize dialog box in the Multi-Thread
Toolpath Manager category.
Once you activate multi-threaded processing, whenever you generate/regenerate 3D
HST and multiaxis toolpaths, you can continue working in Mastercam once the
toolpaths have been sent to the Multi-Threading Manager (MTM). This dialog box
shows you all existing threads, along with their current states, progress bar indicators,
and processing status.
You do not have to wait for the toolpath regeneration to complete before starting
another Mastercam function. Mastercam continues to process these toolpath files in
the background.
You can use the Toggle Multi-Threading Manager button to control the
display of this dialog box for the current Mastercam session. This button is
also located on the What’s New in X4 toolbar, and in the Settings, Customize
dialog box in the Multi-Thread Toolpath Manager category.
When processing toolpaths in multi-threaded mode, the Toolpath Manager displays
two icons to indicate that toolpaths are being processed as threads in the MultiThreading Manager. The icons are green or yellow spools of thread.


Green icons indicate threads that are being processed in the MTM.
Yellow icons are assigned to dependent toolpath threads (for example,
rest toolpaths). Dependent threads require data from prior “parent” toolpath
threads. Dependent threads cannot begin processing until the MTM
completely finishes processing the parent thread (including translation of the
binary NCI data).
Toolpath Refinement
Mastercam X4 adds a new toolpath refinement feature — 3D Advanced Toolpath
Refinement — to 3D surface toolpaths. The 3D Advanced Toolpath Refinement helps
you optimize cycle times and produce better finishes with your 3D surface toolpaths.
This new feature combines the existing arc/line filter with new functionality that
supports smoothing, randomizing points, creating minimal points, maintaining a
consistent distance between points, and even converting arc motion to all G1 motion.
 Adjusting toolpath results using Toolpath Refinement
2 Go to ..\Documentation\ExampleParts and select REFINE.MCX. This
part includes four surface high speed toolpaths.
3 In the Toolpath Manager, expand the first toolpath in the list.
4 Click the Parameters icon to display the Surface High Speed Toolpaths dialog
box.
5 Select the Arc Filter/Tolerance page from the tree control. Notice that the
Total tolerance value is set to 0.001.
6 Click the Refine toolpath button to open the Refine Toolpath dialog box.
In the Tolerances Distribution section, Mastercam displays the formula it uses
to apply the 0.001 Total Tolerance value. For this toolpath, the percentages of
Line/Arc filter tolerance and Smoothing tolerance are set to 0%, making the
Cut tolerance 100% of the Total tolerance value. This indicates that the 3D
Advanced Toolpath Refinement feature is not in effect.
7 Select the Smoothing Settings check box to activate smoothing for the
toolpath. This automatically adjusts the Smoothing tolerance in the
Tolerances Distribution to 5% of the Total tolerance and reduces Cut tolerance
to 95%.
8 Select the Line/Arc Filtering Settings check box to activate line/arc filtering
for the toolpath. Line/arc filtering and smoothing tolerance are applied
approximately equally.
9 Slowly move the + slider, located immediately after the Cut tolerance field, to
the right. This adjusts the ratio between the two sections in 5% increments,
but respects the final number for the total tolerance.
10 Move the slider in between the line/arc filter and the smoothing tolerance to
the left. This adjusts the ratio between the two fields.
Notes: There are other ways to change the distribution between the fields:
• Type values directly into the fields
• Use the sliders in the My preferences section.
11 Click Cancel to close the Refine Toolpath dialog box.
12 Click Cancel to close the Surface High Speed Toolpath dialog box.
Examining the Toolpath Results
1 Select all four toolpaths in the Toolpath Manager and click the Backplot
button.
2 Expand the Backplot dialog box using
the arrow button in the upper left corner
so you can see all four toolpaths.
3 Select the first toolpath.
4 Select the Display Endpoints button to
see the entity endpoints within the tool
motion.
5 Zoom in on a section of the part. The first toolpath has no filter applied, so you
can see how the points line up with neighboring points. This introduces the
potential for a low-quality surface finish.
6 Select the second toolpath in the Backplot dialog box. The Refine Toolpath
filter is turned on for this toolpath, which randomizes the point placement to
avoid patterns.
7 Select the third toolpath in the Backplot dialog box and notice the reduction in
the number of points. For this toolpath, the Minimize number of points
option in the Smoothing section is selected, which further filters the toolpath
and creates smaller NC files.
8 Select the last toolpath in the Backplot dialog box. This toolpath uses the Use
Fixed Segment Length option in the Smoothing section. No two points are
more than 0.04 inches apart, which is ideal for high speed machining.
9 Click OK to close the Backplot dialog box.
Toolpath Refinement Frequently Asked Questions
Mastercam X4’s Toolpath Refinement gives you a single control panel for two powerful
methods of toolpath improvement. The first method — Line/Arc Filtering — you may
already be familiar with. The second method of toolpath refinement — Smoothing — is
new to Mastercam.
Note: The Cut Parameters Smoothing option used to round corners in high speed
toolpaths is unrelated to 3D Advanced Toolpath Refinement.
Here are a few commonly asked questions that should help you decide if the new
Smoothing feature is for you:
Which toolpaths use Toolpath Refinement?
All 3D surface toolpaths and surface high speed toolpaths have the option of using
Toolpath Refinement. This includes both roughing and finishing toolpaths.
What does Toolpath Refinement Smoothing do?
Smoothing distributes a toolpath’s node points, avoiding the clustering and grouping
of points that can cause marks and other imperfections. It does this through shifting,
removing, and/or adding node points along an already generated toolpath.
What are the benefits?
Smoothing delivers three clear benefits on certain parts:
 Superior finish quality. Tests show a much smoother, consistent finish with
fewer visible tool marks on many parts.
 Reduced machining time. Smoothed toolpaths eliminate many of the small
moves common to 3D toolpaths, letting you run the program at much higher
feed rates.
 Reduced tool wear.
How do I access the Refine Toolpath options?
Choose a 3D surface toolpath or a surface high speed toolpath from the Mastercam
Toolpath menu or toolbar.
Then choose one of the following actions based on your toolpath selection:
For tree-style toolpaths:
1 Choose the Arc Filter/Tolerance page.
2 Enter a Total Tolerance value.
3 Click the Refine Toolpath button.
For tab-style toolpaths:
1 Choose the toolpath's parameters tab (for example, Rough radial parameters
or Finish project parameters).
2 Enter a Total Tolerance value.
3 Click the Total Tolerance button.
Try out this powerful new technique and see for yourself the smoother, faster results it
can deliver. You can also use it together with Mastercam’s standard Line/Arc filtering, as
the two techniques work well together.
Minimum Tilt in Multiaxis Toolpaths
This new feature automates tool axis motion when the tool or holder encounters a
potential collision with a selected surface. These options are available in Port 5-axis,
Flow 5-axis, and Multisurface 5-axis toolpaths. You can enter a clearance distance to
maintain between the tool shank/holder and the part. For Mastercam X4, this function
can only be used with a lollipop cutter.
New Tree-Style Dialogs for Curve 5-axis and Drill 5-axis
Mastercam continues to convert toolpaths to the new tree-style dialog boxes. The new
dialogs for Drill 5-axis and Curve 5-axis streamline the programming process.
Circle Mill 5-axis Toolpath
The new Circle Mill 5-axis toolpath is useful for creating circular pockets normal to a
surface, parallel to a line, or referencing a plane in order to insert an object such as a
fastener. It can also generate round holes at any orientation where drilling is not
desirable. You can access this toolpath by choosing Toolpaths, Multiaxis, Circle 5 axis
from the Mastercam menu.
Router Enhancements
Mastercam X4 Router provides new functions that give you additional control over
your router machining jobs.
Bump Nesting
Mastercam X4 allows you to perform automatic nesting with just enough manual
intervention to achieve the best possible result in the least amount of time.
 Adjusting nesting results using Bump Nesting
1 From the Mastercam menu, choose Settings, Configuration and select the
English (Inch) configuration file.
2 Click OK to close the System Configuration dialog box.
3 Choose Xform, Geometry Nesting from the Mastercam menu.
4 Click the Open button at the bottom of the Nesting dialog box.
5 Go to ..\Documentation\ExampleParts and select BUMP.NSTX. This
file contains settings from a previous Mastercam nesting session.
On the Sheets tab, the sheet size is preset to 24x12 inches and the sheet
margin is set to 0.25 inches.
6 Click on the Parts tab. Two copies of each part have been requested, using a
0.25 inch part-to-part distance to accommodate tool size.
ROUTER ENHANCEMENTS • 59
7 Click OK to create the nesting results. The Nesting Results dialog box displays.
8 Click the Drag button at the bottom of
the Nesting Results dialog box to enter
Bump Nesting mode.
The graphics window shows the nested
geometry and the Bump Nesting ribbon
bar displays.
Copying and Rotating Part Geometry
1 Click the Copy button on the ribbon bar.
2 Click anywhere on the number 4 shown in the following picture.
3 Use your mouse to move the copied geometry around the open area on the
right side of the sheet. You can see that the part-to-part distance is respected.
4 Press the [+] and [-] keys to rotate the part ten degrees in either direction.
5 Hold down the [Ctrl] key and press the [+] and [-] keys again to rotate the part
one degree in either direction.
6 Move the new geometry down next to the lower number 4. Notice that it can
be difficult to align with both the number 4 and the lower edge of the sheet.
7 Press and hold the left mouse button. An additional arrow displays that can be
pointed towards the bottom edge of the sheet to bump against two edges.
8 Release the left mouse button to place the copied geometry.
Deleting and Moving Part Geometry
1 Click the Delete button on the ribbon
bar.
2 Click on the number 4 that you just created to delete it from the sheet.
3 Click on the letter E at the center of the nested geometry.
4 Press [Esc] to exit Delete mode.
5 Click the Move button on the ribbon bar.
6 Click on one of the letter C parts and try to drag it into the space left in the
center of the sheet. Due to the part-to-part distance, it will not fit in the space.
7 Click anywhere on the right side of the sheet to place the letter C.
8 Click on one of the number 4 parts and
move it to the open space in the center of
the sheet. Because this part is smaller,
Bump Nesting allows you to place it in
the space.
TIP: You can press the [+] and [-] buttons
to rotate the part within the space for more
efficient sheet usage.
9 Click once to place the part.
10 Click OK on the ribbon bar to return to
the Nesting Results dialog box.
The Minimum Quantity Not Achieved dialog box displays because you
deleted one of the letters and a minimum quantity of two was set for each
part.
11 Click OK to continue.
12 Click OK to accept the nesting results and complete the nesting process.
Vertical and Horizontal Cutoff in Nesting
Nesting can now generate a toolpath for vertical and horizontal cutoffs in order to
preserve rectangular remnants for future use. If you wish to make horizontal and
vertical cutoffs, you can use the Trim settings to choose which cut to make first. The
horizontal and vertical trim check boxes in the Results dialog are used to specify which
cuts to make.
Lathe Enhancements
Mastercam X4 Lathe provides many new features to make your lathe jobs faster and
more efficient, including several enhancements for grooving toolpaths, better
functionality for creating turned profiles, and a user-friendly interface for C-axis
toolpaths.
Grooving Enhancements
Mastercam X4 includes several improvements that provide a new level of control for
Lathe grooving toolpaths.
Multiple Chains Grooving Option
The new Multiple chains option allows you to select more than one groove for a groove
toolpath.
When you use this option to chain multiple grooves, the chaining function is impacted
in the following ways:




The type of chain in the Chaining dialog box defaults to Partial Chain.
You are prompted to select an entry point or chain the inner boundary.
Using the Partial Chain method, select the first entity and then the last entity.
Using the Point method, select an entry point or points.
You can then select a retraction point or complete the chaining process.
Because the grooves can be different widths, you can only select the new Middle
overlap option on the Groove Finish parameters tab.
LATHE ENHANCEMENTS • 67
Feed and Speed Settings for Finish Passes
New parameters in Mastercam X4 Lathe allow you to set speeds and feed rates
specifically for finish groove passes, making it easier to produce your desired finish.
Corner Dwell on Finish Grooving
The Groove finish parameters page now includes a Corner Dwell option. The dwell
occurs at the intersection of the wall or corner geometry and the flat bottom of the
groove. Dwell may not work in odd-shaped grooves.
Independent Feed Rate for First Plunge
The Groove rough parameters page has a new option to set a feed rate specifically for
the first plunge move, providing precise control of your toolpath motion.
Tool Inspection
Mastercam X4 Lathe also provides the ability to program tool inspections into your
groove toolpaths. You can program safe approach and retract locations for performing
the tool inspection. You can also define specific conditions for when you want to
inspect the tool.
IMPORTANT: This feature only works if the post is customized to capture the new
information in the NCI file. For more information, see Support for Lathe Tool
Inspection on page 76.
Create Turn Profile
Customers asked for a better solution to the problem of generating a turned profile
from a solid. Mastercam X4 includes a new function for doing this, which replaces the
Solid to 2D Profile function in Mastercam X3. The Turn Profile functionality is a subset
of the Create, Silhouette Boundary functionality.
You can access this new function by selecting Create, Turn Profile from the Mastercam
menu. After you select an existing solid, solid face, or surface, the following dialog box
displays.
Two methods are available for generating the turned
profile:
Spin — Designed for complex, non-symmetrical
geometry containing Mill and Turn features. The entire
model is spun to generate the profile of the maximum
turned envelope for the component. This option can
also be used on symmetrical geometry.
Slice — Designed for symmetrical, revolved geometry
and a simple slice is taken through the model.
The final profile can be limited to the Upper or Lower
profiles or both sides. The new function always uses the
current WCS X axis as the axis of rotation and the
resulting profile is created in the Top view of the active
WCS.
New Tree-Style Dialogs for C-axis Toolpaths
Since C-axis toolpaths are very similar to the 2D chain-based and point-based
toolpaths, these toolpath dialog boxes are also being converted to the new tree-style
dialog. This will help maintain consistency between Mastercam Mill and Mastercam
Lathe.
Round Boring Bar Display in Verify
Mastercam X4 now shows round boring bars in Verify. The display is a simplified
representation of round tools, including boring bars. Collision checking is performed
in the background against the 2D profile as it has always been.
All boring bar-type tools, including any custom boring bars, are now created with the
new, simplified round representation. For other tool types like General, ID groove, and
ID thread, the option to create a round tool shank is available.
Wire Enhancements
Mastercam X4 Wire provides a new, customized interface if your wire machining
processes include using Agie EDM with Agievision controls.
Agievision Workflow
In Mastercam X4 Wire’s new Agievision mode, the wirepaths and related dialog boxes
are intentionally designed to closely resemble the actual Agievision interface for a
familiar look and ease of use. This new Agievision support also includes a complete set
of machine definition/control definition/post processor files. You can identify these
files by the _AWF in the file names.




AGIE GENERIC AGIEVISION_AWF 4X WIRE.WMD
AGIE GENERIC AGIEVISION_AWF 4X WIRE MM.WMD
AGIE GENERIC AGIEVISION_AWF 4X WIRE.CONTROL
AGIE GENERIC AGIEVISION _AWF 4X Wire.PST
Select one of the Agievision AWF Wire Machine Definitions (WMD files) to switch
Mastercam Wire into the Agievision mode. Once you switch to this mode, the Toolpaths
menu shows the following wirepaths:
As you go through the pages in the wirepath dialog boxes, you will see the Agievisionspecific parameter pages that anyone familiar with the Agievision will instantly
recognize.
Notes:
• Mastercam X4 still includes the Agie C-Hook. This means that you can still run
and maintain your current Agie C-Hook files using your current Agie machine
definition and post.
• Since these new Agievision wirepaths are Agievision-specific, they are not
compatible with existing wirepaths that have been created with the Agie CHook. The part geometry can be reused, but all the wirepaths must be recreated
using the new interface.
Post Enhancements
Mastercam X4 includes a number of post enhancements that support the other new X4
features. Your \Documentation folder includes two additional resources for posts
information:
 Post Debugger User’s Guide — Describes how to use the post debugger,
including a tutorial example and quick reference.
 NCI & Parameter Reference — Lists all of the NCI codes and associated
parameters, 20000s-series codes, and all the operation parameters. It includes
procedures and examples for accessing each type of value.
Updating Posts for Mastercam X4
All posts need to be updated before they can be used with Mastercam X4. Use the
UpdatePost C-Hook to update them. This is installed in your \chooks folder and is run
like any other C-Hook. If you try to use a post that has not been updated, Mastercam
displays an error message.
UpdatePost will make the following changes to your post:
 The header will be updated with the latest version number, 13.00.
 String initialization will be updated to conform to current best-practice
standards.
The following picture shows the new string initialization. All such statements will use
the : operator, with the string value in double-quotes " ". This also applies to blank
strings.
UpdatePost also includes routines that search for references to specific parameter
numbers and validates them against known changes. If your original post tries to read a
parameter with a number that has changed, the following line will be written to the
updatepost.log file:
PARAMETER DATA - - Possibly incorrect parameter number detected:
99999. Please check the parameter number.
When you see this message, look up the parameter number in the tables in the NCI &
Parameter Reference and make sure that your post is actually referencing the
parameter that you want.
Note that UpdatePost only looks at parameter numbers in fprm tables. Postlines that
are inside postblocks are not validated. Here is one example:
pparameter$
if prmcode$ = 10068, z_stock = rpar(sparameter$, 1)
Support for Lathe Tool Inspection
The generic lathe posts supplied with Mastercam have been modified to support the
new tool inspection retract moves for lathe groove toolpaths. To implement this
feature, there are two enhancements to the NCI output for lathe groove toolpaths:
 A retract move to the inspection position. This is indicated by the same 70000
cur_cflag$ (rpd_typ$ = 7) used for the Mill tool inspection feature in the
surface high speed toolpaths.
 A comment that is written to the NCI just before the 70000 move. A new 29999
NCI code has been created for this comment.
Unlike other 20000s lines, which are written to the NCI before the tool change line, the
29999 is written in the middle of the toolpath, at the point where the tool inspection is
to take place.
The following picture shows the NCI code for a lathe groove toolpath, with and without
the tool inspection. You can see how the retract move and new codes are implemented.
POST ENHANCEMENTS • 77
If you are not using one of Mastercam’s generic lathe posts, you (or your reseller) will
need to modify your post to properly process the new NCI codes. UpdatePost will not
make these changes for you. See the NCI & Parameter Reference for detailed
instructions and examples.
Agievision Support
The Agievision interface introduced with Mastercam X4 includes many new dialog
boxes that mimic the look and feel of the Agievision control. A new range of parameters
has been established, 22000–22999, to encapsulate these settings and pass them to the
post. These are then read and stored during pparameter$ like any other 20000-style
parameters.
This represents a significant change from how Agie data was written out by the Agie CHook used in Mastercam X3. The C-Hook wrote the data to a separate .ADT file to be
read by the post, instead of the 22000 parameters. Posts written for the new Agievision
interface therefore need to be completely different.
The Agievision interface supplied with Mastercam X4 includes a complete post, along
with a machine and control definition:




AGIE GENERIC AGIEVISION_AWF 4X WIRE.WMD
AGIE GENERIC AGIEVISION_AWF 4X WIRE MM.WMD
AGIE GENERIC AGIEVISION_AWF 4X WIRE.CONTROL
AGIE GENERIC AGIEVISION _AWF 4X Wire.PST
When you select the Agievision machine definition, the correct post is automatically
loaded.
The new Agievision interface also includes a new control definition page that supplies
key information to the post.
This information is used to validate the post and ensures that the selected post has
been properly configured for the interface. This means that any current Agie posts
(posts that had been developed to work with the Agie C-Hook) will not work with the
new interface.
See the NCI & Parameter Reference for detailed lists of all the new 22xxx parameters and
other information about the Agievision post.
New Operation Parameters
Mastercam X4 includes many new operation parameters to support the new toolpath
types and other new features. These new parameters are itemized in the NCI &
Parameter Reference.
Traditionally, operation parameters have been numbered from 10000–19999. Since we
are running out of numbers in this range, new parameters are now numbered in the
40000s.
Post Debugger Improvements
The Mastercam Post Debugger, which was introduced in Mastercam X3, has several
significant enhancements.
 Run Turbo mode - Lets you quickly preview your NC output so you can set
breakpoints, add variables to the watch list, and otherwise identify areas of
interest that you want to look at closely.
 Expanded NC Output - Lets you see each element of each NC line as it is
output, and identify the specific postline element or statement that output it.
In addition, the documentation has been significantly enhanced, including a quick
reference, FAQ, and tutorial example. Click the new Help button on the debugger
toolbar, or open the Post Debugger User’s Guide directly from the \Documentation
folder.

What`s New in Mastercam X4

Transcription

Similar documents

Editing CNC Code

Bmp2MC - MR Soft

Importing 3D Toolpaths

KeyCeator Machinist Datasheet

Mastercam Getting Started Series

Mastercam Getting Started Series

Getting Started Series Tutorials

Getting Started with Mastercam Lathe

Free Information - Tech Directions

What`s New in Mastercam 2017

Vectric Cut 3D (Frogmill)

PDF

Mastercam Getting Started Series

Getting Started with Mastercam Mill-Turn