Mastercam® Maintenance Release 0304

Overview

Mastercam Maintenance Release 0304 is released to distribution March 2004. It contains both new features and enhancement/corrections to the following CNC products: Design, Mill, Router, and Wire.

New Features

3-axis constant Z milling

Enhancements and Corrections

New Features

New Advances for 3-Axis Constant-Z Milling

Mastercam's March 2004 Maintenance release delivers a select but exciting preview of the upcoming Mastercam X. With the March Maintenance release, Mastercam users can experience a dramatic boost in speed and reliability in creating constant Z toolpaths, and can take advantage of a series of new tool motions.

Faster Constant Z Toolpaths

The March 2004 Maintenance release delivers dramatically faster processing time for important Z-level toolpaths:

Rough Pocket
Rough Contour
Finish Contour
Rough Restmill

Generation times for these toolpaths can be reduced by amounts ranging from 10% all the way up to 75% or more, depending on the cut. The most dramatic increases are in Rough Contour and Finish Contour, where users can easily drop three-quarters or more from their processing time, getting parts to the machine faster than ever before.

Below you will see the results of time tests we performed on a variety of parts. To make sure that we put the software through its paces, we chose a variety of complex models built from a fairly large number of surfaces with real tolerances and settings.

Previous Calculation time: 883 seconds

New calculation time: 248 seconds

Calculation time improvements: 71%

Toolpath type: Multisurface Finish Contour

Surfaces: 2,250

Cut tolerance: .001"

Tool: .75" ball

Stepdown: .05"

Previous Calculation time: 655 seconds

New calculation time: 184 seconds

Calculation time improvements: 70%

Toolpath type: Multisurface Rough Pocket - Parallel Spiral

Surfaces:3,647

Cut tolerance: .001"

Tool: .75" ball

Stepdown: .1"

Mastercam's new Z-level cutting techniques also deliver a better finish on STL files. Traditionally, STL files can result in a faceted finish. Mastercam's new strategy can yield results as high quality as toolpaths created from a surfaces or a solid model.

Smoother High-Speed Multisurface Pocketing

The March 2004 Maintenance release also includes a sample of some exciting new high-speed motion that will be expanded on in Mastercam X. We've introduced two new elements to high-speed multisurface pocket machining that will help ensure smoother transitions and reduce interrupted cuts.

Current multi-surface pocket toolpaths use a constant stepover. When a small island of uncut material lies outside those tool moves, the tool makes a small diversion to clean out that area, then continues on with the cut. With the new version, users have a "variable stepover" option. This will automatically adjust the stepover to reduce small uncut areas, helping ensure that the cut remains uninterrupted.

Transition between pocketing passes is also important to high-speed machining, and this has been improved as well. The current strategy is a looping transition that eliminates sharp angular moves. While beneficial for high-speed machining, this technique disengages the tool from the material for a short time. The new version creates true tangential motion between cuts, reducing tool movement and ensuring that the tool stays engaged in the material.

Great news for Multi-axis users

Mastercam Mill 9.1 MR 0304 introduces significant new capabilities for Multi axis toolpaths.

Shank and holder avoidance

Without doing anything more than just defining the tool with its shank and holder, Flow 5-axis, Multisurface, Curve 5-axis, and Swarf toolpaths will be gouge-checked to avoid all check surfaces. The shank protection includes definitions that are both larger and smaller than the tool shank or arbor.

Shank and Holder Collision Detection

This function applies to CHECK surfaces in:

· Curve5ax

· Swarf5ax

· Flow5ax

· Msurf5ax

The tool shape defined in the DEFINE TOOL dialog is used for checking. The tool profile will be visible and accurate in backplot.

The holder is also defined in the DEFINE TOOL dialog. The tool holder is implemented as an additional cylinder above the tool. It is not displayed in backplot. The tool holder displayed in backplot by activating “Show hold” is not used for checking.

Surface Gouge Removal

Flow 5-axis (and only Flow 5-axis) has an additional option to check the tool, shank, and holder against the drive surfaces as well, but not Comp surfaces. It is activated by checking the “Check Flowline motion for Gouge” checkbox on the Flow5ax parameters page.

· With the box unchecked, everything, except Check Surfaces should be the same as before this was added

· With the box checked, “fish tails” from the tool going into small corners should be removed.

Approach and retract motion is also being checked to avoid gouges.

This new gouge protection applies to the following tool types:

· Flat End Mills

· Ball End Mills

· Bull End Mills

· Slot End Mills

· Lollipop Mills

· Tapered Flat End Mills

· Tapered Ball End Mills

· Tapered Bull End Mills

Undercuts are allowed with any of the tools above. Full radius slotting mill works correctly. If corner radii are used, the tool is positioned relative to the tool nose.

Fishtail gouges have been eliminated in Flow5-axis when the “Check flowline motion for Gouge” is activated on the Flow5ax Parameters dialog box.

The Reference point option on the Tool Parameter dialog box has also been activated for 5-axis toolpaths.

Approach and retract motion is also being checked to avoid gouges.

The surface side is now important for CHECK surfaces when Stock on Check Surfaces is used.

The “negative stock larger than the tool corner radius” limit has been removed for CHECK surfaces. This allows negative stock on flat end mills.

Undercuts are allowed on CHECK surfaces.

rev2rev C-Hook

Date: 09 October 2003

Programmer: CNC Software, Inc.

Description:

Convert a single surface to a new surface. This C-Hook allows the patches of the new surface to be created from a fixed number (in U and V) rather than from a chordal deviation. This is useful for reverse-engineered surfaces (those made from some sort of scanning or digitizing process). Such surfaces often have a very large number of patches and some noise. This C-Hook allows the number of patches and the noise to be significantly reduced.

Input

Surface - the surface must be untrimmed and not offset.

Number of patches in U

Number of patches in V

Output

Output is a new surface on the main level in the main color. The original surface may be kept or deleted.

swept2r C-Hook

Date: 08 January 2004

Programmer: CNC Software, Inc.

Description

Modify an existing Swept 2D operation to allow a choice of zigzag or one-way cutting and to allow roughing passes.

Input

There must be at least one Swept 2D operation and only one such operation must be marked "selected" in the Operation Manager.

Dialog box description

Zigzag or one way cut method radio button toggles cut method.

Rough passes checkbox turns rough cuts on or off.

Start, End, and Step Z values define the rough cuts. (Start is highest.)

Order cuts using the Depth checkbox. If checked, the rough cuts will be output by depth, first. If unchecked, the rough cuts will be output by Z level, first.

Output

The one selected Swept 2D operation will be modified and locked.

TCPoint C-Hook

Date: Original version 01/14/04

Programmer: CNC Software, Inc.

Additional files required: TCPoint.TXT and TCPoint.PRM

Purpose

To convert ‘plain’ point entities into Wire Thread or Wire Cut type points. Also allows for changing the Color and/or Level when the point type conversion occurs.

Note:

Works only with Mastercam Wire V9.1

How to use:

TCPoint.DLL can be run as any Mastercam C-Hook.

For convenience, we recommend that you add “TCPoint” be added to the Wire system menu structure on the menus that appear when you select Thread/Cut on the Secondary Menu. The edits to Wire9.TXT shown below will place the “TCPoint*” command on the Next menu sub-menu of Thread/Cut.

To add the C-Hook to that sub-menu:

Note: Always save a backup copy of the original WIRE9.TXT file before making changes!

To add TCPoint to the menu, you will change one line near the end of the Wire9.TXT file.

In the example below, the original Menu 2 line that appears in the Wire9.TXT file is commented out. The altered Menu 2 line containing the new command is just below the original line (commented out with a #).

[Wire Create Point]
menu 1 {"Point:", "&Position", "Along &ent", "&Node pts", "&Cpts NURBS",
"&Dynamic", "&Length", "Pe&rp/dist", "Small &arc", "Pt &style", "Ne&xt menu"}
#menu 2 {"Point:", "&Grid", "&Bolt circle", "&Slice", "Srf pro&ject"}
menu 2 {"Point:", "&Grid", "&Bolt circle", "&Slice", "Srf pro&ject", "TC&Point*"}
1. "TC"
2. "THREAD"
3. "CUT"
4. "Point style = "

This change to the Wire9.TXT will alter the ‘Next menu’ menu to appear as follows.

Selecting TCPoint* from this menu will execute the TCPOint C-Hook, and display the TC Point menu (Primary Menu):

Note: If it does not display, make sure that you have spelled the name correctly and have the required trailing asterisk (*).

If you click Thread or Cut in the TC Point menu, Mastercam displays the standard Select Points options menu so that you can select points to be converted into Thread or Cut points using See the Selection Menu.

Mastercam continues to redisplay the TC Point menu so that you can convert additional points to Thread/Cut points, until you select Done.

If you select Settings on the TC Point menu, Mastercam displays the TC Point Settings menu:

Here you can alter the default Color and/or Level applied to the converted points.

Note: These setting are valid only during the current execution of the TC Point C-Hook.

Menu summary

Primary Menu	Selection Menu	Settings Menu

Set the default startup Color and Level settings by editing the TCPoint.PRM file. Note that this is the only way to alter the startup settings of the TCPoint C-Hook. We assume that most users will leave the PRM settings as shown below or use a single common setting of their own choosing.

# 'TCPoint.PRM'

# Default configuration settings for the 'TCPoint.DLL' C-Hook

[Thread_Cut]

1 -2 ' Thread Point Color : 0-255 or (-1 = use Main Color, -2 do not change color)

2 -2 ' Cut Point Color : 0-255 or (-1 = use Main Color, -2 do not change color)

3 -2 ' Geometry level : 1-255 or (-1 = use Main Level, -2 do not change level)

Design Issues Addressed in Maintenance Release MR0304

Translators - AutoCAD / ACIS / SAT

Reference #	Description
25077	Updated ACIS translator to handle more files.
24887, 24723	Improved handling of levels in files with Solids where no level information exited.
24863	Added support for Inventor 8 files.
24684	Improved support of DXF polyface mesh.
24555	Improved handling of DWG files with embedded double percent (%%) signs.
24487	Added support for DIMLFAC in Linear Dimensions in DWG files.
24413, 24412 24297 24192	Improved Solid handling in DWG files.
24411	Improved handling of files with True Type notes containing more than 1024 characters.

Translators - Pro-E

Reference #	Description
24643, 24477 24432, 24359 24346, 24280 24278, 24245 24222, 24213 24131	Improved handling of NURBS faces

Translators - Parasolids / SolidWorks / Solid Edge

Reference #	Description
25093	Implemented Solid Edge V15 part reader API.
24842	Improved handling of pre-SW2000 files.
24610, 24575 24560	Improved the reading of imported bodies.

Translators - IGES

Reference #	Description
24911, 24601	Improved degenerate edge processing on triangular surfaces.

Translators - STEP

Reference #	Description
23991	Improved translation of STEP files into surfaces.

Misc. Design functionality

Reference #	Description
24613	Improved handling of printer line widths greater than 5.
23807	Improved detection of infinite loops due to reversed tangents with Surface Extend.

Mill Issues Addressed in Maintenance Release MR0304

3D Surface Machining

Reference #	Description
25105 25104 24175 23148 14269	Finish, Contour, shallow, add cuts Improved when corner rounding is used.
25027	Finish, Contour, Entry/Exit Improved gouge checking.
24981	Finish, Shallow Improved toolpath memory allocation.
24939	Finish Parallel Improved toolpath edge roll gouge checking.
24918	Finish, Contour Significantly improved the speed of optimize cut order. .
24912	Rough, Pocket Improved tool containment issues after facing.
24892,24728	Rough, Pocket Improved gouge checking with ramp entry.
24873	Improved handling of tool containment boundaries when an outside condition fails and an “out of memory” error appears.
24871	Ensured that the cut tolerance is properly maintained when using flat or bullnose tools and relatively loose tolerances.
24623	Finish, Parallel Removed extra tolerance moves when “follow surface gap” motion is used.
24618	Finish, Constant Scallop Improved gouge checking when large stepovers are used.
24590	Leftover Added support for filtering.
24538	Finish, Shallow Removed “Toolpath allocation too low” message by correctly allocating storage to include vertical cut segments.
24152	Eliminated tool circle drawing when toolpath display is turned off.
24075	Addressed issues with toolpath display when levels are turned off.

Multi-Axis Machining

25073	Swarf Improved rapid collision detection.
25062	Swarf Improved handling when multiple passes are active but set with 0 passes.
25032	Swarf Improved handling of non-visible levels when creating toolpaths.
24925	Multi-Surf Improved depth cut order processing.
24820 24807 24569	Swarf Improved the checking of boundary points array for wraparound.
24804	Drill 5-axis Improved 4-axis output.
24741	Flow 5-axis Improved 4-axis output reliability.
24740 24739 24679 24636	Flow 5-axis Improved multi pass reliability with 4-axis output.
24619	Flow 5-axis Improved shank behavior.
24604	Swarf Removed previous limits of 32,500 tool positions.
24579	Multi-axis Improved WCS support.
24578	Multi-axis Improved stepover and step along limits.
24533	Drill 5-axis Added new reference point application logic.
24483	Swarf 4-axis Improved gouge protection.
24463	Curve 5-axis Added radial offset absolute value range validation.
24462	Curve 5-axis Addressed issues with a combination of vector length, compensation, and negative stock.
24313	Swarf 4-axis Improved error message when user settings don’t allow for a toolpath on the selected geometry.
24267	Improved handling of contour start and end flags.
23859	Swarf Improved suppression of backup moves.

Misc Mill Issues

Reference #	Description
25015	Operations Manager Improved repaint when levels with toolpaths are not visible.
24526 24474 24334	Graphical Setup Sheet Improved time reports by improving handling of arcs in views other than top.
24344	Pocket Improved pocket facing with islands.
24225	Contour 3D Added check for 3D chamfer contour type so previous depth is saved.
24209	Contour, Adjusted lead in and out Improved handling of this function with full circles.

Router Issues Addressed in Maintenance Release MR0304

Reference #	Description
23994 23796 24379	Router9.exe Improved the “change startpoint dynamic” option to work with tabbed contour toolpaths through the Chain Manager.
25090	Router9.exe Improved handling of skewed arcs in geometry nesting.
n/a	MCAMVB Improved the way we automate block drill toolpaths to work more consistently with different flavors of imported geometry.
n/a	Nesting.dll Major speed enhancements. Preliminary testing on a typical cabinet job is functioning up to five times faster than Version 9.1 SP2.
24908 24520 24408	Nesting.dll Updated toolpath nesting to improve sorting capabilities.
n/a	MCATP Added additional nesting parameters and sorting controls to the user interface.Uses new grid control for improved interaction. Added an option to Mastercam and KCDw ATP to use either the top of the table OR the top of the part as the Z origin.
n/a	KCDwATP Added additional nesting parameters and sorting controls to te user interface. Uses new grid control for improved interaction. Added an option to Mastercam and KCDw ATP to use either the top of the table OR the top of the part as the Z origin.
n/a	MCNestingToolpaths Added additional nesting parameters and sorting controls to the user interface. Uses new grid control for improved interaction. Allows read/write of file listings to and from XML file.
24661	Engrave Updated to work with XP Themes.

Wire Issues Addressed in Maintenance Release MR0304

Reference #	Description
22496	No Core path with wire compensation in control The final rough pass move and final finish pass move could violate the part boundary if the lead-in/out line was not at least as long as the wire radius + overburn value. Added a warning message to inform the user and guide correction.
22837	Selection of thread/cut points with windows chaining When window chaining, if there were “non” thread/cut points at the same location as a selected thread/cut point, Mastercam would issue the warning message: Wire thread warning! Unequal number of thread points and wirepaths. Several wirepaths will share the same thread point. Mastercam now ignores any regular (non Thread/Cut type) points when window chaining.
22869	Chaining thread/cut points When chaining geometry, if a cut point was selected before the chain, Mastercam issued the warning message: You have not chained thread points nor entered a thread distance. In this situation, the message has been changed to: Cut point cannot be chained before contour.
22885	No core path with finish pass on a chained path that is a single arc (circle) Made motion to position for the finish pass more efficient. The “Start finish pass at closest entity” option now has the desired effect.
24042	Disabled “roll cutter around corner” setting affecting path With wire compensation type set to “control” with “optimize” active, the “roll cutter around corner” setting incorrectly affected the path even though the option was disabled (grayed out). This has been corrected.
24165	Backplot Corrected display of cutter compensation direction vector arrows.

Reference #	Description
24237	No Core wirepath The “End of Contour” flag at the end of a No Core wirepath was on the incorrect NCI data line (one move later that it should have been). This could affect the NC output from certain post processors that use this NCI flag. This has been corrected.
24452, 24460	4-axis wirepath on “open” contours Under certain conditions, a 4-axis wirepath operation on “open” contours would not regenerate. This has been corrected.
24753	Mastercam lockup upon entering the Operations Manager Corrected the lockup that occurred under certain (very rare) conditions when entering the Operations Manager dialog.
24798	Z-axis output to the NC file during No Core path Eliminated the spurious Z-axis move that would be output at the end of a No Core wirepath under certain conditions.
24864	Wire compensation “in computer” In certain rare situations, the wirepath would not start at the beginning of a chain when compensation mode was “Comp in Computer” and an “Overburn” amount was specified. This has been corrected.
24948	Reverse skims on an open contour If trimming of the lead-out was selected using the “max lead out” option on the Lead in/out dialog box, the first skim cut after tab (when in Reverse mode) would return to the original Thread Point to start the next skim cut instead of reversing from the end of the Rough/Tab cut pass. This not longer occurs.