Cutter Compensation: Control Definition Manager
Use this page to
tell Mastercam how your control implements cutter compensation
and which compensation options will be available to the user.
The first checkbox determines if the control supports cutter
compensation at all. If this option is not selected, you will
not be able to select Control as the
compensation type, but you will be able to select Computer to
have Mastercam calculate compensated toolpaths. If this option
is selected, the other options are enabled.
Select Optimize Toolpath to enable
this option as the default for new toolpaths. It causes Mastercam
to eliminate arcs from the toolpath if, in the compensated toolpath,
they would be smaller than the radius of the selected tool.
Parameters
Control supports cutter compensation in control
Selecting this option lets users select Control as the compensation type when creating
toolpaths. If this option is not selected, the other options on this page are not
available.
Number of look ahead NC blocks for cutter compensation on machine control
Consult your control documentation to determine this value. This value is only used
by the post processor, it is not used within Mastercam.
Allow cutter compensation in control to be activated/deactivated on arcs
Select this option if it is supported by your control. This setting is not used anywhere
in Mastercam, but it is available to your post and needs to be implemented there.
Control supports wear compensation (negative offset value)
Selecting this option lets users select Wear as the compensation type when creating
toolpaths.
Control supports reverse wear compensation
Selecting this option lets users select Reverse as the compensation type when creating
toolpaths.
Start and end cutter compensation above part (read by post only)
Select this option if cutter compensation is to be turned on before the lead in move
and turned off after the lead out move. Selecting this option does not change the
toolpath or NCI file, but it is available to the post and needs to be implemented
there. This setting does not apply to Wire.
Optimize Toolpath
Enables this feature as the default for new toolpaths. Mastercam uses this feature
to remove arcs from toolpaths that would be smaller than the tool radius when the
toolpath is compensated.
Stock to leave application
The Program coordinates and Machine offset register options determine how the Stock
to Leave value is applied to a wirepath. These options can be edited in the Apply
additional offset to section of the Wire/Power page of any wirepath dialog box. The
Stock to Leave values are also set in the Wire/Power page.
Right-click
menu options
Default
Reset either the current
page or the entire control definition to the default values.
Import
Import values for either
the current page or all pages from a different control definition. However, importing
values will not change the following:
- selected post processor, control
type, and name
- toolpath/operation defaults
- post text
- miscellaneous integer
and real values
You can import
post text and miscellaneous values from the Text page.