This page is shared
by all machine types.
For Wire machines, the only selection on this page is to enable
subprograms for wire operations.
Use this page to tell Mastercam how your control supports both
types of subprograms.
Maximum subprogram nesting levels
If the control supports nested subprograms, enter the maximum number of nested levels.
MP currently supports a maximum of 1 nested level.
Subprogram type
Indicate where in the NC program the control expects the subprograms to be located.
Allow mirror coordinate subprogram routines
This option tells
Mastercam if the control can create subprograms for mirror transformations. If this
option is not selected here, you will still be able to create the transforms, but
Mastercam will create long-hand output instead of subprograms.
Allow rotate coordinate subprogram routines
This option tells
Mastercam if the control can create subprograms for rotational transformations.
If this option is not selected here, you will still be able to create the transforms,
but Mastercam will create long-hand output instead of subprograms.
Allow nesting of mirror/rotate coordinate subprogram routines
Indicate to Mastercam if this control supports nesting toolpath transformation subroutines
that involve mirroring or rotating coordinates. Some controls which support simpler
subprograms might not support these more sophisticated operations.
Maximum mirror/rotate coordinate subprogram routines nesting levels
If the control does support nested subprograms for mirrored or rotated toolpath transformations,
enter the maximum number of levels here. MP currently supports a maximum of 1 nested
level.
Ignore work offset numbers when processing subprograms
Select this option to ignore the work offset numbers while creating subprograms for
transform toolpaths operations. If this option is selected, transform operations
will still create a single subprogram number even if the work offset numbers in copied
patterns do not match. This happens frequently with rotate transform toolpaths. Ignoring
the work offset number prevents identical subprograms from being generated.
Ignore contour flags when processing subprograms
Contour flags, also called control flags, are post variables which hold information
about a number of different toolpath states, such as the start or end of a contour,
coolant status, etc. Normally each NCI block contains a contour flag. Use this option
to retain or ignore the flags in your subprograms.
Ignore tool diameter offsets when processing subprograms
Select this option to ignore the tool diameter offsets while creating subprograms
for toolpath operations. If this option is selected, operations still create a single
subprogram number even if the tool diameter offsets in copied patterns do not match.
Ignoring the tool diameter offset number prevents identical subprograms from being
generated.
Absolute drillcycle subprograms
Use the drop-down selections to control how drill subprograms are output. Ignoring
values will output a single subprogram for identical motion. Comparing values can
output multiple subprograms, even if they have identical motion.
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.