NC Output page: Control Definition Manager
Use the NC Output page to set a variety of options which affect how the NC code is formatted and presented. All machine types use this page.
Use this option to tell the post which type of coordinate output to generate, either incremental or absolute. Typically, this results in either a G90 or G91 code being output near the beginning of your program, but the exact effect is determined by your post processor.
All comments are typically written to the NCI file; use these options to tell Mastercam which comments you want automatically written to the NC file. The selections you make here are defaults which you can override. You can configure NC comments in the Files tab of the Machine Group Properties dialog box.
These options gather together information that was set in several locations in previous Mastercam versions. All of the information in this section is written directly to the control definition. The Start sequence number and the Increment sequence number can be changed on the Tool Settings tab of the Machine Group Properties dialog box.
Mastercam supports both integer and real values for sequence numbers; choose Use decimal sequence numbers to activate this feature. When decimals are enabled, input fields for sequence numbers can be entered as a real number. These are limited by the Number of places values which you enter here.
These values are read directly by the post and cannot be overridden on the fly.
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.
Main program default absolute/incremental
Select whether the default mode for coordinate positions will be incremental or absolute. Typically, this results in either a G90 inserted in the NC header block for absolute mode, or G91 for incremental.
Output operation comments to NC
Choose whether to include operation-specific comments in the NC program. These are created in the Toolpath parameters tab for each operation. This setting is a default which can be overridden in the machine group properties.
Output machine name to NC
Choose whether to include the machine name as a comment in the NC program. The name comes from the machine definition. This setting is a default which can be overridden in the machine group properties.
Output group name to NC
Choose whether to include the name of the machine group in the NC program, as displayed in the Toolpaths Manager.
Output group comments to NC
Choose whether to include machine group-specific comments in the NC program. These are created in the Files tab of the Machine Group Properties or the Machine page of the Machine Group Setup function panel.
Maximum characters in NC comment
Enter the maximum number of characters allowed by your control for NC comments.
Output sequence numbers
Choose whether to include sequence numbers in the NC program. These are created in the Toolpath parameters tab for each operation. This sets the post variable omitseq$.
Start sequence number
If you choose to include sequence numbers in the NC program, enter the first number here. This setting is a default which can be overridden in the machine group properties. This sets the post variable seqno$.
Increment sequence number
If you choose to include sequence numbers in the NC program, Mastercam will increment each line by this amount. This setting is a default which can be overridden in the machine group properties. This sets post variable seqinc$.
Maximum sequence number
If you choose to include sequence numbers in the NC program, enter the highest sequence number allowed by your control. This sets the post variable seqmax$.
Reset sequence numbers in subprograms
Select this option to control whether or not the sequence numbers continue through subprograms. This sets the post variable sub_seq_typ$.
Use decimal sequence numbers
Select this option if your control is capable of using decimal sequence numbers.
Number of places to right/left of decimal
If your control is capable of using decimal sequence numbers, use these fields to format the sequence number output by telling Mastercam how many decimal places to use on either side of the decimal point.
Spaces between NC addresses
Enter a value in this field to have Mastercam automatically insert spaces between codes in your NC program lines. It will insert the number of spaces you enter here. This sets the post variable spaces$.
Remove CR/LF at the end of the NC block
Select this option to tell Mastercam not to insert a carriage return / line feed combination (ASCII characters 10/13) at the end of every block. Use the alternate EOB fields to specify a different block delimiter, if desired. This sets the post variable omitcrlf$.
First/second alternate EOB character (Ascii value equivalent)
Use these fields to tell Mastercam the characters to insert at the end of each NC block. Enter the ASCII value of the desired character. For example, enter 36 to insert a $ at the end of each block. The first alternate character sets the value of the eob$ post variable. The second alternate character sets the value of prv_eob$.





