Use the Post Options dialog to specify how PartMaker generates NC programs for the current part.
PartMaker displays the Post Options dialog when you generate an NC Program for the first time when programming a part. You can also display the dialog by selecting Job Optimizer > Post Options.
The following settings are available:
Main Program No — Enter the main program number for the NC Program file. PartMaker automatically generates a number when you use the Job Optimizer > Generate NC Program menu option. This number is used for Fanuc and similar controls.
Block Start — Enter the starting line number in the NC Program file.
Block Increment — Enter the incremental line number to use in the NC Program file. If the value is 0 (zero), the part program will not contain sequence numbers.
Stop to Include User Input— Select this option if you want ConfigPost to prompt users to enter any specific job-related information that is required to complete the post processing and produce an NC Program file. This is useful for situations when the postprocessor needs more information than PartMaker can supply to it.
When prompting for user input, PartMaker displays the current process number, corresponding tool name and a prompt to enter the additional process information required by ConfigPost. Autodesk recommends that you leave this option selected. For a complete list of prompts that may appear during post processing, refer to the "Prompts" section in the Post Processor Reference Guide.
Auto-Reload Post Config File — Select this option so PartMaker automatically reloads the currently loaded Post Config file(s) whenever the NC program is generated. Use this option if modifications to the post processor are made using ConfigPost.
Separate Faces —Select this option if you want PartMaker to write the NC program output for different faces to different NC Program files. See Multiple Faces Programming for more details.
Subprograms
- Subprogram Option Enabled — Select to use subprograms when the NC Program file is generated for the current part.
- Min. No Holes for Subprogram — Enter the minimum number of holes in a group that are required to generate a subprogram.
- Subprogram Start — Enter the start number for any subprograms required.
- Subprogram Increment — Enter the increment for numbering subprograms.
4th Axis Output — Use the following options if you are using a Rotary 4 Axis Table in PartMaker/Mill.
- X Axis Rotary — Select if the stock rotates around the X axis. This sets the corresponding reserved word in ConfigPost <is-x-axis-rotary> to True.
- Y Axis Rotary — Select if the stock rotates around the Y axis. This sets the corresponding reserved word in ConfigPost <is-x-axis-rotary> to False.
Output Coordinate System — The options available in this area vary depending on whether you have selected a Rotary 5 Axis table, a Vertical Rotary table. or a Tombstone table.
- Local Coordinates — Select this option so the NC coordinates are relative to the Face Coordinate system. Use this option when the machine is capable of a work shift or a coordinate system transformation.
- Global Coordinates — Select this option so the NC coordinates are relative to the Global Coordinate system. You can specify the origin of the Global Coordinate system using the Global Origin drop-down list on the Rotary 5 Axis or Vertical Rotary Table Settings dialogs.
For Tombstone tables, the global origin is at the bottom center of the base plate.
Output Control — Click to display the Output Control dialog, where you can set options to control the content and format of the NC Program output from PartMaker.