Post Options dialog - PartMaker/Turn-Mill

Use the Post Options dialog to specify how PartMaker generates NC programs for the current part.

PartMaker displays the Post Options dialog the first time you generate an NC Program when programming a part. You can also display the dialog by selecting Job Optimizer > Post Options.

Note: Refer to the machine-specific Post Processor Reference Guide for the machine you are using before completing this dialog. Some of the terms described below may not be used depending on the postprocessor loaded into PartMaker.

The following settings are available:

Program No.

• Program #1 — Enter a four-digit number, which is required at the beginning of the NC program. For twin turret machines, this number corresponds to the NC program created for Channel #1 machining operations.
• Program #2 — Enter a four-digit number that corresponds to the NC program created for Channel #2 machining operations. Applicable for twin turret machines.
• Bar Load — Enter the name of the bar loading macro, if required. Refer to the Post Processor Reference Guide to find out if this is available for your machine.

Wait/Queue Commands

• Start — Enter the start number of the first wait code in the NC program on multi-channel machines. Refer to the Post Processor Reference Guide for more details.
• Increment — Enter the amount by which the wait code increments on multi-channel machines. Typically, you would enter an integer less than, or equal to, ten.

Job Settings

• Phase Angle — Enter a phase angle (in degrees), if required. This value represents the angle between the main spindle C-axis zero degree position and the sub-spindle C-axis zero degree position. It is used for jobs that require the main spindle and the sub-spindle to align at specific angles during part support or pickup of non-round stock.
• Sub Spindle Feed onto Part (UPM) — Enter the feed rate for the sub-spindle to use prior to part gripping.

Part Release Data

• Station No. — Enter the station number the turret will index to drop the part from the gripper/basket into the parts chute. The value should be a one or two-digit integer.
• Release-X — Enter the coordinate along the X-axis where the basket/sub-spindle can release/eject the part.
• Release-Z — Enter the coordinate along the Z-axis where the basket/sub-spindle can release/eject the part.

Machine Options

• Air Blast — Select this option to use air blast features on the machine, if supported. Refer to the Post Processor Reference Guide for more details.
• Cut-off Detection — Select this option to use cut-off detection features on the machine, if supported. Refer to the Post Processor Reference Guide for more details.

Axis Support

• Main Spindle C-axis — Select this option if the machine’s main spindle is equipped with a continuous C-axis.
• Sub-Spindle C-axis — Select this option if the machine’s sub-spindle is equipped with a continuous C-axis.

Customer PIN — Enter the seven-digit customer PIN supplied with PartMaker.

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.

B-Axis Output

• Local Coordinates — Select this option if the machine allows a translated part origin and a rotated coordinate system orientation within a part program.
• Global Coordinates — Select this option if the machine does not allow a translated part origin and a rotated coordinate system orientation within a part program. All PartMaker's coordinates entered for a 5-axis machining plane will be converted to the global coordinate system. When using this option, make sure you also select the Break Arcs Into Lines option in the Face Options dialog.
• 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.