Process Parameters dialog – Turning (PartMaker)

When a turning process is selected in the Process Table, the following settings are available on the Process Parameters dialog:

Note: Some settings apply only to particular types of turning process, so may not always appear on your Process Parameters dialog.

Info — This area displays information about the process you have selected:

• Process ID — This is the ID of the selected process.
• Tool ID — This is the ID of the tool used to machine the selected process.
• Face — This is the name of the Face window in which the process has been programmed.

Coolant — Select the coolant type used for the selected process (Standard, High Pressure, or None).

Multi Coolant — Click to display the Multi Coolant dialog, where you can select the coolant you want to use for the selected process. The Multi-Coolant button is displayed only if the currently loaded postprocessor has been configured to support multiple coolant pumps. Post files that have been configured to support multiple coolant pumps include vc in their file name; for example, Swiss_Demo-vc10.pst.

Tool No — Enter the number of the tool used to machine the selected process.

Offset No — Enter the tool offset used for the selected process.

Tool Change Point — Use these options to specify the tool change location (turret indexing location) for the selected process.

• X — Enter the X-axis tool change point.
• Y — Enter the Y-axis tool change point. (PartMaker/Mill only)
• Z — Enter the Z-axis tool change point.

Mode — Select a machining pattern for swiss-type lathes that require machining patterns.

Feeds and Speeds

Lock Feeds and Speeds — Select to lock the feeds and speeds values. When selected, the fields are disabled, and a padlock icon is displayed beside the locked values in the Process Table.

Feed

• Units per Minute (upm) — Enter the linear velocity in inches per minute or millimeters per minute.
• Units per Revolution (upr) — Enter the linear velocity in inches per revolution or millimeters per revolution.

Speed

• Turning Spindle Direction — Select the direction of the spindle.
  • cw — Select this option to set a clockwise rotation for the spindle.
  • c-cw — Select this option to set a counter-clockwise rotation for the spindle.
  • none — Select this option to stop the spindle rotating. The Spindle Speed is set to 0, and the field is disabled.
• Revolutions per Minute — Enter the rotational velocity when CSS is not active.
• Speed in Feet per Minute — Enter the rotational velocity when CSS is active.

  PartMaker uses Speed in Meters per Minute when using metric measurements.

• Constant Surface Speed (CSS) — Select to specify that CSS must be used for the current process.
• Max Speed — Enter the maximum rotational velocity allowed for this process when CSS is active.
• Gear No. — Enter the gear range selection for machines that require gear numbers.

Thread Whirl Tool Speed

• Revolutions per Minute (rpm) — Enter the rotational velocity for a thread whirling tool.

Output Canned Cycle for Turning — Select this option to specify that a canned cycle for turning is output to the NC program for the selected process, if the post processor is configured to do so.

Note: For a complete list of Canned Cycles for Turning that are configured in the Post Processor, refer to the Canned Cycles for Turning Support section of the Post Processor Reference Guide.

Output Hole Canned Cycle — Select this option to specify that a hole canned cycle is output to the NC program for the selected process, if the post processor is configured to do so.

Note: For a complete list of Hole Canned Cycles that are configured in the Post Processor, refer to the Hole Canned Cycles Support section of the Post Processor Reference Guide.

Output Profile — Select how the Profile is output to the NC program for a canned cycle for Turning.

• Programmed — Select this option when you enter the tool nose radius in the Machine Tool's control.
• Compensated — Select this option when you do not enter the tool nose radius in the Machine Tool's control.

Note: For more information about using the Output Profile option, see Using Output Profile for canned cycle for Turning.

Nose Radius Compensation

• None / Left / Right — Select an option to specify the relation of the tool to the contour. The initial value is set according to the settings in the group's profile parameters.
• Comp Register No. — Enter the nose radius compensation register number.
• Apply Comp in PartMaker — Select this option if you want PartMaker to compensate the toolpath output to the NC Program based on the tool nose radius. For more information on using this option, see Using Apply Comp in PartMaker for Turning.

Note — Enter any note you want to be associated with the process.

User Data — Click to display the User Data dialog, where you can specify custom data (known as User Data) for the current Post Configuration file.