When a milling process is selected in the Process Table, the following settings are available on the Process Parameters dialog:
Info — This area displays information about the process you have selected:
- Process ID — This is the ID of 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.
Hole Canned Cycle — Select the type of hole canned cycle you want to use.
Laser Data — For laser machining, select a material and thickness to use the feed rate and laser settings specified in the Laser Data dialog.
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.
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.
Cutting Feed — Enter the cutting feed rate for the selected process.
Plunge Feed — Enter the vertical feed rate for the selected process.
Rapid Feed — Enter the rapid feed rate for the selected process.
Tool Spindle Direction — Select the direction of the tool 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.
Spindle Speed — Enter the spindle speed for the selected process.
Axial Step (Q) — This field displays the axial step value for the selected process.
Tool Change Point — Use these options to specify the tool change location for the selected process:
- X — Enter the X-axis tool change point.
- Y — Enter the Y-axis tool change point.
- Z — Enter the Z-axis tool change point.
The following information is displayed about the groups used for the selected process:
- Group — The group name. To display the group number, as well as the group name, select Display Group Numbers on the Preferences dialog.
- Depth — The hole or profile depth.
- Z_Surf — The signed distance from the zero point to the part surface.
- Z_Rapid — The initial clearance between the tool and the part surface.
- Z-Clear (C)
— The clearance between the tool starting point and the part surface.
In PartMaker/SwissCAM and PartMaker/Turn-Mill, X_Surf, X_Rapid and X_Clear are displayed in Face windows that use X-oriented tools.
Modify Feed rate on Arcs — Click to display the Modify Feedrate on Arcs dialog. Use this dialog to set feed rate modification parameters for the selected process. This button is displayed only for a Contour Mill process with a tool position LEFT or RIGHT.
Output Hole Canned Cycle — Select to specify that a hole canned cycle has to be used for the selected process.
Cutter Diam Compensation — Use these options to specify cutter diameter compensation. These options are displayed only if relevant to the current process.
- None / Left / Right — Select an option to specify the relation of the cutter to the contour. The initial value is set according to the settings in the group's profile parameters.
- Comp Register No — Enter the cutter compensation register number.
- Apply Comp in
PartMaker — Select to specify that
PartMaker applies cutter diameter (or radius on some machines) compensation. When selected, only the wear value (that is, the difference in diameter (or radius) between the cutter used for machining and the one programmed in
PartMaker) must be entered as the compensation amount.
If this option is not selected, PartMaker outputs the actual contour coordinates and the compensation amount must be the full diameter (or radius) of the cutter being used for machining.
The first and last tool position on the Leads In and Leads Out are compensated by the tool diameter, as cutter compensation is not activated at these points in the output G-code.
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.