Use the Defaults for Turning dialog to specify default machining parameters, such as group and process parameters, for turning.
To display this dialog, select Job Optimizer > Defaults.
Hole Group Parameters
Use this options to set the default values for new hole groups created in a Turning Face window. PartMaker uses these default values on the Hole Group Parameters dialog
Through Hole — When selected, specifies a through hole; when deselected, specifies a blind hole.
Diameter — The default hole diameter.
Chamfer — The default chamfer size.
Clearance — The default clearance for roughing operations.
Nominal Depth — The default nominal hole depth.
Profile Group Parameters
Use these options to set the default values for new profile groups created in a Turning Face window. PartMaker uses these default values on the Profile Group Parameters dialog.
X Finish — The default thickness of the finishing pass in X.
Z Finish — The default thickness of the finishing pass in Z.
Return Length — The default return length.
Return Angle — The default return angle.
Surface Roughness — The default surface roughness factor.
Chamfer Length — The default chamfer length.
# of Spring Passes — The number of spring passes.
Start at Cutting Point — When selected, the tool starts at the defined cutting point before following the toolpath.
Return to Cutting Point — When selected, the tool returns to the defined cutting point after completing the entire toolpath.
Thread Height — Specify how you want the Thread Height value for threading or thread whirl cycles to be defined:
Select %Pitch to define the height as a percentage of the pitch, so the resulting height is Pitch * Thread Height / 100.
Select Part Units to define the height as the actual measured height of the thread in the current part units.
Process Parameters
Apply Comp in PartMaker — Select this option if you want PartMaker to compensate for the tool nose radius.
Output Canned Cycle for Turning — Select this option if you want Canned Cycles for Turning to be used by default.
Coolant — The default coolant type for machining (High Pressure, Standard or None).
Feed Units — The units used to display feeds. You can select upr (Units per Revolution) or upm (Units per Minute).
Constant Surface Speed — Select this option if you want Constant Surface Speed (CSS) to be used by default.
Default Feed — The default feed rate for all tools.
Default Speed — The default RPM (spindle speed) for all tools.
Primary Tool Post — Select the Tool Post (for example, Gang Slide or Turret) that has to be the Primary Tool Post in M2S* mode in PartMaker/SwissCAM.
Retract From Groove Options
When PartMaker creates a grooving toolpath, some retract moves are Rapid and some are Linear depending on how far these moves are from the walls of the groove profile.
To set default options for controlling retract moves in grooving toolpaths, click Groove Options Defaults to display the Groove Options Defaults dialog.
Machining Data
Min Feed — The default minimum feed rate.
Max Feed — The default maximum feed rate.
Rapid Feed — The default rapid feed rate.
Max Speed — The default maximum speed that can be reached.
Tool Change Time — The default tool index time.
Leads
Arc Radius — The default arc radius.
Line Length — The default line length.
Lead Angle — The default lead angle.
Input Options
Diameter Programming — Select this option if you want to perform diameter programming in CAD.
Positive Z Programming — Select this option to enter the Z value as a positive value.
Toolpath Options
Corner Rounding — Select this option if you want PartMaker to insert circular arcs when going around sharp corners when it performs tool nose radius compensation.
Remaining Stock Detection — Select this option if you want PartMaker to detect which sections of a toolpath must be avoided due to tool angle. This prevents the tool from gouging. Autodesk recommends that this option is selected.