Face Options dialog (PartMaker)

Use the Face Options dialog to orient the part and control the arc output options.

To display this dialog, click the Face Options button in theSetup dialog.

Note: The Face Options button is unavailable if you have selected a Mill Polygon, Mill Diam,Index, Mill End,Index, or Turn machining function.

The following settings are available:

Orientation Options — Use the settings in this area of the dialog to orient the part and set the Local Coordinate System to be used for machining features in a Mill 5-Axis Face window. You can enter the values manually or you can double-click a planar face on the solid model to display the Surface Info dialog and then click the Transfer Geometry button.

• Index Angle (C) — Enter the angle to which the C-axis is indexed for this Face window.
• Inclination Angle (B) — Enter the angle about the Z-axis about which the machining plane is oriented. The tool will be perpendicular to this plane.
• Plane Orientation (R) — Set the plane orientation for your Rotary 5 Axis table.
  • -90 — Use Plane Orientation (R)=-90 when programming on an A table if the Inclination Angle (B) is not 0.
  • 0 — Use Plane Orientation (R)=0 when programming on an A table if the Inclination Angle(B) is 0, or if you are programming on a B table.

  An A table is a Rotary 5 Axis table that tilts about the X axis. A B table is a Rotary 5 Axis table that tilts about the Y axis.

  The Plane Orientation option is available only if you have Mill 5 Axis Face window in PartMaker/Mill.

• Local Origin (Xo), Local Origin (Yo), Local Origin (Zo) — Enter the coordinates for the local origin created to machine the planar face. These represent coordinates relative to the workpiece's Global Coordinate System origin after the workpiece is indexed by the Index Angle (C).

Note: The Orientation options are available only if you have a Mill 5 Axis Face window.

Arc Output Options

• Break Arc Into Lines — Select this option if you want PartMaker to break all toolpath arcs into small lines in the NC program when programming for machine controls that do not support circular interpolation of arcs. You can also use this option to break helical ramp entry into lines when creating advanced milling strategies.
• Arc Tolerance — When Break Arc Into Lines is selected, you can also specify:
  • Roughing — Enter the chord tolerance that PartMaker uses to break arcs into lines during roughing operation.
  • Finishing — Enter the chord tolerance that PartMaker uses to break arcs into lines during finishing, chamfering, and corner rounding operations.

  The default Arc Tolerance values are specified on the Defaults for Milling dialog.