Quick Finish Parameters
Use this tab to
create a quick finish toolpath. First, select the geometry for
the operation. Choose Chain to return to the graphic window and select the geometry, or
choose an operation from the list to finish it. Then, use the
pictures as a guide for entering the cutting parameters. This
toolpath also lets you create simple entry and exit moves. Use
Mastercam's standard finish operation to have access to complete
lead in/out capabilities.
Parameters
Chain
Select to base the toolpath on chained geometry. Click Chain to return to the graphics window and select the geometry.
Operation
Select to finish a roughing toolpath that has already been created. Select
the operation from the list. Only rough and quick rough operations will be available
for selecting.
Finish stepover
Enter a stepover distance
to define how much stock gets removed during each finish cut.
Number of finish passes
Enter the number of finish passes. If you choose to make more than one finish pass,
then Mastercam determines the offset direction.
Finish direction
Choose from which direction the tool will cut the toolpath: ID (inner diameter),
OD (outer diameter), Face (front face), or Back (back face).
Compensation type
The options that are available to you are determined by the active control definition.
Choose how you want to handle cutter compensation:
- Computer: Mastercam computes the compensated toolpath and does not output control
codes for compensation.;
- Control: Mastercam outputs control codes for compensation and does not compute the
compensated toolpath.;
- Wear: Mastercam both computes the compensated toolpath and outputs control codes
for compensation. Compensation direction in the computer and control are the same.;
- Reverse wear: Mastercam computes the compensated toolpath and outputs control
codes for compensation. Compensation direction in the computer and control are opposite.
- Off: Mastercam programs the tool tip directly on the chained geometry and does not
output compensation codes.
Optimize cutter compensation in control
Eliminates arcs in the toolpath that are less than or equal to the radius of the
tool and helps prevent gouging. The default setting is set on the
Cutter Compensation, General page in the Control Definition.
This field is available only when Cutter compensation is set to Control on the parameters tab, and applies only to that setting.
Compensation direction
Choose to offset the tool to the right or left of the toolpath. Even if cutter compensation
is set to Off, Mastercam uses this setting to determine the orientation of other
toolpath features such as multiple passes.
Lead in/out
Select to have Mastercam add lead in/out moves to the toolpath. Click
to edit the moves.
Extend contour to stock
Extends the contour established by the part geometry to the stock boundary. Click
Adjust contour ends to control how the contour is extended. This option
is available only if you have defined stock for the current active spindle in Machine Group Properties and the chained contour lies entirely within the stock boundary.
Adjust contour ends
Opens Adjust Stock dialog box and lets you adjust the area of the stock to be
removed by extending the chained contour to the stock boundary. This option is available
only if you have defined stock for the current active spindle in the Machine Group Properties
and the chained contour lies entirely within the stock boundary, and if Extend contour
to stock is selected.
Linearization tolerance
Used when converting 3D arcs and 2D or 3D splines in the chained geometry from curves
to lines. Smaller linearization tolerance values make more accurate toolpaths, but
may take longer to generate and create a longer NC program. This option is only available when chaining splines.