Use the options
on this tab to create a finish toolpath for your part. Unlike
canned finish toolpaths, your part does not need to have a roughing
toolpath already created for you to create a toolpath with this
tab.
Enter your cutting parameters in the fields, and choose
an orientation for the toolpath in the Finish
direction drop-down list. You can also
enable the additional options and advanced features on the right side of the
tab.
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).
Finish stepover
Select to create one or more finish passes. 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 automatically.
Stock to leave in X
Determines how much stock remains in the X direction when the operation is finished.
Typically, this would be removed by a separate finish operation.
Stock to leave in Z
Determines how much stock remains in the Z direction when the operation is finished.
Typically, this would be removed by a separate finish operation.
Compensation type
The options that are available to you are determined by the active control definition. Tool compensation adjusts the toolpath to allow for the cutting tool's radius.
- 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 both 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 for this field 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 Compensation
type is set to Off, Mastercam uses this setting to determine the orientation of other
toolpath features such as multiple passes.
Roll cutter around corners
Inserts arc moves around the corners in the toolpath. Choose the type of arc move:
- None: Guarantees all
sharp corners.
- Sharp: Only rolls the tool around sharp corners of 135 degrees or less.
- All: Rolls the tool around all corners and creates smooth tool movement. The radius
of the arc moves equals the radius of the tool.
Corner break
Select the checkbox to automatically create radii or chamfers on all outer corners
of the toolpath. Click the button to edit the corner break settings.
Down cutting
Select to activate Down cutting. If the checkbox is already selected,
click to open the Down Cutting Parameters dialog box, in
which you can set the down cutting options for walls and flats of cut regions of
a profile.
Lead in/out
Select to have Mastercam add lead in/out moves to the toolpath. Click to edit the moves.
Plunge parameters
Click to define how the tool handles undercuts on the toolpath along each
axis.
Filter
Select to eliminate unnecessary tool moves in the toolpath to create
smoother movement. Click to configure toolpath filtering options.
Tool inspection
Select to turn on Tool Inspection. If the checkbox is already selected,
click to open the Tool Inspection dialog box, in which
you can change the tool inspection options.
Chip break
Select to turn on chip break. If the checkbox is already selected, click the button to open the Chip Break dialog box, in which you can change the chip break options.
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 stock for the current active spindle is defined in the machine
group properties and the chained contour lies entirely within the stock boundary.
Adjust contour ends
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 stock for the current active spindle is defined in the machine group properties
and the chained contour lies entirely within the stock boundary, and if Extend contour
to stock is selected.