Use this tab to
create a facing toolpath without chaining geometry. Mastercam creates the toolpath
from the parameters you enter here.
First you must
specify how much stock to remove, using either of the following
methods:
Then, enter values for the cutting parameters.
Select points
Click to choose the boundary points from the graphics window. You will
select two corners of a rectangle.
Use stock
Computes the start and end points for each cut based on the stock boundary and the
Z coordinate of the finished face of the part. If the stock changes, regenerate the
facing operation to update the start and end positions of each facing pass.
Finish Z
Enter the Z coordinate of the face of the part or click to choose the point from the graphics window. Only active if you select the Use
stock option.
Entry amount
Determines the distance from the stock that the tool starts to feed.
Rough stepover
Select to create multiple roughing cuts. Enter a stepover distance to define how much stock gets removed during each rough
cut.
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.
Overcut amount
A rectangle is used to define the material removed by the facing toolpath. The overcut
amount determines how far past the rectangle the tool will cut. Typically this is
a small distance that the tool cuts past the part centerline.
Retract amount
Determines the distance the tool moves away from the face of the part before it moves
to the start of the next cut.
Rapid retract
Determines how the tool moves back to the feed plane. If you select Rapid Retract,
the tool uses the machine's rapid rate. If you deselect Rapid Retract, the tool uses
the retract rate set in the Tool Parameters tab.
Stock to leave
Determines how much stock remains on the part when the operation is complete. Typically,
this would be removed by a separate finish operation.
Cut away from center line
A rectangle is used to define the material removed by the facing toolpath. Cut away
from center line sets the tool to start each cut on the side of the
rectangle closest to the center line and cut away from the center line.
Cross centerline cut
Create the toolpath on the opposite side of the centerline from the selected tool. Mastercam automatically switches the directions of the spindle rotation, compensation, and entry/exit moves.
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 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.
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.
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.
Maximum number of finish passes
Determines the number of finish passes the tool will make. Finish passes are made
after the rough passes using the finish stepover amount.
Corner
Select to activate and click to access the Face Corner dialog box where
you can set options for adding a chamfer or radius to the edge of a part. The break
or chamfer is only allowed on the “leading” corner of the face, which is the first corner
encountered moving in the direction of the toolpath.
Lead in/out
Select to have Mastercam add lead in/out moves to the toolpath. Click
to edit the moves.
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 the button to open the Tool Inspection dialog box and change the tool inspection options. Not available for Mill-Turn Face operations.
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.
Second feed/speed
Select to change the feed rate and spindle speed at a given diameter of the face cut. If the checkbox is already selected, click the button to open the Second Feed Rate/Spindle Speed dialog box, in which you can change the feed rate and spindle speed options. These settings are not available if Cut away from center line is selected.