Cutoff Parameters
Use the Cutoff Parameters dialog box to create a cutoff toolpath. You do not need to create or chain any geometry for this toolpath. Mastercam will create the toolpath based on the parameters you enter in this tab and the boundary point you selected.
Use the diagrams on the tab as a guide to entering the cutting parameters and toolpath dimensions. You can create a radius or chamfer on the corner. Activate advanced toolpath features by selecting checkboxes on the right side of the tab. These let you create lead in/out moves, plunge in pecks, add canned text at specific radius values, or use toolpath filtering.
Entry amount
Determines the distance from the stock that the tool starts to feed.
From stock
Determines how the Entry amount in the Cutoff parameters tab, the Incremental Retract Radius in the Cutoff parameters tab, and the Entry amount in the Clearance Cut dialog box is computed. Select this option to calculate the value from the maximum stock diameter of the Z coordinate. Deselect to use a selected point for the toolpath. If the selected point is outside the Z bounds of the stock, Mastercam uses the maximum radius at either the minimum or maximum stock Z coordinate, depending on which is closer to the point.
The From stock checkbox for Entry amount is disabled if stock in the active spindle is not defined.
Retract radius
Choose a retract radius option:
- None: The tool will not retract before returning to the home position.
- Absolute: Uses the exact value you enter to determine how far above the Z axis the tool will retract before moving to the home position.
- Incremental: Determines how far above the Z axis the tool will retract before moving to the home position. Mastercam calculates this value relative to the current top of stock.
X Tangent point
Click to select a point on the geometry, or enter a value to set the point on the part's radius to cut to. For example, when cutting a tube set this value to the radius of the ID of the tube. In Lathe mode, X Tangent Point is interpreted as an absolute value.
Back face stock
Use this option if you want to leave stock on the back face for finishing operations. Enter a value or click to populate the field with the stock amount set in the Left margin or Right margin field in the Geometry tab of the Machine Component Manager. This field uses the Left margin value if the stock is in the left spindle, and the Right margin value if the stock is in the right spindle. You must select the Use margins checkbox to populate the Back face stock field.
If you click Back face stock and have defined your stock as anything other than a cylinder, a warning message appears, and the field value does not change. You can manually enter a value.
Front radius
Directs the tool to enter the part only as deep as the center of its front radius.
Back radius
Directs the tool to enter the part only as deep as the center of its back radius.
Corner geometry
Choose how Mastercam should handle corners:
- None: Select to create a square corner on the part.
- Radius: Select to create a radius on the corner of the part. Enter a radius value.
- Chamfer: Select to create a chamfer on the corner of the part.
- Parameters: Click to enter the dimensions and other chamfer options.
Clearance cut
Select to create a clearance cut for the chamfer. Click to define the chamfer parameters.
Radius to apply new settings
Used to adjust the feed rate and spindle speed part way through a cut. Enter the radius in the cut at which you want the secondary feeds and speeds to be applied.
Feed rate
Enter the speed at which the tool cuts along the toolpath and choose a unit:
- in/rev or mm/rev: Calculates the value in inches per revolution or millimeters per revolution.
- in/min or mm/min: Calculates the value in inches per minute or millimeters per minute.
Spindle speed
Enter the rotation speed of the spindle and choose a unit:
- RPM: Calculates the value in revolutions per minute.
- CSS: Calculates the value in constant surface speed.
Compensation type
Tool compensation adjusts the toolpath to allow for the cutting tool's radius. The options that are available to you are determined by the active control definition.
- 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.
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.
Canned text
Select to add canned text commands at specific points or radius values. Click to select the locations and canned text commands to be added.
Peck
Select to have the tool approach the part in several pecks instead of a single move. Click to set the peck dimensions.
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.





