Cut Pattern: Swarf
Use this page to establish the cut pattern parameters for your Multiaxis Swarf toolpath. Cut pattern settings determine the geometry your tool follows and how it travels along that geometry.
Common Toolpath Parameter Controls
Surface
Select to use surface geometry for the walls. Click Select to return to the graphics window for surface selection. The number of surfaces selected is displayed to the right of the Select button.
Chain
Select to use chained geometry to define the walls. Click Select to return to the graphics window for chain selection. The standard chaining dialog box becomes active for selecting the upper and lower rails. The number of chains selected is displayed to the right of the Select button.
Cutting method
Use the drop-down selection to choose zigzag or one way. The selection generates tool motion as described by the name.
Compensation type
Choose how you want to handle Compensation type:
- 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. The options that are available to you are determined by the active control definition.
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.
Tip compensation
Sets amount of offset to the tool's center or tip for bull-nose and ball (spherical) tools. Used for touching the tool off the part. Outputs the tool tip offset as either the tip or the corner radius distance from the tip.
Stock to leave on walls
Enter the amount of material to leave on the selected geometry. Negative values are allowed for cases where extra clearance is required.
Diameter for simulation
Only available when Compensation type is set to Control, Wear, or Reverse wear. Enter a value to be used by Backplot and Verify to represent a control compensated tool. The field is initially given the value of the tool selected for the operation, with the ability for the user to override this value.
Distance increment
Select the checkbox and enter a value. The value is a linear distance along the path taken by the tool. An additional vector will be added to the toolpath when the distance between calculated vectors is greater than the distance increment value.
Distance
Select to use a distance value to limit tool motion. The specified value is the distance between generated vectors along the selected geometry. A smaller value creates a more accurate toolpath, but may take longer to generate and may create a longer NC program.
Cut tolerance
Determines the accuracy of the toolpath. A smaller cut tolerance value creates a more accurate toolpath, but may take longer to generate the toolpath and create a longer NC program. This value is also used to eliminate duplicate positions and as a tolerance when compensating to surfaces.
Maximum step
Enter a value for the maximum space allowed between tool vectors. Additional vectors may be desirable in areas where the tool travels in a straight line for a large distance. Not available if you select the Distance option.
Enter at middle of first wall
Select to begin the toolpath at the middle position of the first wall selected. Use this option if your first wall begins at complex geometry or near a small internal corner.
Enter at start of first wall
Select to begin the toolpath at the starting position of the first wall selected. Use this option when the geometry allows safe entry, such as near an external corner.
Use wall surface rulings
Available only for 5-axis output when the following geometry selection conditions are met:
- Surfaces are selecting for walls
- Fanning is not selected
Select this option to create a toolpath using the existing surface rulings of the wall surfaces. This method is especially useful when working with impeller parts. Deselect this option to use the selected lower rail and the corresponding upper rail curves from the wall surfaces. This method creates rails that are evenly divided and proportional, based on the wall following method you choose (distance or cut tolerance).





