Rough Parameters
Use this tab to create a Lathe Rough toolpath. Compared to other types of Lathe roughing toolpaths, this tab offers you the most complete set of roughing options.
Enter your cutting parameters in the fields, and choose a cutting direction and select an orientation for the toolpath in the Rough direction/angle drop-down list. Use the pictures as a guide for entering the toolpath dimensions. You can also select cutter compensation and enable advanced features such as a semi-finish pass, lead in/out moves, and toolpath filtering on the right side of the tab.
Entry amount
Enter the distance from the stock that the tool starts to feed.
Exit amount
Specify the amount that the tool moves beyond the stock boundary at the end of a cut.
Cutting Method
Choose a cutting method/direction from the drop-down menu.
- One way: The tool cuts the part in one direction, comes up, goes back to the beginning, and cuts again. The picture in the dialog box changes to show this tool motion.
- Zig zag straight: The tool cuts the part in a straight back and forth motion. The picture in the dialog box changes to show this tool motion.
- Zig zag downward: The tool cuts the part in a downward back and forth motion. The picture in the dialog box changes to show this tool motion.
Rough direction/angle
Determines the angle that the tool cuts into the part. This angle is relative to the rough direction, OD, ID, Face, or Back.
Overlap
Select to create an overlap between each rough cut. Click to set how much the tool overlaps the previous cut before making the next cut. If deselected, the tool will not retract before cutting down to the next level. For canned rough toolpaths, you only enter the value.
Auto
Removes material equal to the Depth of cut during each pass, until the depth of cut value becomes too large and will begin to make smaller passes. Those passes will not be less than the Minimum cut depth.
Equal steps
Removes the same amount of material per pass without exceeding the Depth of cut value.
Incremental
Removes an incremental amount of material with each pass, starting at the Initial cut depth and increasing or decreasing until it reaches the Final cut depth.
Initial cut depth
Sets the initial cut depth of the incremental type of Depth cuts.
Depth of cut
Sets the amount of material to be removed during each cutting pass. This option is only available when Depth cuts is set to Equal steps or Auto. If Equal steps is selected, then this value determines the maximum amount of material the tool can remove per pass.
Increments of
When selected, Mastercam will cut the first pass at the Initial cut depth and then cut the following passes at the Initial cut depth plus the Increments of amount until the Final cut depth has been reached.
Only available when Depth cuts is set to Incremental.
Final cut depth
Sets the final cut depth of the incremental type of Depth cuts.
Minimum cut depth
Determines the smallest cut that can be taken per pass. Only available when Depth cuts is set to Auto or Equal steps.
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.
Variable depth
Allows you to vary the point that the surface contacts the tool insert to prevent notching and improve tool life. The variable depth can vary up to 25% of the depth of cut. The actual depth of cut can vary from 75% to 125% of the depth of cut. The valid range is -25% to 25%. A positive value will result in an upward cut and a negative value will result in a downward cut. Zero will result in a straight cut.
- The passes will alternate between angled and straight.
- If the cut length is less than three times the cut depth, a straight cut will be made instead of an angled cut.
- In flat areas, a straight cut will be made instead of an angled cut.
- One-way and zig-zag cuts are both supported, as well as ID, OD, Face, Back, and Angled.
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 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 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.
This option is available only when Compensation in computer is turned on.
Semi finish
Select to create a semi-finish pass after the final roughing pass. This pass follows the contour of the part with the roughing tool, preparing it for the actual finish operation. Click to configure the semi-finish pass.
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 the button to open the Tool Inspection dialog box and 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.
Section turning
Select to turn on Section turning. If the checkbox is already selected, click the button to open the Section Turning dialog box, in which you can set the toolpath to break into sections.
Stock recognition
Adjusts the area of the stock to be removed by the roughing operation. The following options are available:
- Remaining stock: uses only stock remaining from previous operations.
- Use stock for outer boundary: uses a section of the stock boundary as the outer boundary.
- Extend contour to stock only: linearly extends the ends of the chained contour to the stock.
- Disable stock recognition: provides no stock recognition.
Adjust stock
Opens the Adjust Stock dialog box and lets you adjust the area of the stock to be removed by the roughing operation. This option is available only if:
- You define stock boundaries in the machine group properties.
- The chained contour lies entirely within the stock boundary.
- You select either the Use Stock for Outer Boundary or Extend Contour to Stock Only options.
Shorten pass
Use to adjust the start of each pass based on the shape of the remaining stock from the previous pass and the shape of the tool.
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 parameter is only available when chaining splines.





