Rough Parameters: PrimeTurning™
Use this tab to create a rough PrimeTurning toolpath. Enter your cutting parameters in the fields, using the picture as a guide for the toolpath dimensions. You can also select cutter compensation and enable advanced features such as lead in/out moves, toolpath filtering, and chip break on the right side of the tab.
Rough
Activates the roughing page of options.
Strategy
Choose a strategy for the desired cutting motion, as follows:
- Horizontal: All roughing passes will be horizontal, parallel to the rotary axis.
- Vertical: All roughing passes will be vertical, perpendicular to the rotary axis. The passes may cut toward or away from the rotary axis depending the Up cut diameter option.
- Horizontal then vertical: Roughing passes will start out horizontal. Once the passes cut to a critical depth, the roughing passes will switch to vertical. A critical depth is the depth where the geometry is flat, like the top of a step or a wall. Potentially, there can be multiple steps in the geometry that will result in multiple switches between horizontal and vertical passes.
- Vertical then horizontal: This is the same as Horizontal then vertical except the initial passes will be vertical and then switch to horizontal.
- Alternate horizontal then vertical: The first roughing pass will be horizontal, the next will be vertical, and so on.
- Alternate vertical then horizontal: The first roughing pass will be vertical, the next will be horizontal, and so on.
Up cut diameter
Use this option to divide vertical passes into an up cut, away from the rotary axis, and then a down cut, toward the rotary axis. When the option is deselected, all vertical passes will be down cuts, toward the rotary axis. You can also set Up cut diameter to zero, and all passes will then be up cuts, away from the rotary axis.
Select
Returns you to the graphics window where you can select a point to define the Up cut diameter.
Minimum up cut
Used when a vertical pass is divided into an up cut and down cut. If the up part of the divided pass is less than the Minimum up cut, the entire pass will be a down cut. If the down part of the divided pass is less than the Minimum up cut, the entire pass will be an up cut. This prevents very small up or down cuts.
Clean up corners
After all of the roughing passes complete, this option adds extra passes to cleanup material leftover in the corners. The material leftover in the corner is the result of the arc lead-in move at the start of the rough passes.
Approach arc radius
Use this option to control the arc radius used to enter new cuts.
- Maximum entry angle: Controls the approach arc generation when the tool is plunging into material at the beginning of a roughing pass. The angle is relative to the plunge direction of the toolpath. If any portion of the chained geometry is at or less than the angle entered, the approach arcs will be applied. If any portion of the chained geometry is greater than the entered angle, it will not have approach arcs applied. The maximum allowable angle is 90 degrees.
- Same as depth cut: Uses the depth cut as the approach arc radius.
- Manual: Specify a value to be used as the approach arc radius.
Feed rate
Opens the Feed Rate dialog where you can set feed rates for roughing passes.
Spindle speed
Determines the rotation speed of the spindle in revolutions per minute (RPM) or constant surface speed (CSS). Mastercam calculates a default value according to the machine group properties, but you can override this by typing in a new value. If you are in RPM mode, Mastercam warns you if either the default or the value you type in is outside the range set in the machine definition.
Cut direction
Choose from which direction the tool cuts the toolpath: ID, OD, face, or back.
Overlap amount
Select and enter 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.
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.
Depth of cut
Sets the amount of material to be removed during each cutting pass. If Equal steps is selected, this value determines the maximum amount of material the tool can remove per pass.
Minimum cut length
Determines the smallest cut that can be taken per pass.
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 the cut.
Stock to leave in X
Determines how much stock remains in the X direction when the operation is completed. 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 completed. Typically, this would be removed by a separate finish operation.
Compensation type
The options that are available here are determined by the active control definition. Choose one of the following:
- 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
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 General page in the Control Definition dialog box.
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.
Lead in/out
Select to have Mastercam add lead in/out moves to the toolpath. Select the button to open the Lead In/Out dialog box.
Plunge parameters
Opens the Plunge Cut Parameters dialog box, which defines 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. Select the button to open the Filter dialog box.
Tool inspection
Select to turn on tool inspection. Select the button to open the Tool Inspection dialog box.
Chip break
Select to identify when chip breaks can occur. Select the button to open the Chip Break dialog box.
Stock recognition
Stock recognition is locked to Remaining stock in the PrimeTurning toolpath. The Remaining stock setting uses only stock remaining from previous operations.
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.





