Use this tab to
create a lathe contour rough toolpath. This roughing toolpath
is designed to take passes parallel to chained geometry. This
toolpath is useful for parts where the initial stock shape is
similar to the final part shape, such as using a casting for stock.
First, select whether the cutting method is one-way or zig-zag, and select a toolpath orientation from
the Rough direction list. Then, use
the graphics as a guide for entering the toolpath dimensions.
Use the options on the right side of the tab to select the type
of cutter compensation and complete the toolpath by adding advanced
features such as a semi-finish pass, lead in/out moves, and toolpath
filtering.
Entry amount
Determines the distance from the stock that the tool starts to feed.
Exit amount
Specifies the amount that the tool moves beyond the stock boundary at
the end of a cut.
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
The tool cuts the part in a back and forth motion. The picture in the dialog box
changes to show this tool motion.
Rough direction
Choose from which direction the tool will cut the toolpath: ID–inner diameter,
OD–outer diameter, Face–front face, or Back–back face.
Constant offset
Select to set how far the toolpath is offset from the stock. Enter
a constant offset value in the Offset field. Constant offset and XZ offset are mutually exclusive options.
XZ offset
Select to set how far the toolpath is offset from the stock. Enter separate
values for the X axis and Z axis. Constant offset and XZ offset are mutually exclusive options.
Stock to leave in X
Enter 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
Enter how much stock remains in the Z direction when the operation is finished.
Typically, this would be removed by a separate finish operation.
Minimum cut
Enter the smallest cut that can be taken per pass. Used to prevent very short
cuts.
Minimum air
Enter the distance needed to trim the pass and insert a rapid move. Used to
prevent very short rapid moves along a pass.
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 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.
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 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 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.
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 and choose how you want the tool to cut undercuts along 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.
Chip break
Select to turn on chip break. Click
to open the Chip Break dialog box, in which you can change
the chip break options.
Stock Recognition
Lets you choose how to adjust 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: Disables Stock Recognition.
Adjust stock
Opens Adjust Stock and lets you adjust the area of the stock to be
removed by the roughing operation. This option becomes available only if:
- stock boundaries are defined in the machine group properties
- the chained contour lies entirely within the stock boundary
- either the Use stock for outer boundary or Extend contour to stock only options are
selected.
Linearization tolerance (only available when chaining splines)
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.