Use this tab to create a canned rough toolpath. This produces the
same type of cutting action as a standard roughing toolpath, but
the NC code uses your machine tool controller's canned cycles
for a more efficient program.
The parameters you see on this tab are a subset of the parameters that are available for a standard roughing toolpath. Also, these
parameters are only available if they are enabled
in the current control definition.
Stock to leave in Z
(W)
Determines how much stock remains in the Z direction when the operation is finished.
Typically, this would be removed by a separate finish operation.
Stock to leave in X
(U)
Determines how much stock remains in the X direction when the operation is finished.
Typically, this would be removed by a separate finish operation.
PERMANENTLY change to longhand
Select this checkbox to disable the canned cycle output. Instead of outputting a single canned cycle G-code with its parameters, your NC program will contain all of the individual position moves. Once you generate the toolpath with this option selected, you will not be able to change back to canned cycle output.
Clearance X
Enter a clearance value to automatically extend the start or end of the chain in
the X direction. If stock is defined, the start and end of the toolpath extend from
the end and/or the outside (or inside) diameter of the stock. If stock is not defined,
the start and end of the toolpath extend from the ends of the chain.
For example, the start will be extended in X and the end will be extended
in Z, or the start will be extended in Z and the end will be extended in X.
There are two settings on which the Clearance X value is based. First the chain
is modified based on the lead parameters in the Lead In/Out dialog box, where it
can be shortened or extended and a line could be added. Next the chain could be extended
to the stock based on the Adjust contour ends option on the Finish Parameters tab. Then the chain is extended based on the Clearance X and Clearance Z values.
Clearance Z
Enter a clearance value to automatically extend the start or end of the chain in
the Z direction. If stock is defined, the start and end of the toolpath extend from
the end and/or the outside (or inside) diameter of the stock. If stock is not defined,
the start and end of the toolpath extend from the ends of the chains.
For example, the start will be extended in X and the end will be extended
in Z, or the start will be extended in Z and the end will be extended in X.
There are two settings on which the Clearance Z value is based. First the chain
is modified based on the lead parameters in the Lead In/Out dialog box, where it
can be shortened or extended and a line could be added. Next the chain could be extended
to the stock based on the Adjust contour ends option on the Finish Parameters tab.
Then the chain is extended based on the Clearance X and Clearance Z values.
Depth of cut (U)
Sets the amount of material to be removed during each cutting pass.
Exit Length
Defines the height of the 45 degree retract move at the end of the pass.
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).
Compensation type
The options 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 Compensation type is set to Control 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 corners in the toolpath. Select None to guarantee all sharp
corners, Sharp to only roll the tool around sharp corners of 135 degrees or less,
or All to roll the tool around all corners and create smooth tool movement. The radius
of the arc moves equals the radius of the tool.
Lead In/Out
Select to 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.
Extend contour to stock
Extends the contour established by the part geometry to the stock boundary. Click
Adjust Contour Ends to control how the contour is extended.
Adjust contour ends
Opens Adjust Stock dialog box so that you can adjust the area of the stock to be
removed by extending the chained contour to the stock boundary. This option is available
only if you select Extend contour
to stock, and if the stock for the current active spindle is defined in the machine group properties
and the chained contour lies entirely within the stock boundary.
Display profile
Displays the final profile output in the toolpath. This option also allows you to
save the profile as geometry.
Linearization tolerance
This parameter is only available when chaining splines, and is 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.