Type and Methods: Transform Operation Parameters (Mill-Turn)
Use the Type and Methods tab in the Transform Operation Parameters dialog box to create or edit a transform operation for milling toolpaths in Mill-Turn. You also define how Mastercam creates the transformed operations.
When creating a transform option, the preferred selection order is:
- Mill type
- Axis combination
- Source operations
- Transform type
Each selection influences the options available for subsequent selections, including which source operations are available. Only options, based on the capabilities of the machine and the selected geometry, will display.
Use the large window in the left side of the dialog box to select the operations to transform. You can choose only operations in the active machine group (the machine group is activated by the position of the red arrow in the Toolpaths Manager).
Use standard Windows techniques to select operations in the list—single click, [Ctrl+Click], and [Shift+Click]. Mastercam creates the transformed operations in the active machine group.
Mill type
Select the type of machining to use for the current operation.
-
C-axis face—Enables polar interpolation for operations where the tool axis is parallel to the rotary axis.
-
Y-axis face—Enables Y-axis machining for operations where the tool axis is parallel to the rotary axis.
-
Y-axis cross—Enables Y-axis machining for operations where the tool axis is perpendicular to the rotary axis.
-
Plane rotation—Enables coordinate conversion (tilted-plane) machining cycles. This option rotates the coordinate system to simplify your NC output.
Mill-Turn toolpaths that use Axis Substitution cannot be transformed.
Reset
Removes all selections made on the Type and Methods tab. The dialog is reset to an original state.
Source operations
Select the source operations to use for the current operation. Only operations that are possible with your Mill type, Axis combination, and Transform type are displayed.
Comment
Enter comments for the toolpath. Comments help identify the operation in the Toolpaths Manager. These can be output in the NC file when you post if you select the proper option in your machine group properties.
Remove comments
Select to remove comments that exist in the selected source operations from the transformed operations. Deselect to copy comments from the source operations to the transformed operations.
Axis combination
Select the axis combination to filter out the source operations that do not use this axis combination. Only available combinations for the current machine are displayed.
Transform type
Select the type of transformation to use for the current operation. Only available types are displayed. Choose between:
-
Rotary rotate—Rotates your source operations around the Z-axis of your part.
-
Planar rotate—Translates your source operations with the plane of the source operation.
-
Planar translate—Rotates your source operations within the plane of the source operation.
Copy source operations
Creates a single transform operation, which embeds the original source operation. To cut the original part plus the transformed ones, you post only the single transform operation.
The transform operation is associative to changes in the source operations.
Disable posting in selected source operations
Since the transform operation includes the source operation, if you post both, your machine will cut the original part twice. Select Disable posting in selected source operations to ensure that this does not happen.
Subprograms
Instructs the post to create absolute or incremental subprograms for the transformed operations.





