Type and Methods: Transform Operation Parameters
Use the Type and Methods tab in the Transform Operation Parameters dialog box to create or edit a Transform operation. Here you select the source operations and the type of transform. You also define how Mastercam creates the transformed operations.
After you select the type of transformation, choose the remaining dialog box tab to complete the operation. For example, if you choose a rotate transformation type, only the Rotate tab is available, the Translate and Mirror tabs do not display.
Click on a drop-down below to learn more about using this tab.
Use the large window in the center of the dialog box to select the operations to transform.
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.
The Type and Method sections tell Mastercam how to transform the selected operations.
Select a transformation type:
- Translate runs the operations at a new location; for example, cutting multiple copies of the same part at different fixtures on the table. Select this option to also run the same operation in a different plane; for example, cutting a contour on each side of a block.
- Rotate runs the operations at an angle to the original operation. You can choose to rotate the operation in the same plane as the original operation, or through a different plane.
- Mirror creates a mirror image of the selected operations. Like Rotate, you can mirror the operation in the same plane or in a different one.
Choose the transformation method:
- Tool plane transforms the selected operations in a different orientation than the original and transforms the tool axis with the operation. An operation's tool plane contains both an origin and a plane. You can choose to change the origin along with the plane or keep the origin stationary when Mastercam transforms/copies the tool plane. If you keep the origin stationary, Mastercam transforms only the tool plane. The Tool plane option also activates the Work offset numbering parameters so that you can output a different work offset with each new tool plane.
- Coordinate computes new coordinates for the transformed operation in the same tool plane as the original operation.
Choose the operation types to create. You can create Transform operations, new toolpath operations, or both. In general, transform operations maintain associativity with the original operations. The new toolpath operations option lets you edit each individual toolpath that Mastercam creates from the Transform operation. In addition, this option copies the toolpath geometry to each transform location.
You can associate different work offsets with each transformed operation. Choose one of the following Work offset numbering options:
- Automatic automatically assigns a matching work offset number (if one exists), or the next available number if no matching work offset number is found.
- Maintain source operation's uses the same offset as the original toolpath.
- Assign new creates a different offset for each new operation based on the specified values. Enter a start value, increment, and select By instance or By tool plane. If you select Match existing offsets, Mastercam checks for an existing offset that matches a particular Transform. If a matching offset exists, Mastercam uses it instead of creating a new one.
Remove comments
Removes comments that exist in the selected source operations from the transformed operations. Deselect to copy comments from the source operations to the transformed operations.
Source operations
Select the operations to transform from the current machine group.
- With the exception of Manual operations, operations that do not contain NCI code are excluded from the selection list—for example, trimmed operations, or FBM Drill and FBM Mill parent operations.
- Operations that already reference a Transform operation are also excluded from the list. This includes any sub-programs referenced by another Transform operation.
- You can select operations based on solid models. If you also activate Create new operations and geometry, Mastercam saves the geometric entities it generates from the solid to create the transformed operations. These entity types include surfaces, chains, and points. Mastercam does not copy the solid model.
Comment
Enter a text comment for the operation.
Translate
Copies toolpaths to a new location. This option activates the Translate tab, where you can set the location, plane (if desired) and number of copies.
Rotate
Revolves toolpaths about a specified point in a plane. This option activates the Rotate tab, where you can set the rotation point, plane of rotation, and number of copies.
Mirror
Replicates toolpaths about the X axis, the Y axis, or a specified entity. This option activates the Mirror tab, so you can specify the orientation and toolpath direction.
Tool plane
Creates a new tool plane (Tplane) for the transformed toolpath. This activates the work offset options so that you can assign new work offsets to each copy of the toolpath.
Include origin
Available only for the Tool plane transform method. An operation's tool plane contains both an origin and a plane. Transforms the operation's tool plane and its origin. Deselect to transform only the tool plane, keeping the origin stationary.
Include WCS
Creates a new WCS plane when transforming a toolpath by tool plane.
Save planes
Saves the new tool plane Mastercam creates during the operation transformation.
Coordinate
Creates new coordinate positions for the new toolpaths in the original tool plane.
NCI
Copies and transforms only the source operation's NCI lines to the transformed operations.
Geometry
Copies and transforms the geometry needed for toolpath creation from the source operations. This method generates new NCI for the transformed operations.
Operation order
Sorts the transformed operations by the order they were selected. For example, if you select a Pocket and a Contour operation and then transform them, Mastercam executes them in that order (Pocket, Contour, Pocket, Contour, etc.)
Unique subprograms
Creates subprograms for each source operation separately instead of making subprograms for a selected block of operations.
Operation type
Groups the transformed operations by the operation type. For example, if you select a Pocket and a Contour operation, all transformations of the pocket operation are executed together, as are all transformations of the contour operation (Pocket, Pocket, Contour, Contour, etc.)
Create new operations and geometry
Copies geometry from the original operation to each transform location and applies the parameters from the original operation to each new toolpath. This method creates several new independent operations with the same geometry and parameters instead of a single transform operation.
Keep this transform operation
Keeps the transform operation in addition to the new operations and geometry. This allows you to regenerate all of the resulting operations quickly by regenerating the transform operation. Only available if Create new operations and geometry is enabled.
Copy source operations
Creates a duplicate operation directly above the source operation.
Disable posting in selected source operations
Prevents source operations from being posted twice by disabling posting for the source operation. Only available if Copy source operations is enabled.
Subprogram
Sets values in the subprogram lines in the NCI file to indicate a section of the operation that is repeated at a different location (for example, a drill cycle or depth cut). This information is then passed to the post processor. The control definition must be set to support subprograms for this function to work.
Absolute
Tells the post processor to output absolute coordinates in the NC subprogram. An absolute subprogram contains absolute coordinate values; in other words, the same points are machined every time the subprogram executes. Typically an absolute subprogram has a G90 code.
Incremental
Tells the post processor to output incremental coordinates in the NC subprogram. With an incremental subprogram, the points machined are relative to the tool's location when the subprogram is called. Typically an incremental subprogram has a G91 code.
Automatic
Automatically assigns a matching work offset number (if one exists), or the next available number if no matching work offset number is found. Work offsets can exist assigned to planes, in a toolpath operation's Tplane, and in a transform operation's NCI. Mastercam searches for existing work offset numbers in that order. The value for Automatic is -1.
Maintain source operation
Uses the work offset settings from the source operation for each transformation. Only available for Translate and Rotate toolpaths using the tool plane method.
Assign new
Creates new work offset numbers for each translation. The work offset numbers begin with the specified Start number and increase by the Increment number with each new translation.
By instance
Assigns a new work offset numbers based on operation instance. Each instance is given a new work offset number regardless of tool plane.
By toolplane
Assign new work offset numbers based on tool plane. Each change in tool plane is given a new work offset number.
Match existing offsets stored in planes
Checks to see if any of the work offset planes that are created when the toolpath is posted match any existing or predefined planes. If the planes match, then the existing plane is used. If the planes do not match, a new work offset plane is created.
Custom Parameters
Applies the values for any custom parameters that have been defined for the transformed operation. Click Custom Parameters to see the list of custom parameters or to edit the values. Use the corresponding Text page in the Control Definition Manager to define the custom variables.





