Setup: Mill-Turn 2D/3D
Use this page to define the setup for a mill operation in Mill-Turn. This includes choosing a setup type, tool plane, axis combination, spindle origin, and work offset value.
Mastercam supports the following setup types.
Only available options, based on the capabilities of the machine and the selected geometry, will display.
See the application guide associated with your .machine file for specific information about how these options are implemented for your machine.
-
C-Axis Face: Select to enable polar interpolation for operations where the tool axis is parallel to the rotary axis. This option is useful for occasions where you wish to mill the face of your part.
For many controls, this setup type lets you choose between longhand or cycle output. For example, on a Fanuc control this might be a G12.1 or similar command.
-
Axis Substitution: Select to enable cylindrical interpolation for operations where the tool axis is perpendicular to the rotary axis. This option is useful for occasions where you wish to mill around the outside diameter of your part.
For many controls, this setup type lets you choose between longhand or cycle output. For example, on a Fanuc control this might be a G7.1 or similar command.
NOTEMill-Turn toolpaths that use Axis Substitution cannot be transformed.
-
Multiaxis: Select to create a multiaxis drill operation (4-axis or 5-axis output). You can also choose any of the other setup types to create a 3-axis drill operation.
This setup type enables the Tool Axis Control page and the Safety Zone page.
-
Y-Axis Face: Select to enable Y-axis machining for operations where the tool axis is parallel to the rotary axis.
-
Y-Axis Cross: Select to enable Y-axis machining for operations where the tool axis is perpendicular to the rotary axis.
-
Plane Rotation: Select to enable coordinate conversion (tilted-plane) machining cycles. This option rotates the coordinate system plane to simplify your NC output.
For many controls, this setup type lets you choose between longhand or cycle output. For example, on a Fanuc control this might be a G68 or similar command.
For C-Axis Face and Axis Substitution setup types, Mastercam automatically selects the Toolplane from the planes that were created during the Job Setup process. Each plane sets the proper tool orientation for your part.
For Multiaxis, Y-Axis Face, Y-Axis Cross, and Plane Rotation setup types, you tell Mastercam how to establish the tool plane.
-
For most applications, you will want Mastercam to automatically create a tool plane based on the selected geometry. Select the Derive from geometry option to do this.
The name for the new plane is displayed at the bottom of the dialog box. Mastercam tries to create a name that describes its rotation.
-
You can also use an existing tool plane instead of creating a new one from the geometry. To do this, deselect the Derive from geometry option and select an option from the Toolplane drop-down.
Depending on the setup type, you may choose to automatically keep the axes for a generated tool plane aligned with the machine axes, as well as leave the spindle origin at the location defined in Job Setup.
| Icon | Name | Description |
|---|---|---|
|
Detect (FBM Drill) | Analyzes the solid model and detects features based on the Feature Based Machining (FBM) operation's current parameters. View the results of all detected features and their machining information in the Features page. For more information, please refer to Detection States and Modes in FBM. |
|
Reselection is not available | Hole Wizard features for a Wizard Holes operation can only be selected in Mastercam for SOLIDWORKS. Contact your Reseller for more information. |
|
Preview toolpath operations (FBM Drill/Wizard Holes) | Opens the Toolpath Operations Preview dialog box where you can view the list of operations FBM will generate using the current Features page list. |
|
Save parameters to defaults file | Makes the current toolpath settings the default for future toolpaths of this type. Saves the current values in the toolpath properties pages to the .mcam-defaults file specified in the machine group properties. |
|
Reload parameters from defaults file | Overwrites the current values in the toolpath properties pages with the toolpath's default parameters. These parameters are reloaded from the .mcam-defaults file specified in the machine group properties. |
|
Hide dialog | Minimizes the dialog box so that you can use other Mastercam functions, like changing your shading settings or the graphics window view. When finished, press [Esc] to maximize the dialog box. |
|
Tool Manager | Opens the Tool Manager. Use the Tool Manager to create and edit tool definitions and to work with tool libraries. When you close the Tool Manager, the toolpath dialog box will reappear just as you left it. |
|
Feed speed calculator | Opens the Feed & Speed Calculator dialog box where you can modify the calculated feed rate or spindle speed by adjusting the material and tool parameters. |
|
None |
Page window | This window displays all of the pages that are available to you, depending on the selected toolpath type. A green check mark indicates pages where data has changed in the current session. |
| None | Quick View Settings | This window summarizes key toolpath information from the Tool page, Coolant page, and Planes page. It updates automatically as you make changes to the different pages and is always visible. |
| None | Generate toolpath | When selected, automatically generates the toolpath when you click OK. For more information, refer to Accepting and Generating Toolpaths. |
|
OK | Generates the toolpath and closes the dialog box. If editing a toolpath, applies the changes and closes the dialog box. |
|
Apply | Applies your changes to the toolpath without closing the dialog box. |
|
Cancel | Closes the dialog box and cancels the toolpath creation. If editing a toolpath, any changes to the toolpath are discarded. |
Mill type
Select the mill type to use for the current operation. Mill types in the upper row move the rotary axis during toolpath motion, while mill types in the bottom row only use the rotary axis for positioning.
Axis combination
Select the axis combination to use for the current operation. Only available combinations for the current machine will be displayed.
Toolplane
Select the appropriate tool plane from the drop-down selection. Standard system planes and planes created by Job Setup are available.
Align with machine
This option is used for Y-axis Cross and Plane Rotation operations where the tool plane is based on the toolpath geometry. Select this option to transform the tool plane so that it is aligned with the machine coordinate system axes. Note that this changes the orientation of the tool plane, but not the origin. Select the Maintain spindle origin option to move the origin also.
Derive from geometry
Select to create a tool plane from the selected geometry.
The Derive from geometry option will only be available if the selected geometry defines a plane. For example, if the chained geometry is only a single line, the option will be grayed out because you cannot specify a plane based on only a single line.
Maintain spindle origin
If the origin of the selected tool plane is not the same as the origin defined on the Toolplane Origin Z page in Job Setup, this option creates a copy of the tool plane with the same origin defined in Job Setup.
Use alternate B-axis solution
Select to choose the second B-axis solution, which is 180 degrees from the initial C-axis position.
Rotary diameter (Axis Substitution)
Enter the roll diameter for the operation. Click Select to return to the graphics window to select the diameter from existing geometry.
Internal cutting (Axis Substitution)
Select to create the toolpath on the inside of the rotary diameter. An example would be when cutting an internal groove.
Flat geometry (Axis Substitution)
Select when the geometry used in the operation is planar. The flat geometry is rolled around the rotary diameter during toolpath creation.
Reverse geometry (Axis Substitution)
Select to reverse the direction the geometry is rolled around the rotary diameter.
Geometry is in Top plane (Axis Substitution)
Select only if the geometry used in the operation is in the Top plane.
Wrapped geometry (Axis Substitution)
Select when the geometry used in the operation lies in 3D space. The geometry typically lies around the rotary diameter.
This option is only available for Drill, Contour, and Pocket toolpaths.
Unroll tolerance (Axis Substitution)
Determines how finely to break up rotary axis geometry during unrolling.
Unroll seam angle (Axis Substitution)
Reverses rolled entities to make them lie flat. Each chain starts somewhere between 0 and 360 degrees. Sometimes, the zero degree position runs through several chains. As a result, some chains will start before 360 degrees and some will start after 0 degrees.
When the chains are unrolled, they end up 360 degrees apart. The toolpath rapids between the chains across the 360-degree gap. This causes many 360-degree rotations in the middle of the toolpath. The Unroll seam angle option lets you specify the angle to split the geometry so that it all finishes on the same side of the seam. The unroll zero angle will not change; instead some of the geometry will be shifted 360 degrees.
Spindle origin
The selected tool plane is displayed unless Maintain spindle origin is selected, in which case the spindle selected for the axis combination is displayed.
Work offset
Enter the work offset value to apply to the selected tool plane. This field is unavailable if Maintain spindle origin is selected.
Plane selection and creation information
Read-only. Displays the selected tool plane when no other options are selected on this page. The information changes when Align with machine and/or Maintain spindle origin are selected. When either option is selected the displayed information reflects the created plane.





