Cut Parameters: Radial
Use the Cut Parameters page to configure the cutting passes for a Radial toolpath. Use radial toolpaths to create cutting passes that radiate outwards from a central point. Select a Cutting method to organize and orient the cuts. You can choose to create one-way cuts in either direction; zig-zag cuts in both directions; or up/down mill.
Then, define the machining zone with the center point of a circle and its outer radius. Mastercam will project this circle onto your selected drive surfaces and calculate the toolpath within this area. Mastercam automatically calculates a default center point and outer radius based on your selected geometry. You can edit these if you wish. Enter an inner radius to define a zone around the center point that is not machined. This is useful to prevent overmachining near the center point.
| 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. |
Cutting method
Orients the cutting direction. Select one of the following options:
- Zigzag: Cuts each pass in the opposite direction to the previous pass. A short linking motion connects the two ends.
- One Way: Cuts one direction, steps over to the next cut while making a rapid move to same start side of the cut, and cuts in the same direction as the previous pass.
- Other Way: Cuts maintaining a conventional orientation throughout the operation.
- Down Mill: Cuts in only the down direction.
- Up Mill: Cuts in only the up direction.
Tip compensation
Select whether the compensation point will be the center of the tool or the tip. Compensating to the center of the tool is frequently used with ball cutters where compensation is applied at the control.
Optimize cut order
Keeps the tool within an area until all cuts in that area are completed.
| Optimize cut order off | Optimize cut order on |
|---|---|
|
|
Stepover
Places the tool in an area and keeps it there until all cuts in the area are made. This is a 2D value measured parallel to the tool plane.
Scallop height
Unavailable for tools with a corner radius equal to zero. Specifies the spacing between cutting passes in terms of the height of the scallop that is left. Mastercam will calculate the Stepover based on the value that you enter here and the selected tool.
The Stepover and Scallop height fields are linked so that when you type a value in one field, the other is automatically upated. This lets you specify the spacing between your cutting passes in terms of either the Stepover distance or the Scallop height. Scallop height is calculated against a flat surface. Bull nose tools produce no Scallop height unless the Stepover is large enough.
Center point
Enter the X and Y coordinates of the center point of the machining zone. Mastercam will project this point onto the drive surfaces to determine the starting point of the toolpath, so a Z coordinate is not necessary. Right-click in each field to select the X or Y coordinate from geometry in the graphic window.
Inner radius
Creates cutting passes in the circles defined by the Inner radius, outer radii, and the Center point, and projects them onto your drive surfaces. Enter 0 to machine the entire circle, or enter a non-zero value to machine only the ring between the two radii. This can be a useful technique to prevent overmachining the center of your part.
Outer radius
Creates cutting passes in the circles defined by the Inner radius, outer radii, and the Center point, and projects them onto your drive surfaces. Mastercam automatically calculates the Outer radius based on the selected geometry.
Angles (Start/End)
Use these values to limit the radial cutting passes to a specific angle sweep within the machining zone. Each value is measured relative to the positive X-axis. For example, enter 0 and 90 to create cutting passes in only the X+ Y+ quadrant of the circle, or 90 and 180 for the X– Y+ quadrant. Mastercam will not calculate a toolpath unless you enter a value between 0 and 360 in the End field.
Overlap (Down/up mill)
Enter a distance here to ensure that the toolpath does not leave unwanted scallops or cusps in the transition areas between passes of different direction.
Shallow angle (Down/up mill)
In areas where the Machining geometry is almost flat, there is no advantage to machining up or down. Mastercam creates either down or up milling passes. Enter the angle that defines the region where this can occur.





