Cut Parameters: Pencil
Use the Cut Parameters page to configure the cutting passes for a Pencil toolpath. Use this toolpath to create additional finish passes along the intersections between two or more surfaces.
| 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: Starts with climb cutting and cuts each pass in the same direction.
- Other Way: Starts with conventional cutting and then cuts each pass in the same direction.
- 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.
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.
Maximum number of offsets
Select and enter the maximum number of offsets for cutting passes.
Reference tool diameter
This setting is available when you use multiple offsets. It represents the size of the theoretical roughing tool that would have machined the cutting zone defined for your pencil toolpath. Use it as a guide to make sure that you are in fact machining all of the areas that were missed by your roughing tool. In other words, if the value is greater than the actual tool you used for your roughing operation, you can be confident that the pencil toolpath will reach all of the areas that could not be roughed.
If you manually override the calculated diameter with a different value, Mastercam will adjust the number of offsets. In other words, if you know how wide your machining zone needs to be, you can enter that value directly in the field and Mastercam will automatically calculate the proper number of cutting passes for your selected finishing tool. This distance is measured from each side of the surface boundaries. For example, if the Reference tool diameter is 20mm, the machining zone will be 40mm wide with the surface boundary in the middle. Once you manually override the calculated value, Mastercam will not automatically change it again.
Overthickness
Use this option to increase the apparent size of the cutter to force a cutting pass when one would not ordinarily be created. This can also be useful when the size of the cutter is equal to, or very close to, the size of the fillet; entering an Overthickness amount greater than the Cut tolerance helps ensure that Mastercam will create a smooth continuous pass through the pencil zone.
Bitangency angle
Specifies how shallow the corner or angle between two surfaces needs to be in order for Mastercam to create a cutting pass. Use this to prevent cutting passes where the transition between two surfaces is flat or nearly flat. A typical recommended value is 165 degrees.
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.





