Cut Pattern: Curve
Use the Cut Pattern page to establish the cut pattern parameters for a Multiaxis Curve toolpath. Cut pattern settings determine the geometry your tool follows and how it travels along that geometry.
| 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. |
Curve type
Select the type of geometry to be used for the drive curves:
- Use 3D curves when you have chained geometry to cut. The 3D curves can be chains or from solid selection. The curves will be projected onto a surface for toolpathing.
- Use Surface edges when you are not using chained geometry. You will return to the graphics window to select surfaces and a single edge to cut, or an edge to start on if you chose Surface edge - all. Use Select to return to the graphics window for geometry selection. The number of curves selected will be displayed to the right of the button.
Compensation type
Choose how you want to handle Compensation type:
- Computer: Mastercam computes the compensated toolpath and does not output control codes for compensation.
- Control: Mastercam outputs control codes for compensation and does not compute the compensated toolpath.
- Wear: Mastercam both computes the compensated toolpath and outputs control codes for compensation. Compensation direction in the computer and control are the same.
- Reverse wear: Mastercam both computes the compensated toolpath and outputs control codes for compensation. Compensation direction in the computer and control are opposite.
- Off: Mastercam programs the tool tip directly on the chained geometry and does not output compensation codes. The options that are available to you are determined by the active control definition.
Compensation direction
Choose to offset the tool to the right or left of the toolpath. Even if Compensation type is set to Off, Mastercam uses this setting to determine the orientation of other toolpath features such as multiple passes.
Tip compensation
Sets amount of offset to the tool's center or tip for bull-nose and ball (spherical) tools. Used for touching the tool off the part. Outputs the tool tip offset as either the tip or the corner radius distance from the tip.
Radial offset
Sets the distance that the center of the tool is offset (left or right) based on the Compensation direction.
Diameter for simulation
Only available when Compensation type is set to Control, Wear, or Reverse wear. Enter a value to be used by Backplot and Verify to represent a control compensated tool. The field is initially given the value of the tool selected for the operation, with the ability for the user to override this value.
Distance increment
Select the checkbox and enter a value. The value is a linear distance along the path taken by the tool. An additional vector will be added to the toolpath when the distance between calculated vectors is greater than the distance increment value.
Distance
Select to use a distance value to limit tool motion. The specified value is the distance between generated vectors along the selected geometry. A smaller value creates a more accurate toolpath, but may take longer to generate and may create a longer NC program.
Cut tolerance
Determines the accuracy of the multiaxis toolpath. A smaller cut tolerance value creates a more accurate toolpath, but may take longer to generate the toolpath and create a longer NC program. This value is also used to eliminate duplicate positions and as a tolerance when compensating to surfaces.
When Distance is deselected, Mastercam uses the cut tolerance you specify as a tolerance to fit tool positions to the surface based on the curvature of the surface. Otherwise, Mastercam uses the Distance value as an absolute distance for the space between each tool position.
Maximum step
Enter a value for the maximum space allowed between tool vectors. Additional vectors may be desirable in areas where the tool travels in a straight line for a large distance. Not available if you select the Distance option.





