Cut Parameters: Hybrid
Use this page to configure the cutting passes for a Hybrid toolpath. This is a finishing toolpath which generates waterline-style cut passes for steep regions and scallop cut passes for shallow regions. Mastercam switches smoothly between both styles to cut in a logical optimized order.
| 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. |
Closed contour direction
Orients the cutting direction of the closed contours. Closed contours contain continuous motion without a need for a retract or reversal of direction. Select one of the following options:
- Climb: Cuts in one direction with the tool rotating in the opposite direction of the tool motion.
- Conventional: Cuts in one direction with the tool rotating in the same direction as the tool motion.
Open contour direction
Orients the cutting direction of the open contours. Select one of the following options:
- One Way: Cuts the open contour by taking a pass, moving up to the retract height, moving back to the beginning of the cut, and taking another pass in the same direction. All passes are in the same direction.
- Zigzag: Cuts each pass in the opposite direction to the previous pass. A short linking motion connects the two ends.
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 |
|---|---|
|
|
Z stepdown
Defines the constant Z distance between adjacent stepdowns. Mastercam uses these stepdowns in combination with the Limiting angle and 3D stepover to calculate cut passes for the Hybrid toolpath. Mastercam first slices the entire model into sections defined by the Z stepdown distance. It then analyzes the drive surface's slope transition between each stepdown along the specified Limiting angle. If the drive surface's slope transition within the stepdown distance is less than the applied Limiting angle, the Hybrid toolpath considers it steep and a single 2D waterline cutting pass is generated. Otherwise, the stepdown is defined as shallow. Mastercam uses the 3D stepover to create 3D scallop cut passes along the shallow slope.
Limiting angle
Sets the angle that defines the shallow region on the part. A typical limiting angle is 45 degrees. Mastercam adds or removes cuts in an area that ranges from zero to the limiting angle.
- Steep stepdown
- Limiting angle (applied)
- Steep
- Shallow
3D stepover
Defines the spacing between 3D scallop-style cutting passes in shallow stepdowns.
Preserve Z passes
Select to maintain Z passes in steep areas. Passes in shallow areas are calculated based on the Offset method. Deselect to calculate collapse motion across the entire part when a shallow region is encountered.
Offset method
Select a method for handling the boundaries between steep and shallow areas from the drop-down.
- Closed offsets: The boundaries are treated as closed chains when calculating the 3D collapse motion.
- Upper to lower: The boundaries are treated as closed or open chains that collapse from the highest Z value to the lowest.
- Lower to upper: The boundaries are treated as closed or open chains that collapse from the lowest Z value to the highest.
- Automatic: If the toolpath engages part surfaces that includes core and cavity properties, Mastercam applies upper to lower offset methods to core features and lower to upper offset methods to cavity shapes.
Flat detection
Allows you to control how the toolpath handles machining flat surfaces.
Flat area
Enabled when Flat detection is selected. Select the type of flat processing:
-
Include flats: Select to include flat surfaces when machining, regardless of the Limiting angle. You can then set a separate stepover for the flat surfaces. The image below shows this option, as well as a separate stepover for flat surfaces.
-
Ignore flats: Select to not machine any flat surfaces.
-
Flats only: Select to only machine flat surfaces.
Smoothing
Smooths sharp corners and replace them with curves. Eliminating sharp changes of direction results in a more even load on the tool and lets you consistently maintain a higher feed rate.
- Angle: Sets the minimum angle between two toolpath segments that you want Mastercam to consider as a sharp angle.
- Blend distance: Sets the distance Mastercam will back away from the sharp corners before and after.





