Cut Parameters: Blend Mill
Use this page to control the cutting motion Mastercam uses between the two open chains you selected for the 2D High Speed Blend Mill toolpath. The blend cutting method can be Zigzag, One way, Spiral, From center, or To center. The Along or Across options let you create cuts that start with the first blend chain and then morph toward the second blend chain in either an across or along direction. For along cuts, you can change the resolution of the tool stepover. Extending your entry or exit motion allows for fine tuning of the toolpath.
If your part has a consistent shape in the region between the blend curves or if the blend curves are similar in shape, you may be able to make the resolution less refined: use a larger distance or percentage of stepover, 500% or 1000%, for example. A larger stepover reduces the toolpath calculation time.
If your part has many small features (bosses or cavities), then you might need to make the resolution more refined: use a smaller distance or percentage of stepover, 50% or 25%, for example. A smaller stepover increases the toolpath calculation time but the toolpath will maintain a consistent stepover.
| 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.
- Spiral: Cuts in a continuous motion from one boundary to the other.
- From Center: Cuts one direction, steps over to the next cut, and cuts in the opposite direction starting from the center and working its way outside while maintaining a climb cut.
- To Center: Cuts one direction, steps over to the next cut, and cuts in the opposite direction starting from the outside and working its way to the center while maintaining a climb cut.
Compensation direction
Offsets to the tool based on the selected direction. Choose one of the following:
- Off: The tool center is allowed to travel to the selected chains.
- Left: The tool is allowed to travel to the left of the selected chains.
- Right: The tool is allowed to travel to the right of the selected chains.
- Inside: The tool stays between the selected chains.
- Outside: The tool is allowed to travel to the outside of the selected chains.
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.
First pass feed reduction
Reduces the feed rate of the first pass of the toolpath entering stock from the outside.
Maximum stepover
A smaller maximum stepover value may take longer to generate the toolpath.
Across
Cuts from one chain to the other, beginning at the start point of the first selected chain.
Along
Cuts in the along direction stepping over in the across direction.
Distance / Percent of stepover
Sets the spacing between the temporary across moves. These moves are used to generate final along cuts, but are not included in the final toolpath.
Extend Entry/Exit
Use these fields to adjust the initial and final tool engagement with the material. Select the checkbox to active the option, then enter an Additional entry/exit distance. By default the initial cut is defined by the stepover amount. Mastercam adds the additional amount you specify to the beginning and/or end cut. These options are useful if the part geometry between the two chains is something other than a straight line, such as a slot that spans the corner of a part.
Extend entry off:
Extend entry on with an applied extension value:
Stock to leave on walls
Sets the amount of stock on selected vertical machining geometry. Enter a positive value if you do not want to remove all stock or enter a negative value to remove more stock. If the machining geometry (or a portion of it) is not vertical, Mastercam interpolates a value between the Stock to leave on floors and Stock to leave on walls amounts.
Stock to leave on floors
Sets the amount of stock on selected horizontal machining geometry. Enter a positive value if you do not want to remove all stock or enter a negative value to remove more stock. If the machining geometry (or a portion of it) is not horizontal, Mastercam interpolates a value between the Stock to leave on floors and Stock to leave on walls amounts.





