Cut Parameters: Model Chamfer
Use this page to enter cutting parameters for a Model Chamfer toolpath.
| 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. |
Compensation type
Choose how you want to handle cutter compensation:
The available options are determined by the active control definition.
Compensation direction
Offsets to the tool based on the selected direction. Choose one of the following:
- 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.
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 cutter compensation in control
Eliminates arcs in the toolpath that are less than or equal to the radius of the tool and helps prevent gouging. Only available when Cutter compensation is set to Control.
Roll cutter around corners
Inserts arc moves around corners in the toolpath. Select None to guarantee all sharp corners, Sharp to only roll the tool around sharp corners (135 degrees or less), or All to roll the tool around all corners and create smooth tool movement. The radius of the arc moves equals the radius of the tool.
Infinite look ahead
Prevents the toolpath from crossing itself to protect against gouging.
Internal corner rounding radius
Creates smoother tool motion in sharp corners. Corner smoothing reduces tool wear and makes your tool motion more efficient.
External corner break radius
Enter a radius value to break external sharp corners defined within a chain to create a smooth, rounded corner.
This option will violate the defined chains and cut into the defined geometry.
Without an External corner break radius:
With an External corner break radius:
Maximum depth variance
Sets the amount that the Z value of the endpoints of 3D entities can be adjusted to make a smooth intersection during cutter compensation. A smaller value creates a more accurate representation of entities, but may insert an extra step move to meet an intersecting entity. A larger value means that Mastercam may not make the step move, but provides a less accurate representation of the entities' actual depth.
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.
Maintain sharp corners
Available only when a positive Stock to leave on walls value is entered. Rolls your tool around sharp corners while including the stock amount. The following images display how selecting this option affects your toolpath:
- Roll cutter around corners set to Sharp.
- Stock to leave on walls set to 0.0.
-
Maintain sharp corners is not selected.
- Roll cutter around corners set to Sharp.
- Stock to leave on walls set to 0.175.
-
Maintain sharp corners is not selected.
- Roll cutter around corners set to Sharp.
- Stock to leave on walls set to 0.175.
-
Maintain sharp corners is selected.
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.
Chamfer width
Defines the width from the chained geometry adjusted by the cut depth defined on the Linking Parameters page.
Top offset
Defines how far the full diameter of the tool is above the top rail of the chamfer.
Bottom offset
Defines how far the tip of the tool is from the bottom of the chamfer.
Depth
Defines the depth of the bottom of the chamfer when using a ball or bullnose tool.
Mastercam alerts you if the tool you selected for the toolpath is not wide enough to accommodate both the defined Chamfer width and Top offset.





