Toolpath Control: Dynamic OptiRough
| 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. |
Boundary chains
Select one or more closed chains that limit tool motion.
Automatic boundary
Mastercam creates a boundary around the selected Machining geometry and uses it as a containment boundary in addition to any selected Boundary chains. Select from the following:
-
None: No boundary is created. The Include stock option is automatically applied.
-
Silhouette: Creates a boundary that is a silhouette of the selected Machining geometry and Boundary chains.
-
Bounding rectangle: Creates a rectangle as a boundary.
-
Bounding circle: Creates a circle as a boundary.
Include stock
Includes the stock settings from the Stock page for the selected Automatic boundary. If Automatic boundary is set to None, this option is automatically applied.
Strategy
Select how the toolpath machines the selected geometry.
-
Stay inside: This strategy is enabled by default and keeps the toolpath inside the selected machining geometry. Use this strategy when machining pockets.
-
From outside: Select to use free-flowing motion to machine features, such as standing bosses or cores. A toolpath using this strategy starts from the outside and work its way in.
Contain
Select one of the following options:
- Tool tip: Confines the tool center inside the containment boundary.
- Tool contact point: Confines the tool contact points inside the containment boundary instead of the tool center. The tool center may run outside the selected boundary, but the contact point of the tool will not.
Compensate to
Select how the toolpath compensates to the selected Boundary chains:
- Inside: Results in a toolpath where the entire tool remains inside the Boundary chains. Selecting this option allows you to adjust the boundary's offset distances.
- Center: Results in a toolpath where the center of the tool travels to the containment boundary. You cannot make adjustments to the offset distances.
- Outside: Results in a toolpath where the outer edge of the tool is bound to the containment boundary. Selecting this option allows you to adjust the boundary's offset distances.
Offset distance
Adjusts the inside or outside tool containment. For example, to ensure that the tool is completely clear of the containment boundary, you might enter a value of 0.050 inches. Or, to ensure that the tool overlaps the boundary, you can enter of a value of +/- 0.050 inches. For both inside and outside containment, enter a positive value to move the tool away from the boundary, and a negative value to pull it towards the boundary.
Include tool radius
When selected, the Offset distance is an incremental value that is added to the tool radius. Use this option to ensure that the tool is always clear of (or overlaps) the tool containment boundary by the Offset distance. When deselected, the Offset distance represents the total distance between the tool center and the containment boundary, regardless of the tool size.
Total offset distance
Read-only. Displays the net distance between the Boundary chains and the center of the tool. It takes into account the following dimensions:
- The size of the selected tool.
- The amount of the Offset distance.
- Whether Include tool radius has been selected.
Skip pockets
Enables the skip pocket parameters. This is useful when the pocket is large enough to accommodate the tool, but the entry move is so compressed that the tool is effectively plunging into the part when Mastercam attempts to machine it.
- Skip all: Skips all pockets.
- Smaller than: Specifies a minimum pocket size for creating
cutting pass. While you can set these values to 0 to ensure that entire surface will be machined, a low value on a cutting area that is too small will result in the tool plunging straight down in the pocket. A more typical value to use is 110% of the tool diameter.
- Tool diameter percentage: Enter a minimum pocket size, as a percentage of the tool diameter. The right field updates to display this value as the minimum pocket size.
Minimum pocket size: Enter a minimum pocket size to create cutting passes. The left field updates to display this value as the tool diameter percentage.
Approximate start point
Select the point near the start of the toolpath. If the toolpath has several machining regions, the Approximate start point indicates which region is first.
Curve
Returns you to the graphics window to select curves. When curves are selected, the toolpath is created outward using the curves as a starting point.
If the selected Curves lie entirely outside of the set Minimum depth or Maximum depth on the Steep/Shallow page, then you receive an error when generating the toolpath. The curves must be inside the set limits.
Points
Returns you to the graphics window to select points that will be projected onto the selected surfaces or solids.





