Cut Parameters: Horizontal Area
Use this page to configure the cutting passes for a Horizontal Area toolpath. This toolpath creates finish passes over a flat area. Mastercam will create multiple cutting passes which represent the surface boundary offset by a stepover value.
| 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:
- 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.
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.
Number of depth cuts
Removes the stock in several passes. Use this when there is too much stock left on the part to plunge all the way to the surface. A value of 1 allows the tool to make a single cut at the programmed depth; enter a value greater than 1 to create additional cuts.
Stepdown (Depth cuts)
Enabled when Number of depth cuts is set to 2 or greater. Determines the Z spacing between adjacent cutting passes.
Percentage of diameter (XY stepover)
Expresses the maximum XY stepover as a percentage of the tool diameter. The Maximum (XY stepover) field will update automatically when you enter a value in this field. The actual stepover is caFlculated by Mastercam between the Minimum and Maximum values.
Minimum (XY stepover)
Enter the smallest acceptable distance that you want Mastercam to use for a stepover distance between two cutting passes. Mastercam will calculate an XY stepover that lies between the minimum and maximum values that you enter here.
If you are using Corner rounding, make sure that the Minimum stepover is greater than the Offset tolerance value and less than the radius of the tool shaft.
Maximum (XY stepover)
Enter the largest acceptable distance that you want Mastercam to use for a stepover distance between two cutting passes. Mastercam will calculate an XY stepover that lies between the minimum and maximum values that you enter here.
This field is linked to Percent of diameter, so that you can express the maximum stepover as either an absolute distance or as a percentage of the tool diameter. When you make an entry in one field, the other automatically updates. The default maximum stepover is 45% of the tool diameter. Ensure that the maximum stepover is at least twice as large as the minimum stepover.
Corner rounding
Activates toolpath corner rounding, which replaces sharp corners with arcs for faster and smoother transitions in tool direction. Once you activate corner rounding, set the maximum radius, profile tolerance, and offset tolerance.
- Maximum radius: Enter the radius of the largest arc that you will allow Mastercam to insert to replace a corner. Larger arcs result in a smoother toolpath, but with greater deviation from the originally programmed toolpath.
- Profile tolerance: Represents the maximum distance that the outermost profile of a toolpath created with corner rounding can deviate from the original toolpath.
- Offset tolerance: Represents the maximum distance that a profile of a toolpath created with corner rounding can deviate from the original toolpath. This is the same measurement as the profile tolerance but is applied to all the profiles except the outermost one. This lets you maintain different tolerances for the first profile and subsequent profiles.





