Cut Parameters: Dynamic OptiRough
Use the Cut Parameters page to enter values for cutting parameters and compensation options for Dynamic OptiRough toolpaths, a high speed roughing toolpath capable of machining very large depths of cut.
| 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.
- Zigzag: Cuts each pass in the opposite direction to the previous pass. A short linking motion connects the two ends.
Conventional feed rate
Sets an alternate feed rate for the conventional motion of a zigzag cut. Enter a percentage of the programmed feed rate or a value.
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 stepups
Defines the cut order Mastercam applies to different cutting passes in the toolpath.
- By depth: Mastercam machines all cut passes Z-level by Z-level.

- Next closest: Mastercam moves to the closest cut from where it finished the previous cut.

- By pocket: Mastercam first machines all the stepdowns, moving from pocket to pocket. After all
stepdowns on a Z-level are machined to completion, Mastercam machines the stepups
by next closest, in the safest cut order.

Optimize stepdowns
Controls the cut order Mastercam applies to different cutting passes in the toolpath. When the tool finishes a machining pass, it must select a start point to resume. The start points can be set as the following. The images below show a toolpath with Classic Backplot to help show the differences between the options. The numbers indicate the order of machining to also help visualize the options.
-
Material: Set by default. Starts at the material that is closest to the entire tool. Mastercam attempts to do smaller pieces within a general area when pieces of material become isolated before moving on.
-
None: No optimization is applied to the cutting passes.
-
Air: Starts nearest to the tool. Mastercam attempts to create the shortest possible air moves between machining areas.
Stepover
Sets the distance between cutting passes in the X and Y axes. Enter a percentage of the tool diameter, an absolute distance, or an angle. The value or percentage is limited to 95% of the tool's flat diameter. A larger value will automatically be reduced to the 95% limit after a warning message. Be aware when using a bullnose tool that the percentage is a calculation based on the tool's flat diameter.
The field becomes a drop-down selection when the following conditions exist:
- An ISCAR CHATTERFREE tool is selected
- The Iscar HEM checkbox in the Tool page is selected
Your options then become 5%, 7%, and 10%.
Stepdown (Passes)
Determines the Z spacing between adjacent cutting passes.
Stepup
When this option is selected, Mastercam calculates and adds stepup cutting passes (+Z) to the toolpath. Enter the stepup value to use between up cutting passes as either a percentage of tool diameter or an absolute distance.
Mastercam also inserts extra cut passes when stepping up to clear all detected flat areas. Stepup cutting passes help remove material left behind between the stepdowns, for example, islands or large scallops on angled walls, using a dynamic rest motion. Deselect to disable stepup cutting for the toolpath. The toolpath then uses dynamic milling motion to remove material only on stepdowns, avoiding any islands.
When you set the Stepup value equal to the Stepdown value, Mastercam calculates up cutting passes for only flat areas.
Mill vertical walls
Select to always calculate a rest area for stepup cuts. This results in a waterline cut motion on vertical walls. Deselect to machine only the actual rest area Mastercam calculates from the stepup cuts.
Minimum toolpath radius
Enter the minimum toolpath radius to create in the operation. Enter the value as a percentage of the tool diameter or an absolute value. Mastercam uses the specified minimum toolpath radius in combination with the Microlift distance and Back feed rate parameters to calculate 3D arc moves between cut passes. The Minimum toolpath radius value is beneficial when the following conditions are present:
- Sharp corners in your machining chain: If you machine a rectangular-shaped pocket, each of the four corners will have a radius. The Minimum toolpath radius is the radius of those corners.
- Arc on and off: The arc motion on and off during toolpathing tries to target 45% of the tool's diameter for its size. However, if the percentage prevents the tool from going into a tight space, Mastercam makes this value less than 45%, but never less than the Minimum toolpath radius value.
Micro lift distance
Enter the distance the tool lifts off of the part on back moves. Microlifts are slight lifts that help clear chips and minimize excessive tool heating.
Back feed rate
Controls the speed (inches per minute or millimeters per minute) of the tool's backfeed movement. This allows 3D arcs between cuts to have a different feed rate than the rest of the toolpath, which can help reduce cycle time.





