Cut Parameters: Face
Use the Cut Parameters page to enter cutting parameters and compensation options for a Face toolpath. Follow this general outline:
- Choose a cutting method. Then set the tip compensation, and define how you want to roll the cutter around corners.
- Set an overlap distance for the edges of the stock. You can also add an approach/exit distance on the first and last passes.
- Define the maximum stepover amount. Then set the cutting direction.
- Choose the type of tool motion to use when transitioning between passes, and the feed rate you want to use.
Use options in the Depth cuts page to remove the stock in several layers.
| 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.
- One pass: Creates a single pass down the center of the stock.
- Dynamic: Cuts from the outside to the inside, maintaining a constant load on the tool with minimal entries and exits. With this method, Mastercam internally manages many of the additional cut parameters (they appear unavailable) and you can specify the general start location of the tool.
- For the One pass option, the tool diameter must be equal to or greater than the width of the part.
-
For Zigzag and One way cutting methods, Mastercam provides optional settings that reverse the direction of the final cutting pass for the toolpath. This strategy can prevent burring along the opposing edge of the face based on the selected cutting direction.
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.
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.
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.
Across overlap
Sets the amount that the tool overlaps the stock perpendicular to the roughing angle. Enter the across overlap as a percentage of the tool diameter or as an absolute distance. Unavailable if Cutting method is set to One pass.
Along overlap
Sets the amount that the tool overlaps the stock parallel to the roughing angle. Enter the along overlap as a percentage of the tool diameter or as an absolute distance. This value must be greater than or equal to the across overlap.
Approach distance
Adds an additional distance to the beginning of the first cut. Enter the distance as a percentage of the tool diameter or as an absolute distance. Use the drop-down to select the location of the approach.
Exit distance
Adds an additional distance to the end of the last cut. Enter the exit distance as a percentage of the tool diameter or as an absolute distance.
General start location
Select the start location from the drop-down list. The start location is an approximate area to begin the toolpath as it approaches the part in air.
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%.
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.
Reverse direction of last pass
Select this option if you want the last pass, which cuts along the opposing edge of the face, to reverse the cutting direction. This strategy can prevent burring or chipping on this edge, based on the selected cutting direction.
Even number of passes
Select this option to create an even number of passes.
Auto angle
Determines the roughing angle automatically. If the stock is larger in width than height, the roughing angle is 0 (zero) degrees. If the stock is larger in height, the roughing angle is 90 degrees.
Roughing angle
Sets the angle that the tool moves at during the roughing passes.
Move between cuts
Determines how the tool moves between each cut. Only available if Cutting method is set to Zigzag. Select one of the following options:
- High speed loops to create 180 degree arcs between each cut
- Linear to create lines between each cut
- Rapid to create rapid moves between each cut.
Feed rate between cuts
Allows lines or arcs between cuts to have a different feed rate than the rest of the toolpath. Only available if you select the High speed loops or Linearoptions for movement between cuts.
Roll in
Adds an arc move with the entered Radius or Tool percentage to the lead in move. This move is always opposite of the stepover direction. This option is particularly helpful with tool engagement, resulting in less tool stress.
| Roll in (Off) | Roll in (On) and Radius set to 0.5 |
|---|---|
|
|
When Style is set to One way, the arc is applied to each cut. When set to Zigzag, the arc is only applied to the first cut.





