Cut Pattern: Unified
Use the Cut Pattern page to establish the cut pattern parameters for your Unified Multiaxis toolpath. Cut pattern settings determine the geometry your tool follows and how it travels along that geometry.
Pattern table
This table lists instances of the drive pattern you selected. It contains the following columns:
- Name: Displays the chosen pattern. All entries in the table must be instances of the same pattern.
- Style: Contains a drop-down menu holding options to use with the drive pattern.
- Entities: Displays the number of entities in the geometry selected for the pattern.
- Action: Contains a button for deleting the selected pattern instance. To delete all pattern instances, click the Remove all rows button located below the table.
Add Automatic row
Adds an instance of the Automatic pattern to the table. You can further manipulate the item in the pattern table.
Add Curve row
Adds an instance of the Curve pattern to the table. You can further manipulate the item in the pattern table.
Add Surface row
Adds an instance of the Surface pattern to the table. You can further manipulate the item in the pattern table.
Add Plane row
Adds an instance of the Plane pattern to the table. You can further manipulate the item in the pattern table.
Remove all rows
Removes all pattern instances from the Pattern table.
Select
Returns you to the graphics window to choose geometry for the selected pattern instance.
Clear selection
Removes the selected entities from a pattern instance.
Select machining geometries
Returns you to the graphics window to select the geometry on which to create the toolpath. The number of selected entities appears in parentheses before the button.
Clear machining geometries selection
Removes all machining geometries from the Machining geometries option.
Machining geometries offset
Specifies the offset between the machining geometries and the toolpath.
Type
Select the method for cutting the toolpath area from the drop-down list. The type selected determines where the tool starts, ends, and area cut. Your choices are as follows:
- Full, avoid cuts at exact edges: Mastercam generates the toolpath on the entire drive surface, avoiding the surface edge.
-
Full, start and end at exact surface edges: Mastercam generates the toolpath on the whole surface, and starts and ends at the exact surface edge or the nearest possible position.
- Limit cuts by one or two points: This option allows you to limit the machining between two points on the drive surface. This limitation allows you to work only on certain parts of the surface.
Round corners
Activates the Round Corners page of the tree structure. Use to add fillets to the operation for internal corners of your part.
Extend / Trim
Activates the Extend / Trim page of the tree structure. Use to add or remove cutting motion when the tool gets to the end of a surface.
Containment
Activates Containment and the Containment page of the tree structure. Click Select to select a chain to control the cutting area of the part.
Angle range
Activates the Angle Range page of the tree structure. Use to set the cutting motion by entering two angles.
Start type
- Start on guide: Keeps the cuts on the drive curve.
- Shift to guide: Adds an extra margin at each guide curve or morph curve. The extra margin is half the given stepover.
Step direction
Determines which side is used as the step direction.
- Left: The inside is machined.
- Right: The outside is machined.
Flip step over
Reverses the cutting direction for the operation.
Start point
Activates the Start Point Parameters page of the tree structure. Use to set the tool's initial contact point with the part.
Cutting method
Select the cutting method from the drop-down list. Not all of these options are available for all toolpath types.
- One way: The tool cuts each pass in the same direction.
- Zigzag: The tool cuts each pass in the opposite direction from the previous one.
- Spiral: The tool cuts in a spiral motion on the part.
- Clockwise: The tool cuts in a clockwise direction.
- Counterclockwise : The tool cuts in a counterclockwise direction.
Cut order
Select the cut order from the drop-down list. Not all of these options are available for all toolpath types.
- Standard: The default option which usually cuts from one side of the part to the other.
- From center away: Cuts from the approximate center of the part to the outer edges.
- From outside to center: Cuts from the outer edges of the part to the approximate center.
- From top to bottom: Cuts from the top of the part to the bottom of the part.
- From bottom to top: Cuts from the bottom of the part to the top of the part.
Direction for closed cuts/Direction for one way machining
Specifies the direction of closed cuts.
- Direction one: For open curves, this is the original curve direction. For closed curves, Mastercam uses the counter-clockwise direction.
- Direction two: For closed curves, Mastercam detects the machining direction.
- Follow curve chaining: Mastercam uses the direction of the first drive curves to define the machining direction.
- Follow curve chaining reverse: Mastercam uses the reverse direction of the first drive curve to define the machining direction.
Use machining direction as reference for direction of cuts
Used mainly for closed containment curves, when the option is active, the negative machining direction is also considered, not only the positive machining directions. When it is not active, only the surface normals direction of the geometry are considered. If the machining direction and surface normals are in the same direction (both positive or both negative), activating the option will make no difference.
Machine by
Select an option from the drop-down list. Note that not all options are available for all toolpaths.
- Depth: Cuts the part by its depth.
- Levels: Cuts the part by alternating between pockets for each level.
- Lanes: Cuts the part with the selected pattern.
- Regions: Splits the toolpath into regions when the tool encounters a gap. Use when the part geometry creates excessive air motion around gaps.
Cut tolerance
Determines the accuracy of the toolpath. A smaller cut tolerance value creates a more accurate toolpath, but may take longer to generate the toolpath and create a longer NC program.
Damp
Allows a more flexible application of the axial shift.
Maximum stepover
Enter a value for the maximum distance between cutting passes.
Constant stepover
Enter a value for the constant distance between cutting passes.
Scallop height
Specifies the height of the remaining material between passes when using a rounded tool. Mastercam calculates the stepover based on the value that you enter here and the selected tool. The Maximum stepover and Scallop height fields are linked so that when you type a value in one field, Mastercam automatically updates the other.





