Surface Paths

Pattern

The options that are available in the Pattern group change based on the selected Multiaxis operation type. The options that are common to most operations are listed here. For the options that are specific to each feature type, view the help topics for each operation type that are listed in the Multiaxis Wizard help topic.

• Drive Surfaces - enables selection mode for you to select geometry upon which the toolpath is created.
  
  
• Drive Surfaces Offset - creates a 3D offset of the drive surface geometry. This is used to leave stock remaining on the part.

Area

• Type - defines how the toolpath is applied to the part. The following settings apply to how the toolpath is handled at the part edges and allows you to limit the toolpath area on the part.
  
  
  • Full, avoid cuts at exact edges - does not allow the center of the tool to cut at the exact surface edge.
    
    
  • Full, start and end at exact surface edges - allows the center of the tool to cut at the exact surface edge.
    
    
    • Margins - defines the margin used at surface edges.
      
      
  • Determined by number of cuts - limits the toolpath by a specified number of cuts.
    
    
    • Margins - define the margin used at surface edges.
      
      
  • Limit cuts by one or two points - limits the toolpath to an area between two specified points.
    
    
    • Set points - defines the points between which the toolpath is created.

Note: For all of the following options, you must select the check box to turn on the option, and then click the option to access its parameters. Click the links to view explanations.

• Round Corners - provides an additional radius value used for creating round corners.
  
  
• Extend/Trim - is used to extend or trim toolpaths based on the defined values.
  
  
• Angle Range - is used to limit toolpath creation between specified angles of a specific plane.
  
  
• 2D Containment - is used to project a 2D curve in which the toolpath is contained.

Sorting

• Flip Step Over
  
  Select the check box to swap the cutting order. If the toolpath was from left to right, it changes to right to left.
  Clear the check box to retain the original cutting order.
  
  
• Cutting method - controls the cutting method or the toolpath pattern. Select either: Zigzag, One Way, Spiral.
  
  
  • Advanced - (for Spiral only) opens the Advanced Options for Spiral Machiningdialog box.
    
    
• Cut Order - controls how the selected cutting method is applied: Standard, From center away, From outside to center.
  
  
• Direction for One Way Machining - controls how the tool cuts into the material: Counterclockwise (CCW for Closed Cuts), Clockwise (CW for Closed Cuts), Climb,Conventional, Direction One, or Direction Two. The available options change slightly depending on the selected cutting method.
  
  
• Enforce Cutting Direction (Assume Closed Contours)
  
  Select the check box to use open contours and create a toolpath as if the geometry is closed.
  Clear the check box when creating toolpaths with open contours.
  
  
• Start Point
  
  Select the check box when specifying a toolpath starting point. Click Start Point to open the Start Point Parameters dialog box.
  Clear the check box when not specifying a toolpath starting point.
  
  
• Machine By - controls how toolpaths are handled for multiple surfaces or adjacent areas in one of two ways.
  
  
  • Lanes - the toolpath is created by lanes across multiple surfaces or adjacent areas by treating them as one surface or area.
    
    
  • Regions - the toolpath is created per section (region) for multiple surfaces or adjacent areas.

Tip: The available options change depending on the selections made.

Surface Quality

• Cut tolerance - determines how accurate the toolpath must be in relation to the selected geometry.

Tip: You can reduce the cut tolerance value, for example from 0.0005 to 0.005, to speed up the toolpath calculation while creating and modifying your toolpath. Once your are happy with the result, you can then set it back to the original tolerance to calculate the toolpath before posting the output.

• Maximum distance - controls the greatest distance between toolpath points.
  
  
• Surface edge handling - controls merging of toolpath segments and also how outside corners are handled.
  
  
• Advanced - provides control over the accuracy of toolpaths.

Stepover

Stepover - is defined in one of the two following ways.

• Maximum stepover - controls the maximum distance between toolpath cuts.
  
  
• Cusp height - when using ball end mills you can specify a cusp height to control the stepover.