Multiaxis Machining

Pattern

• Machining - select from one of the following operations.
  
  
  • Roughing - Removes the bulk of the material with multiaxis moves.
    
    
  • Floor Finishing - Finishes the floor surfaces with multiaxis moves.
    
    
  • Wall Finishing - Finishing the wall surfaces with multiaxis moves.
    
    
• Pattern - select from one of the following strategies.
  
  
  • Offset From Floor - When using the Roughing, this option creates parallel cuts that are offset from the selected Floor Surface.
    
    
  • Offset From Ceiling - When using the Roughing, this option creates parallel cuts that are offset from the selected Ceiling Surface.
    
    
  • Morph Between Ceiling and Floor - When using the Roughing or Wall finishing, this option creates cuts that morph or blend between the Ceiling and Floor Surfaces.(The Ceiling Surface button becomes available on the Part Definition tab when this option is selected.)
    
    
  • Offset from wall - When using the Floor finishing, this option creates an offset of the wall to apply the finish to the floor.
    
    
• Type
  
  
  • Offset - When using the Roughing, this option creates a standard offset pattern from the selected geometry.
    
    
  • Adaptive - When using the Roughing, this option creates the feature using the Adaptive high-speed machining strategy. The constant tool engagement is automatically calculated for the feature.
    
    
• Guide curve - When using the Floor finishing with a Parallel pattern, this option becomes available.
  
  
  • Longest dimension - When using the Floor finishing option, this will identify and utilize the longest edge of the floor in order to create a parallel pattern from.
    
    
  • Floor curve - will utilize the edge of the floor in order to create a parallel pattern from.
    
    
  • Ceiling curve - When using the Wall finishing option, this will utilize the edge of the floor in order to create a parallel pattern from.
    
    
  • User defined drive - this option will allow you to select custom geometry to use as a guide curve.
    
    

Sorting

• Cutting Method
  
  

• Zigzag - creates a toolpath with an alternating cutting direction.
  
  

• One Way - creates a toolpath that only cuts in one direction. A retract and rapid move is created at the end of each toolpath slice.
  
  

• Direction For One Way Machining - when using the One Way cutting method, set the cutting direction to Climb or Conventional.
  
  

• Machine By - select one of the following options to define the machining order.
  
  

  • Levels - cuts the entire part to one depth before moving on to the next depth.
    
    

  • Regions - cuts each region of the part to the total depth before moving on to the next region.

Stepover

The parameters used to define the stepover change slightly depending on the selected pattern settings.

With Offset

• Maximum Stepover - is the not-to-exceed distance between each toolpath slice.
  
  

• Cusp Height - is used to define the stepover value using a cusp height instead of a distance when using a ball endmill.

With Adaptive and One Way

• Maximum Stepover - is the not-to-exceed distance between each toolpath slice.
  
  

• Desired Stepover - is the optimal stepover for the feature which is used as much as possible.

With Adaptive and Zig Zag

• Climb Stepover (% Stepover) - is the percentage of the Stepover value that is applied to climb cutting passes.
  
  

• Conventional Stepover (% Stepover) - is the percentage of the Stepover value that is applied to conventional cutting passes.

Depth Step

To define the depth steps of the feature, select one of the following two options.

• Constant Depth Step - determines the maximum amount of material removed for each pass. Type the positive value that you want to use for each depth step. The software automatically calculates the appropriate number of steps.
  
  

• Number of Slices - type a number of slices (or passes) to define the depth of cut for the feature. The software automatically calculates the depth steps value.
  
  

• Advanced - opens the Depth Step dialog box for you to further define the depth step with advanced options as follows.
  
  

• First Depth Step
  Select the check box to define a cutting depth for the first cut depth only. Type the value that you want to apply to the first depth step.
  Clear the check box when the first cut is the same as all other cuts.
  
  

• Final Depth Step
  Select the check box to define a cutting depth for the last cut depth only. Type the value that you want to apply to the last depth step.
  Clear the check box when the final cut is the same as all other cuts.
  
  

• Value
  Select the check box to type specific values at which the depth steps are created. When you select this option, a table displays for you to add values (Z-axis). Right-click anywhere in the table to access a shortcut menu for adding or removing items. After adding an item, set the desired value for it.
  Clear the check box to turn off the value depth step option.
  
  

• Intermediate Slices
  Select the check box to define intermediate slices using one of two options.
  Clear the check box when not using intermediate slices.
  
  

  • Constant Depth Step - automatically creates intermediate slices based on a value (depth) you define. Type the depth step value applied to create a stepped machining in any area with rest material.
    
    

  • Number of Slices - automatically creates intermediate slices based on a number of slices you define. Type the number of slices to use in the box to create stepped machining passes in area with rest material.

Area

After creating a roughing operation, you can create a second operation with Rest Roughing that uses a smaller tool than the first roughing operation. The system automatically finds and applies the toolpath only to the areas not machined by the previous tool.

• Rest Rough
  Select the check box to turn on the rest-roughing option. To open the Rest Roughing dialog box and define the parameters, click Rest Rough.
  Clear the check box to turn off rest roughing.
  
  
  • Roughing Tool Diameter - type the diameter of the previously used roughing tool.
  • Roughing Tool Corner Radius - type the corner radius of the previously used roughing tool.
  • Roughing Offset - type the offset value of the previously defined roughing operation.
    
    
• 3D Containment
  Select the check box to turn on 3D containment which allows you to assign a 3-dimensional curve to define the boundary for the operation. Click 3D Containment, select the geometry from wireframe or surface edges, and confirm the selection to return to the wizard. The resulting toolpath is contained within the boundary, but be aware that the current stock definition may cause cutting outside of (above) the boundary if there is stock to be removed.
  Clear the check box to turn off 3D Containment.
  
  
  
  
• Undercuts - dictates if undercutting is handled. Choose between: 
  
  
  • Do not machine - will prevent undercut areas from being handled in the toolpath.
    
    
    
    
  • Machine - will include undercut areas in the toolpath.
    
    
    
    
  • Machine only - will only handle the undercut area and exclude all other toolpath.
    
    
    
    
• Extend undercuts - allows you to define an extra area to be handled, beyond the undercut itself, when the Machine only option is used.

Machine only	Machine only with extension

Part Definition

• Floor Surfaces - click to enable selection mode and select the floor surface.
  
  

• Stock to Leave - is the amount of material that remains on the surface (for finishing).
  
  

• Wall Surfaces - click to enable selection mode and select the wall surfaces. This should be the entire part, but do not include a ceiling surface.
  
  

  • Stock to Leave - is the amount of material that remains on the surface (for finishing).
    
    

• Ceiling Surfaces - only used with the strategies (Surface Paths page): Offset From Ceiling and Morph Between Ceiling and Floor. Click to enable selection mode and select the ceiling surface.

Surface Quality

• Cut Tolerance - type a value to define how accurate the toolpath is in relation to the selected geometry. Smaller values create a more accurate toolpath but also increase calculation times.

   

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.

Smoothing

The following options display in the Smoothing group when the Type (Surface Paths tab) is set to Offset.

• Smooth Corners
  Select the check box to create fillets in the sharp corners of the toolpath. The fillet is not applied to the outer contour as it is with Smooth Final Contour. When selected, the Smooth Distance/Stepover % parameter becomes available as well as the Smooth Final Contour option.
  Clear the check box to turn off Smooth Corners.
  
  
  • Smooth Distance/Stepover % - sets the radius of the fillet as a percentage of the stepover distance.
    
    
• Smooth Links
  Select the check box to smooth the links within a group. The last segments of the previous contour and the first segments of the next contour are trimmed. The connecting link connects diagonally. In the case of a Blend Spline the connection is an S-type link.
  Clear the check box to turn off Smooth Links.
  
  
  • Smooth Link Gap Size - determines the distance over which the smooth s-links are applied to link two toolpath slices.
    
    
• Smooth Final Contour
  Select the check box to create fillets in the sharp corners of outer contours. The Smooth Distance/Stepover % parameter becomes available.
  Clear the check box to turn of Smooth Final Contour.
  
  
  • Smooth Distance/Stepover % - sets the radius of the fillet as a percentage of the stepover distance.
    
    

• Minimal Curvature Radius - determines the smallest radius used in the toolpath motion. This value must be greater than zero, but be aware that if you set this value too high, no toolpath is created. This parameter is useful, for example, to determine how far into a corner the toolpath can reach.
  
  
  
  

Note: The Minimal Curvature Radius option is the only one available in the Smoothing group when the Type (Surface Paths tab) is set to Adaptive.

Filtering

• Type - allows you to remove toolpath regions based on their size. If the width of a toolpath region is less than or equal to the specified threshold, this region will be filtered out. Choose between: 
  
  
  • Inscribed circle - the width of the region is a maximum circle diameter, which could be inscribed into the toolpath within this region.
    
    
  • Diagonal length - the width of the region is a diagonal of the axis-aligned bounding box built around the toolpath within this region.
    
    
• Threshold Value in % of Tool Diameter - sets the size of small toolpath segments to remove as a percentage of the tool diameter.

Approach Moves

• Ramp Type - sets the lead-in motion for the rough toolpath segments (for center cutting tool only). Several ramping strategies are available:
  
  
  • Automatic - automatically selects from the following ramp options: Line, Spiral, Zig Zag, and Profile are attempted in this order until a ramp entry that does not gouge is accomplished.
    
    
    • Max ramp length (tool diameter %) - sets the maximum length of a single ramp move. The value entered here is a percentage of the tool diameter being used.
      
      
    • Min ramp length (tool diameter %) - Selecting this check box allows you to specify a minimum length to use for the ramp. The vale entered here is a percentage of the tool diameter being used.
      
    
    
  • Line - the lead-in move is along an angular line, using the Ramp Angle value.
    
    
  • Helical - creates a helical or spiral entry into the stock material, the tool engages the stock with helical interpolation. The Ramp Length and Angle of Approach value define the helix.
    
    
    • Max ramp length (tool diameter %) - sets the maximum length of a single ramp move. The value entered here is a percentage of the tool diameter being used.
      
    • Min ramp length (tool diameter %) - Selecting this check box allows you to specify a minimum length to use for the ramp. The vale entered here is a percentage of the tool diameter being used.
      
    
    
  • Zig Zag - similar to line ramp, the length of the ramp is limited so you get zig and zag angular moves. The zag move is in opposite direction to the zig move and at the same angle to the horizontal. This uses the Angle of Approach and Ramp Length values. This option is only available when the Offset Pattern Type is selected in the Surface paths tab.
    
    
    • Max ramp length (tool diameter %) - sets the maximum length of a single ramp move. The value entered here is a percentage of the tool diameter being used.
      
    • Min ramp length (tool diameter %) - Selecting this check box allows you to specify a minimum length to use for the ramp. The vale entered here is a percentage of the tool diameter being used.
      
    
    
  • Profile - the tool engages the stock following the contour of the part or the toolpath profile. This option is only available when the Offset Pattern Type is selected in the Surface paths tab.
  
  

Note: All of the options work similar to the automatic ramp option, that is if that particular option fails, the other ramp options are attempted. IF no ramp strategy is possible in that given area, then a plunge move is applied.

• Ramp angle - defines the angle at which the tool enters the next slice or pass.
  
  
• Allow Tool Outside Stock
  Select the check box to allow the tool to travel outside of the defined stock geometry. For example, when the defined stock is the same as the part geometry.
  Clear the check box to turn off Allow Tool Outside Stock.
  
  
• Stock clearance (stepover %) - defines the start point of the ramp with this value as a minimum distance away from the stock. The value is used from a percentage of the stepover value.

Adaptive Links

The following options display in the Roughing tab when the Adaptive pattern type is selected on the Surface Paths tab.

• Link Clearance - is the clearance height applied to create a retract move to link non-connected cuts when using the Adaptive cut pattern (Type). This value can be set to zero to remove the link clearance from the toolpath. The value can't be greater than the depth of cut and when using Intermediate slices, the value can't be greater than the depth of cut divided by one plus the number of intermediate slices. [0 <= Link Clearance < Depth of Cut / (1 + Number of Intermediate Slices)]

Tip: The Maximum Cutting Feedrate (in Current Settings) is applied to the adaptive link moves between cuts.

• Link Length Threshold (X Tool Diameter) - allows you to define the maximum length of the (adaptive) link moves before applying a standard retract move in its place. Link moves less than this value use the Link Clearance value and link moves greater than this value are replaced with a retract to clearance. The value is specified as a multiple of the tool diameter, for example, 2 is twice the tool diameter.
  
  
• Arc Leads - with this check box cleared, linear leads will be used.
   Arc Leads - with this check box selected, vertical tangential arc moves will be used as default lead-in/outs. The radii of generated lead arc segments are determined by the specified entry/exit feed distances.

Feed Rate Control

• Feed control zone
  Select the check box to turn on the feed control zone option which allows you to specify a geometric boundary as an area to apply a special feedrate. To define the parameters in the Feed Control Zone dialog box, after selecting the check box, click .
  Clear the check box to turn off the option.

Feed Control Zone Dialog Box

• Geometry - click to select geometry as the boundary area for feedrate control.
  
  

• Offset - type a positive value here to offset the boundary area from the selected geometry thus making the feed control zone smaller.
  
  

• Inside feedrate % - type a percentage of the feedrate that is applied inside of the feed control zone.
  
  

• Outside feedrate - type a percentage of the feedrate that is applied outside of the feed control zone.
  
  

• Use rapid feedrate
  Select the check box to use rapid feedrate and type the desired rapid feedrate value in the box.
  Clear the check box to turn off rapid feedrate. Retract moves, for example, now use the standard feedrate.

Feedrate for Direct/Spline Links

• Area Links
  Select the check box to define a feedrate value used for direct or spline links.
  Clear the check box to use the program feed rates.
  
  

• Links Between Slice
  Select the check box to define a feedrate value used for direct or spline links.
  Clear the check box to use the program feed rates.
  
  

• Links Between Regions
  Select the check box to define a feedrate value used for direct or spline links.
  Clear the check box to use the program feed rates.

Miscellaneous

Max. Angle Step for Rotation Axis

This option determines the maximum angle step, or amount or rotation, applied to rotation axis movements. Select the check box to turn on the option and then type the angle value in the box.