Patterns and Parameters

Patterns

• Standard Pocket - creates a pocket with the specified patten. Standard pockets do not support open pockets.
  
  
  • Parallel - creates a pattern of parallel cuts where the tool feeds in both directions. With this pattern, you can select either No Profile, Profile After, or Profile Before, from the Final Contour group.
    
    
    
    
  • Offset Pocket Out - creates a pocket pattern which continually offsets the inner shape of the pocket and creates the toolpath from the inside-out.
    
    
    
    
  • Offset Pocket In - creates a pocket pattern which continually offsets the outer shape of the pocket and creates the toolpath from the outside-in.
    
    

• Advanced Pocket - creates a pocket with the specified patten. Advanced pockets are able to support open pockets. See the Open Pocket Example for more information.
  
  
  • Parallel - creates a pattern of parallel cuts where the tool feeds in a single direction. With this pattern, you can select either No Profile, or Profile After, from the Final Contour group.
    
    
    
    
  • Offset Pocket Out - creates a pocket pattern which continually offsets the inner shape of the pocket and creates the toolpath from the inside-out.
    
    
    
    
  • Offset Pocket In - creates a pocket pattern which continually offsets the outer shape of the pocket and creates the toolpath from the outside-in. This option is different in that the first cut, which is against the wall of the pocket is skipped until the rest of the pocket is cleared out.
    
    

  Standard Pocket	Advanced Pocket

  
  

  • Morph Spiral - creates a pocket pattern which combines a spiral and the offset shape of the pocket in order to eliminate linking moves. A morph is only applied in situations creating a closed contour. Open pockets will not always be able to utilize the morph pattern.
    
    

  Standard Offset	Morph Spiral

  
  

  • Adaptive Roughing - creates a high-speed machining operation with automatic tool engagement settings. When this option is selected, the Minimal Curvature Radius is added to the Parameters group in this dialog box. In addition, the Link Clearance is added to the Finish group in the Parameters page of the wizard.
    
    
    

• Use Spiral for Circular Pockets - Spiral pockets give the user the ability to create spiral toolpath instead of the standard offset toolpath for circular pockets. This option is not available when using the Morph Spiral, or Adaptive Roughing patterns.
  
  Select the check box to a override the previously selected pattern in favor of a spiral pocketing method on circular pockets.
  
  While  the check box remains unselected, the currently selected pattern will be applied to all geometry, including circles.

   

  Offset	Spiral

   

Sharp Corner - This group becomes available when the Offset patterns are selected for Advanced Pockets.

 

Sharp Corner	Sharp Corner

• Open Convex Corners Only - applies the Sharp Corners only to the open areas of the pockets. This can be helpful to avoid roll overs which may interfere with nearby part walls which should not be contacted with the tool.
  
  
  
  
• All Convex Corners - applies Sharp Corners to all areas of the pocket, whether opened or closed.
  
  
  
  
  • Smooth Radius in % of Stepover - is the value for the amount of smoothing measured from the original contour and the rounded corner.
    

 

Cut Direction

These options are only available when Offset Pocket In or Offset Pocket Out is selected.

• One Way (Advanced Pocket)
  
  Select the check box to define a one-way machining for the Advanced Pocket. This enables the Climb Mill and Conventional Mill cutting options.
  
  
  • Climb Mill - the tool travels in a counter clockwise direction along the inside shapes of the model and travels in a clockwise direction along the outside edges of the model.
    
    
    
    
  • Conventional Mill- the tool travel in a clockwise direction along the outside edges of the model.
    
    
    
    

  Clear the check box to use an offset pocketing strategy.

   

  One Way	One Way

  
  

Rest Roughing

• Rest Roughing
  
  Rest Roughing- With this check box cleared, the pocket will be handled normally.
  
  Rest Roughing - When the Advanced Pocket pattern is selected, Rest Roughing calculates the toolpath to remove all the non-machined areas remaining from the previous roughing tool. It machines only those areas that are left behind by the (larger) previous tool. In Rest Roughing toolpaths you normally use a smaller step down (as the cutter size reduces) than the cutter used for the previous roughing toolpath.
  
  

  Rest Roughing	Rest Roughing

  
  

  • Use Previous Operation
    
    Select the check box to have the system automatically set the Rest Roughing parameters using the tool parameters of a roughing operation that is previous to this operation in the feature.
    
    
    
    Clear the check box to manually enter the tool parameters of the previous roughing operation.
    
    
    • Previous Tool Diameter - set this to the diameter of the previous tool used to rough the part. This value must be larger than the tool being used for the rest roughing operation.
      
      
      
      
    • Previous Tool Corner Radius - set this to the corner radius of the previous tool used to rough the part.
      
      
      
      
    • Previous Allowance XYZ - set this to the amount of side allowance used for the previous roughing operation.
      
      

Parameters

• Lace Angle - sets the angular direction of the toolpath from the X-axis of the machining origin when using the Parallel pattern.
  
  
  
  
• Stepover % - Sets the distance between passes as a percentage of the tool diameter. Updating this field automatically updates the absolute value.
  
  
  
  
• Stepover - Sets the distance between passes using an absolute value. Updating this field automatically updates the percentage.
  
  

Note: The following two parameters are only available when using the Advanced Pocket with Adaptive Roughing, without using the Oneway cut direction option.

• Max Stepover % (Climb) - sets the maximum stepover as a percentage of the tool for zigzag cutting. When Max Stepover % (Conventional) is selected, this is only applied to the climb milling portion of the toolpath.
  
  
  
  
• Max Stepover (Climb) - sets the maximum stepover as an absolute value for zigzag cutting. When Max Stepover % (Conventional) is selected, this is only applied to the climb milling portion of the toolpath.
  
  
• Max Stepover % (Conventional)
  
  
  
  Select the check box to specify that maximum stepover as a percentage of the tool for conventional milling.
  
  Clear the check box when not specifying the conventional stepover for conventional milling.
  
  
• Max Stepover (Conventional) - specifies a maximum stepover as an absolute value for conventional milling.
  
  

Note: The following parameter is only available when using the Advanced Pocket with Adaptive Roughing.

• 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.

The following parameter is only available when using the Advanced Pocket with Parallel, and without using the Oneway cut direction.

• Smooth Connections
  
  

Select the check box to apply a tangent move to the link connection. The specified radius can be anywhere from 0, to half the step over. Notice in the animation below, arcs of a specified size can be applied to the link move.

Clear the check box when not utilizing a smooth connection.

Note: The Smooth Connections option is only available when an Advanced Pocket / Parallel Pattern is used, and One Way Cut Direction is turned off.

Finish

• Side Allowance - sets the amount of material that remains on the walls for finishing. The material is removed on the finish pass.
  
  
  
  
• Bottom Allowance - sets the amount of material that remains on the floor for finishing. The material is removed on the finish pass.
  
  
  
  
• Link Clearance - When using the Advanced Pocket with Adaptive Roughing, the Link Clearance becomes available. This will allow you to set a height to the linking moves used in the adaptive moves.
  
  
  
  
• Retract Threshold (x Tool Diameter) - When using the Advanced Pocket with Adaptive Roughing, the Retract Threshold becomes available. This allows you to specify a maximum length link before a Rapid Retract for Large Gaps should be utilized.
  
  
  
  
• Break through amount - When using the Advanced Pocket with Adaptive Roughing, the Break through amount becomes available. This will dictate how far the pocketing moves will continue on an open pocket before coming back to clean up the edges.
  
  

Other

 

Advanced - launches the Roughing Advanced dialog. The content of this dialog will vary depending on the options used.

 

Roughing Advanced - dialog for Parallel, Offset Pocket Out, Offset Pocket in, and Morph Spiral patterns: 

Smoothing

 

• 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 % - With the Smooth Corners check box selected, the Smooth Distance/Setpover % sets the radius of the fillet as a percentage of the stepover distance.
    
    
• Smooth Contours
  
  - With the check box cleared, the Smooth Contours option is not used.
  
  - Select the check box to smooth the offset pattern based on the Deviation/Stepover % allowance, which becomes available when this option is selected.
  
  
  • Smooth Deviation/Stepover % - sets the allowable deviation from the original offset pattern.
    
    
• 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 an S-Link the connection is an S-type link.
  
  - Clear the check box to turn off Smooth Links.
  
  
  • Gap Size/Stepover % - With the Smooth Links check box selected, the Gap Size/Stepover % sets the distance over which the s-link moves are applied as a percentage of the stepover amount.
    
    
• Smooth Final Contour - This option becomes available when Smooth Corners is selected.
  
  
  
  - With the check box cleared, the Smooth Final Contour option is not used.
  
  - Select the check box to create fillets in the sharp corners of outer contours. The Smooth Distance/Stepover % parameter becomes available.
  
  
  • Smooth Distance/Stepover % - sets the radius of the fillet as a percentage of the stepover distance.
    
    
• Ignore Small Contour
  
  - Clear the check box to turn off Ignore Small Contour.
  
  - Select the check box to remove small pockets and segments which are not necessary to machine. The size of these segments must be defined as a percentage of the tool diameter. The Threshold Value in % of Tool Diameter parameter becomes available.
  
  
  • Threshold Value in % of Tool Diameter - sets the size of the small segments to remove as a percentage of the tool diameter.
    
    

 

 

Others

This group is available when the Cut Pattern on the Patterns page is set to Offset Out, Offset In, or Morph Spiral.

 

• Avoid Air Machining
  
  - With the check box cleared, the stepover will be continued over the entire part. This can result in cuts being made to areas which already have stock removed.
  
  - With the check box selected, toolpath will be terminated in areas which have already been cleared of stock.
  
  

  Avoid Air Machining	Avoid Air Machining

  
  
  
• Remove Corner Pegs
  
  
  
  - Clear the check box to turn off Remove Corner Pegs.
  
  - Select the check box to add extra tool movement in corners, removing the rest material; for use when a stepover greater than 50 percent results in small pegs of material remaining in the corners. With this check box selected, you will be able choose between the following three options.
  
  
  • Line-Arc-Line - removes the corner pegs with an arc between two lines as seen in the animation below.
    
    
    
    
    • Corner Peg Height in % of Tool Diameter - sets the size of the corner peg based on a percentage of the tool size in use.
      
      
  • Arc - removes the corner pegs with a single looping arc motion as seen in the animation below.
    
    
    
    
    • Corner Peg Height in % of Tool Diameter - sets the size of the corner peg based on a percentage of the tool size in use.
      
      
  • Line - removes the corner pegs by moving away from, and back to the toolpath with a straight line as seen in the image below.
    
    
    
    
    • Corner Peg Height in % of Tool Diameter - sets the size of the corner peg based on a percentage of the tool size in use.
      

 

Remove Small Regions/Contours

These options allow you to remove small pockets and segments which are not necessary to machine. The size of these segments must be defined as a percentage of the tool diameter. (Threshold Value in % of Tool Diameter)

 

• Filter by - These options allow you to determine the type of areas being considered for elimination. The Filter by options are only available when using the Offset Out, Offset In, and Morph Spiral cut pattern options.
  
  
  
  

  • Regions - A region can be defined as an area which can be handled without the need for a retract to clearance move. By selecting regions to filter, areas under the specified value will be ignored.
    
    

    
    
    
    
    
    
    
    

  Regions

   

  • Type - allows you to define how the size is defined. Choose between: 
    
    
    
    
    • Inscribed Circle - uses the width of the region as a maximum circle diameter, which could be inscribed into the toolpath within this region. With this type, any regions, or contours coming in contact with the boundary are eliminated from the toolpath.
      
      
      
      
    • Diagonal Length - uses the width of the region is a diagonal of the axis-aligned bounding box built around the toolpath within this region.
      
      
      
      
    • Circumscribed Circle - consolidates the diagonal length and inscribed circle types. With this type, any regions, or contours within, and not meeting or exceeding, the boundary are eliminated from the toolpath.
      
      
      

   

   

  • Contours - A contour can be defined as a single pass around a region before a link move is needed for the next pass. By selecting contours to filter, passes under the specified value will be eliminated.
    
    
    
    
    
    

  Contours

   

  • Type - allows you to define how the size is defined. Choose between: 
    
    
    
    
    • Inscribed Circle - uses the width of the region as a maximum circle diameter, which could be inscribed into the toolpath within this region. With this type, any regions, or contours coming in contact with the boundary are eliminated from the toolpath.
      
      
      
      
    • Diagonal Length - uses the width of the region is a diagonal of the axis-aligned bounding box built around the toolpath within this region.
      
      
      
      
    • Circumscribed Circle - consolidates the diagonal length and inscribed circle types. With this type, any regions, or contours within, and not meeting or exceeding, the boundary are eliminated from the toolpath.
      
      
      
      
    • Contour Length - filters out contours equal to or smaller than the threshold.
      
      
      
      
  • Contour Type - specifies the type of contours to filter.
    
    
    
    
    • Open and Closed - applied the filter to contours in open and closed areas.
      
      
      
      
    • Open - applied the filter to contours in open areas only.
      
      
      
      
    • Closed - applied the filter to contours in closed areas only.
      
      
      

   

   

  • Regions and Contours - A region can be defined as an area which can be handled without the need for a retract to clearance move. By selecting regions to filter, areas under the specified value will be ignored. A contour can be defined as a single pass around a region before a link move is needed for the next pass. By selecting contours to filter, passes under the specified value will be eliminated.
    
    
    
    
    
    

    Regions

     

    • Type - allows you to define how the size is defined. Choose between: 
      
      
      • Inscribed Circle - uses the width of the region as a maximum circle diameter, which could be inscribed into the toolpath within this region. With this type, any regions, or contours coming in contact with the boundary are eliminated from the toolpath.
        
        
        
        
      • Diagonal Length - uses the width of the region is a diagonal of the axis-aligned bounding box built around the toolpath within this region.
        
        
        
        
      • Circumscribed Circle - consolidates the diagonal length and inscribed circle types. With this type, any regions, or contours within, and not meeting or exceeding, the boundary are eliminated from the toolpath.
        
        
        

     

     

    Contours

     

    • Type - allows you to define how the size is defined. Choose between: 
      
      
      • Inscribed Circle - uses the width of the region as a maximum circle diameter, which could be inscribed into the toolpath within this region. With this type, any regions, or contours coming in contact with the boundary are eliminated from the toolpath.
        
        
        
        
      • Diagonal Length - uses the width of the region is a diagonal of the axis-aligned bounding box built around the toolpath within this region.
        
        
        
        
      • Circumscribed Circle - consolidates the diagonal length and inscribed circle types. With this type, any regions, or contours within, and not meeting or exceeding, the boundary are eliminated from the toolpath.
        
        
        
        
      • Contour Length - filters out contours equal to or smaller than the threshold.
        
        
        
        
    • Contour Type - specifies the type of contours to filter.
      
      
      • Open and Closed - applied the filter to contours in open and closed areas.
        
        
        
        
      • Open - applied the filter to contours in open areas only.
        
        
        
        
      • Closed - applied the filter to contours in closed areas only.
        
        
        

     

    
    

 

Tip: The images below show the results of the various combinations of filtering by type.

 

	Diagonal	Inscribed	Circumscribed
Value
Contour
Region

 

 

Roughing Advanced - dialog for Adaptive Roughing pattern: 

Stepover

 

• Dependent Desired Stepover - This feature lets you avoid the hard coded dependency between the maximum and desired stepovers in the adaptive roughing pattern. The desired stepover parameter can take any value which is less than the maximum one. The hard coded value is 1.25 x maximum stepover.
  
  - With this check box cleared, you can list a Desired Stepover, which must be lower than the previously specified (Maximum) Stepover.
  
  - With the check box selected, the Desired Stepover will be set so the specified (Maximum) Stepover will be 1.25 times greater.
  
  

  Dependent Desired Stepover	Dependent Desired Stepover

 

Thin Wall Processing

 

• Thin Wall Rollover
  
  - With this check box cleared, toolpath calculation will not attempt to optimize settings in cases where thin walls of material are created. In these cases, the toolpath will continue to loop away and come back to reengage.
  
  - With the check box selected, toolpath calculation attempts to optimize cutting where thin walls are created by continuing around the wall to engage from the other side. This helps to eliminate air cutting.
  

  Thin wall created during machining
  Thin Wall Rollover	Thin Wall Rollover

 

Region Processing

 

• Over Machine - Optimizes the milling conditions for hard metal milling to compensate for long tool deflections and cutting forces.
  
  
  
  - With this check box cleared, toolpath calculation will not attempt to optimize for tool deflections.
  
  
  
  - With the check box selected, toolpath calculation attempts to optimize cutting to avoid chatter caused by thin walls generated due to tool deflections.
  
  

  Over Machine	Over Machine

 

• Remove Stock Pillars
  
  - With this check box cleared, toolpath calculation can result in open areas ending in thin walled areas in the center which can create adverse cutting conditions.
  
  - With the check box selected, toolpath calculation optimizes to leave a wide pillar in the center which is then handled with a spiral ramp motion in order to create optimal cutting conditions and help extend tool life.
  

  Remove Stock Pillars	Remove Stock Pillars

 

Remove Small Regions/Contours

These options allow you to remove small pockets and segments which are not necessary to machine. The size of these segments must be defined as a percentage of the tool diameter. (Threshold Value in % of Tool Diameter)

 

• Type
  
  
  
  
  • Inscribed Circle - uses the width of the region as a maximum circle diameter, which could be inscribed into the toolpath within this region. With this type, any regions, or contours coming in contact with the boundary are eliminated from the toolpath.
    
    
    
    
  • Diagonal Length - uses the width of the region is a diagonal of the axis-aligned bounding box built around the toolpath within this region.
    
    
    

 

 

Depth

• Total Depth - displays the depth (set in the Feature settings) of the material removed by the feature.
  
  
  
  
• Depth of Cut - for the Multiple Steps option, this is the depth at which each equal pass is processed.  This value may be different than entered because the value of the Number of Cuts must be a whole number and the depth of each pass is the Total Depth divided by the Number of Cuts.
  
  
  
  
• Number of Cuts - for the Even Depth option, this value is calculated by the system using the Depth of Cut value.