Options

Rest Roughing

Calculates the toolpath to remove all the non-machined areas remaining from the previous roughing tool. The previous tool is used to identify accurately the areas on a 3D component by sweeping the diameter across the whole part being machined. In this way any non-machined areas are identified and passed to the system and the toolpath is calculated. The Rest Roughing toolpath does not require the whole part to be machined again. It machines only those areas that are left behind by the previous tool. On intricate parts, multiple rest rough toolpaths are required to remove as much material as possible before running semi finishing or finishing toolpaths. 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. The following is an example of using the Advanced Rough feature for rest machining, along with an image showing the rest roughing strategy in blue.

- With this check box cleared, Rest Roughing will not be used.

- With this check box selected, Rest Roughing will be used, and the following options will become available to allow you to specify how the rest roughing is to be handled.

Note: The Use Previous Operation check box doesn't display unless you have another operation previous to the current operation in the feature.

• Use Previous Operation
  
  - Clear the check box to manually enter the tool parameters of the previous roughing 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.
  
  
  • 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 Offset Type - The Offset Type determines if the allowance from the previous operation was applied to the entire model or separately for the bottom and sides of the part. Select one of the following options and then type the allowance value used in the available allowance boxes.
    
    
    • Global - calculates the toolpath applies a single allowance value to the entire model using the Allowance XYZ value.
      
      
      • Allowance XYZ - is the amount of material left on the entire model (XYZ).
        
        
    • Side and Bottom - allows you to specify separate allowances for the side (XY) and bottom (Z) of the part.
      
      
      • Side Allowance - is the amount of material left on the sides of the part (XY).
        
        
      • Bottom Allowance - is the amount of material left on the bottom of the part (Z).
        
        
  • Detect stock thicker than - allows you to focus the toolpath on stock consisting of a particular range of thickness. Setting a value here will force the toolpath to ignore any stock whose thickness does not meet or exceed this value.

Machine Flatlands

Flatlands is designed to finish flat areas of a part, and it is best suited for machining large flat areas at multiple Z-levels.

- Clear this check box to not allow flatland machining.

- Select this check box to allow flatland detection which creates an optimized finishing toolpath for flat areas.

• Min. Width of Flatlands - sets the minimum width of flat areas that are included in the flatlands machining.
  
  
• Max. Width of Flatlands - sets the maximum width of flat areas that are included in the flatlands machining.
  
  - Clear the check box to only set a minimum width of flat areas that are included.
  
  - Select the check box to set a maximum width of flat areas that are included.
  

Important: The Flatlands feature must use flat-end mills or bullnose mills.

Flatlands	Flatlands

Boundary Options

Boundaries are used to contain the toolpath of the operation to stay within the specified area. The Boundary Options determine where the tool cuts when it reaches the boundary in one of three ways.

• Center of Tool - forces the center of the tool to cut directly on the specified boundary.

• Tool Inside - forces the entire tool to stay inside of the boundary. (This offsets the toolpath to the inside of the boundary by the tool radius.)

• Offset - is used to add an additional offset to the location of the tool at the boundary when using Tool Inside or Tool Outside. When using Tool Inside, the tool stays inside of the boundary by the specified distance. When using Tool Outside, the tool goes outside of the boundary by the specified distance. Note that positive or negative values are supported.

• Tool Outside - forces the entire tool to go outside of the boundary. (This offsets the toolpath to the outside of the boundary by the tool radius.)

• Offset - is used to add an additional offset to the location of the tool at the boundary when using Tool Inside or Tool Outside. When using Tool Inside, the tool stays inside of the boundary by the specified distance. When using Tool Outside, the tool goes outside of the boundary by the specified distance. Note that positive or negative values are supported.

Other

• Smoothing - Clicking on the Smoothing button will launch the Smoothing dialog box. The Smoothing dialog box will give access to some, or all, of the following options, depending on the pattern chosen.
  
  
  • 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 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
    
    - 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.
      
      
  • 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.
    
    

Processing

Break through amount

When using the Advanced Rough 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.

 

Less	More