Parameters

Introduction

This topic explains the Parameters page of the Advanced Planar operation found in the 3 Axis Wizard.

Parameters

Finish

Stepover

 

  • Standard - This option creates a standard stepover based on Stepover value.

    • Stepover - defines the distance between each pass in X and Y, or the XY plane.



  • Adaptive- The adaptive stepover is similar to the standard stepover, except that it creates additional passes in steep areas of the feature based on the defined Stepover and Minimum Stepover values. This creates a more consistent finish in steep areas by eliminating significant height changes from one pass to the next.

    • Stepover - defines the distance between each pass in X and Y, or the XY plane.

    • Minimum Stepover - determines the minimum distance between adjacent slices for the Adaptive Stepover  passes.



    •  Trim adaptive passes - when this option is selected, the Adaptive result is trimmed to the remove excessive cuts from areas they are not needed. Click on the images below to see each in action

      - Clear the check box to turn off the Trim adaptive passes.

      - Select the check box to turn on Trim adaptive passes. This localizes the adaptive cut to the areas in which it is required.

      Trim adaptive passes Trim adaptive passes

       

  • Perpendicular - This option creates opposing (perpendicular) passes when the height change between toolpath slices exceeds the specified threshold value. This helps provide a better finish for steep areas of the feature using the Stepover, Pass Extension, and Threshold Distance parameters.Stepover - defines the distance between each pass in X and Y, or the XY plane.

    •  Stepover - defines the distance between each pass in X and Y, or the XY plane.

    • Pass Extension - adds the specified distance to the perpendicular passes of the toolpath to help blend the transition between the perpendicular cutting directions.

    • Threshold Distance - determines the maximum allowable height change from one toolpath pass to the next before perpendicular passes are created.



 

 

  • Machining Tolerance - the amount of variation allowed for creating the toolpath for the feature. The accuracy of the toolpath does not exceed this range.

  • Cut Holes - extends the toolpath into any holes that may be present in the surface.

  • Ignore Holes - does not place the toolpath into any holes and treats the surface as if it is continuous and unbroken.

 

 

Depth Options

  • Top of Job

    - sets the highest Z location for toolpath as the top of stock.

    - allow you to specify the highest Z location for toolpath in this operation. Select the check box and type a value to define a plane for the top of job.

    • Pick - hides the Wizard to allow you to set the Top of Job by selecting geometry whose height, in relation to the machine setup, is at the desired value.

  • Bottom of Job

    - sets the lowest Z location for toolpath as the bottom of stock.

    - allows you to specify the lowest Z location for toolpath in this operation. Select the check box and type a value to define a plane for the bottom of job.

    • Pick - hides the Wizard to allow you to set the Top of Job by selecting geometry whose height, in relation to the machine setup, is at the desired value.

 

Note: The Bottom of Job and Top of Job values are in reference to the machining origin (Machine Setup coordinate) of the part.

 

  • Multiple Passes on Full Width Cut

    - Clear the check box to turn off Multiple Passes on Full Width Cut.

    - Select the check box to turn on Multiple Passes on Full Width Cut and the Depth Step parameter. This helps the operation to cut steep areas of the model better by adding more cuts when the depth between two passes is greater than the stepover amount.

    • Depth Step - determines the depth of cut for extra passes created using Multiple Passes on Full Width Cut.

 

  • Step Down

    - Clear the check box to turn off Multiple Passes on Full Width Cut.

    - Select the check box to turn on Multiple Passes on Full Width Cut and the Depth Step parameter. This helps the operation to cut steep areas of the model better by adding more cuts when the depth between two passes is greater than the stepover amount.

    • Number of Passes - sets the number of additional passes to create.

    • Depth Step - determines the spacing between the extra passes created.

    • Sort by

      • Slices - cuts all depths on one pass before moving to the next pass.

      • Passes - cuts the first depth on all passes before coming back to cut the second depth.

 

 

 

Allowance

The Allowance settings are used to define the rest material, or the amount of material remaining after this operation to be removed by the next operation, in one of two ways. These options offset the model geometry to calculate the toolpath. You can use positive or negative values to leave extra material or cut deeper than the model geometry, respectively.

 

Offset Type

The Offset Type determines if the allowance is 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 in the available allowance boxes.

 

  • Global - 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).

 

  • Advanced - opens the Allowances dialog to allow you to select surfaces to assign as either Part, or Fixture, geometry items. Each of those items can then have specific allowances set.

    - With this check box cleared, only the Offset Type and Allowance above will be used for the Feature Geometry.

    - With this check box selected, the geometry and allowances set in the (Advanced) Allowances dialog will be active.

 

 

Bounds

The Trim to Stock option provides the ability to pass the stock definition to the toolpath calculation, which trims the toolpath to remove air cutting. You can assign stock geometry (.stl or solid model) to the Operation Stock item in the CAM Tree, or if you do not assign operation stock, the software uses the stock definition from the Stock Wizard. This option can be used as a 3D boundary for the operation.

 

Important: In order to pass a stock definition to the toolpath calculation, you must turn on Trim to Stock in the wizard as explained next. If you assign Operation Stock, but do not turn on Trim to Stock, the stock isn't used in the toolpath calculation.

 

  • Trim to Stock

    - Clear the check box to create the operation without trimming the toolpath to the stock.

    - Select the check box when you want the software to trim the toolpath for the operation to the stock in one of two ways. You can (1) assign a solid model or .stl file using the Operation Stock item in the CAM Tree, or (2) if you don't assign operation stock, the software automatically uses the stock from the Stock Wizard to trim the toolpath. View Selecting Operation Stock.

    Trim to Stock

 

 

Tip: You can use simulation to save the stock model as an .stl file, which can then be used as Operation Stock. To learn more, view How to Save Simulation Stock as STL.