How-to
      Back to home
      1. Knowledge base
      2. PowerMill
      3. How-to

      How to optimize settings to remove facets inside PowerMill

      What settings can be changed to eliminate facets in a surface finish? What settings would work best for you to get a smooth finish?

      Issue

      Facets or steps can appear on the surface finish if using some default settings. They can also be caused when a machine tool cannot support contour control or high-speed options.
       

      Answer

      Show the toolpath Points

      1. Activate the finishing toolpath

      2. Go to the Toolpath tab > Draw group > Points

      If the facets on the finished surface match the points in PowerMill, you can tighten up the tolerance and/or the Point distribution for a cleaner result.

       

      Modify the toolpath tolerance

      1. Right-click on the finishing toolpath and click on Settings

      2. Recycle the toolpath to allow you to make modifications

      3. Set your toolpath tolerance between 0.0002 and 0.001 for an accurate finish

      4. Calculate the toolpath and write the NC code again

      Note - The toolpath tolerance controls the accuracy of the toolpath will follow the model. A highly-accurate toolpath will have a tolerance between 0.0002" and 0.001". A typical finishing toolpath should be about 0.0005" for a good finish.

       

      Modify point distribution settings

      Note - Once point distribution settings are confirmed for a specific surface finish, it can easily be repeated with a macro or saved toolpath strategy. Below is the process of finding these settings. 

      1. Right-click on the finishing toolpath and click on Settings

      2. Recycle the toolpath to allow you to make modifications

      3. In the settings tree, Click Point distribution

      4. Select Output type Redistribute

      5. Turn on the Point separation distance

      6. Set a small value to the Maximum distance - this will add a control point to whatever value you enter. This needs to be tested to optimize what finish you're looking for. Something between 0.005" and 0.05" should work well.

      7. Calculate the toolpath and write the NC code again - if you still see facets at the machine, follow steps 1 - 3 and then continue

      8. Set the Tolerance factor to half of its current setting

      9. Set a smaller value to the Maximum Distance

      10. Turn on Limit maximum triangle length

      11. Set the maximum triangle length to half its current value

      12. Calculate the toolpath and write the NC code again - if you still see facets at the machine, follow steps 1 - 3 and then continue

      13. Continue to reduce the above values until you get the result you need