Reducing the Fillet Radius

This task explains how to modify the radius of fillets found with the Search Fillets command.

The Search Fillets command and the Fillet Radius Reduction command are two steps of one tool that helps you find fillets and reconstruct them to reduce the processing time on large models.
However, not all cases are detected nor can be reconstructed.

  • Faces in the NoShow are not dealt with.
  • Fillets with variable radius are not dealt with.
  • Faces smaller that 0.1 mm are not dealt with.
  • Once you have clearly identified strip of fillets to process, we recommend that you join those fillets.
  • We recommend that you use the Target radius option.
  • The result of the reconstruction depends directly of the quality of the faces to process.
  • You recommend that you perform a fillet search, although it is not mandatory.
  • Only rarely can all the surfaces retrieved with the Search Fillets command be used directly to recreate fillets.
    Be sure that you process areas with consistent fillets.
  1. Click Fillet Radius Reduction  in the Modify Fillet Radius toolbar.
    The Fillet Radius Reduction dialog box is displayed.

  2. Specify the curvature radius value to be reached:
    • Select Target radius (recommended option) and enter the value to be reached
    • or select Decrease value and enter an absolute value by which the current value of each fillet will be decreased.
    • or select Decrease percentage and enter the percentage of reduction of the current fillet.

  1. If necessary, display the User Selection Filter toolbar (View>Toolbars>User Selection Filter).
    Click to select surfaces or to select faces.

  2. Select the fillet to reduce, either by selecting surfaces or faces or a Geometrical Set.
    Multi-selection is available.

  3. Create in proposes you a Geometrical Set in which the output surfaces will be created.
    You can edit its name and change its color (double-click the color patch to start the color editor).
    If the Geometrical Set does not yet exist, it will be created.

  4. Click Apply to compute and display the new surfaces in the 3D viewer and in the specification tree.
    In feature mode, the specification tree will look like this:

    In datum mode it will look like this:

    The feature mode is useful when you need to modify the model.
    However, if the quantity of data is an issue, you can work in datum mode, to avoid creating too many data.