Creating Edge Fillets

Edge fillets are smooth transitional surfaces between two adjacent faces. You can fillet several edges.

First you will fillet nine edges, then you will fillet a face and trim this fillet to a plane.

The cases illustrated here are simple. They use a constant radius: the same radius value is applied to the entire edges.

Before you begin:

To perform this task, create a pocket using an oblong as the profile, in a pad.

  1. Click Edge Fillet .

    The Edge Fillet Definition dialog box appears.

  2. Select the edge as shown.



    The edge selected then appears in the Objects to fillet box. The application displays the radius value.

    Tip: The icon available after the Objects to fillet box lets you edit the list of the faces to be filleted.

  3. For the purpose of our scenario, set Tangency.

    The preview clearly shows that the whole edge will be filleted.



  4. Enter 15mm as the new radius value. The radius value is updated in the geometry area.

  5. Select the eight vertical edges.



  6. Click OK.

    The edges are filleted. The creation of this fillet is indicated in the specification tree.



  7. Click Edge Fillet again and select the upper face as the new element to be filleted.

  8. Enter 5mm as the radius value.

  9. Click More>> to access four additional options in Part Design.



  10. Click the Limiting element box and select Plane.1 as the plane that will intersect the fillet.

    An arrow appears on the plane to indicate the portion of material that will be kept. Clicking this arrow reverses the direction and therefore indicates that the portion of material that will be kept will be the opposite one.



  11. Click OK.

    The second fillet is trimmed to Plane.1. Both fillets are displayed in the specification tree. The final 3D shape looks like this: