Edge Fillet

A fillet is a curved face of a constant or variable radius that is tangent to, and that joins, two surfaces. Together, these three surfaces form either an inside corner or an outside corner.

In drafting terminology, the curved surface of an outside corner is generally called a round and that of an inside corner is normally referred to as a fillet.

Edge fillets are smooth transitional surfaces between two adjacent faces.

The purpose of this task is to 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. To see more complex fillets, refer to Variable Radius Fillet or Variable Radius Fillet Using a Spine.

Open the Edge_Fillet1.CATPart document.
1.  Click the Edge Fillet icon .

The Edge Fillet Definition dialog box appears.


2.  Select the edge as shown.

  3.  The edge selected then appears in the Objects to fillet field. CATIA displays the radius value.
Clicking Preview previews the fillet to be created. This capability is supported on Part Design P2 only.


Two propagation modes are available:
Minimal: CATIA does not take any tangencies into account. The fillet will be computed only on a portion of the edge as shown below:

Tangency: tangencies are taken into account so as to fillet the entire edge and possible tangent edges.
  5.  For the purpose of our scenario, set the Tangency option. The preview clearly shows that the whole edge will be filleted.

  If you set the Tangency mode, the option "Trim ribbons" becomes available: you can then trim the fillets to be created. For more, refer to Trimming ribbons
  6.  Enter 15mm as the new radius value. The radius value is updated in the geometry area.
  7.  Select the eight vertical edges.



Click OK.

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


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


Enter 5mm as the radius value.


Click More to access four additional options.

To know how to use:
the Edges to keep option, refer to Keeping Edges.
the Blend corner(s) option, refer to Reshaping Corners.


Limiting Elements


Click the Limiting element field 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.

It is now possible to use one or more limiting elements.


This capability is supported on Part Design P2 only.


Click OK.

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


You can now create limiting elements just by clicking on the edge to be filleted. 

The application displays this element as a blue disk:

Keeping Edges


When filleting an edge, the fillet may sometimes affect other edges of the part, depending on the radius value you specified. In this case, the application detects these edges and stops the fillet to these edges, as illustrated in the example below:



Edge to be filleted

The upper edge is not filleted

When it comes to round corner fillets, you need to explicitly indicate the edges that should not be filleted. To do so, click the Edges to keep field from the dialog box and select the edge in the geometry. CATIA then displays the selected edge in pink meaning that the edge will not be affected by the fillet operation.

Trimming Ribbons


If you choose to use the Tangency propagation mode, you can also trim overlapping  fillets. To do so, simply check the option "Trim ribbons".


Selected edges


Overlapping fillets are not trimmed


Both fillets are trimmed



Compare the above results to the fillets created with the Minimal propagation mode: The fillets are only trimmed.


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