Creating Edge Fillets

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 Creating Variable Radius Fillets or Variable Radius Fillet Using a Spine.

This document deals with the following:

Open the Edge_Fillet1.CATPart document.
  1. Click Edge Fillet .
    The Edge Fillet Definition dialog box appears.

The icon now available after the Objects to fillet field lets you edit the list of the faces to be filleted. For more information about that capability, refer to Editing a List of Elements.

  1. Select the edge as shown.

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

  Clicking Preview previews the fillet to be created.
  1. Two propagation modes are available:

    • Minimal: edges tangent to selected edges can be taken into account to some extent. The application continues filleting beyond the selected edge whenever it cannot do otherwise. In our example below, the fillet is computed on the selected edge and on a portion of tangent edges:
    • Tangency: tangencies are taken into account so as to fillet the entire edge and possible tangent edges.
  2. For the purpose of our scenario, set Tangency.
    The preview clearly shows that the whole edge will be filleted.

    If you set the Tangency mode, the Trim ribbons option becomes available: you can then trim the fillets to be created. For more, refer to Trimming ribbons

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

  4. Select the eight vertical edges.

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

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

  7. Enter 5mm as the radius value.

  8. Click More to access four additional options.

To know how to use:

Limiting Elements

  1. 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.
    This capability is supported on Part Design P2 only.

    • It is possible to use one or more limiting elements.
    • Contextual commands creating the limiting elements you need are available from the Limiting elements field:
      • Create Point: For more information, see Creating Points
      • Create Midpoint: creates the midpoint of the line you select
      • Create Endpoint: creates the endpoint of the line you select
      • Create Plane: see Creating Planes
      • XY Plane: the XY plane of the current coordinate system origin (0,0,0) becomes the limiting element.
      • YZ Plane: the YZ plane of the current coordinate system origin (0,0,0) becomes the limiting element.
      • ZX Plane: the ZX plane of the current coordinate system origin (0,0,0) becomes the limiting element.
      • Create Intersection: Creating Intersections
      • Create Projection: see Creating Projections
      • Create Join: joins surfaces or curves. See Joining Surfaces or Curves.
      • Create Extrapol: extrapolates surface boundaries or curves. See Extrapolating Surfaces and Extrapolating Curves.

      If you create any of these elements, the application then displays the corresponding icon in front of the Limiting element(s) field. Clicking this icon enables you to edit the element.

    • You can create limiting elements just by clicking on the edge to be filleted. The application displays this element as a blue disk:

    • You can select points as limiting elements. These points must be located on the edge to be filleted and they must have been created using the On curve option available in the Point Definition dialog box.
    1. 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 select the Conic parameter check box. This check box allows you to vary the section of the fillet.
For a parameter comprised between or equal to:
  • 0.5, the resulting curve is a parabola.
  • 0 < parameter < 0.5, the resulting curve is an arc of an ellipse.
  • 0.5 < parameter < 1, the resulting curve is a hyperbola.
  • If the conic mode is activated, the Edge(s) to keep and the Parting element fields cannot be selected.
  • Conical fillets do not handle twist configurations. If a twist is detected, the fillet
    operation fails.
  • If the fillet surface curvature is lower than the support curvature, fillet surface
    relimitation may fail. In such cases, the conic parameter has to be decreased.

Interrupting Fillet Computations

In case you made a mistake when defining a fillet (wrong radius value for example), you can interrupt the feature computation launched after clicking OK, when the computation requires a few seconds to perform.
In concrete terms, if the computation exceeds a certain amount of time, a window appears providing a Cancel option. To interrupt the operation, just click that Cancel button. This interrupts the process and then displays an Update Diagnosis dialog box enabling you to edit, deactivate, isolate or even delete the feature.

This new capability is available for any types of fillet features you are creating or editing.

Keeping Edges

When filleting an edge, depending on the radius value you specified the fillet may affect other edges of the part that you do not want to fillet. In case you can anticipate such a result, before confirming the Fillet operation, specify the edges you want to exclude from the operation by filling in the Edges to keep field.

In the example below, the user selects the upper edge as the edge to keep. Once selected, this edge turns purple.

Edge to be filleted
The upper edge is selected as the edge to be kept
The upper edge is not filleted


Note: Selecting an edge as an edge to be kept can propagate the selection of edges to be filleted. Propagated edges are displayed in red dotted lines.

In the example below, both purple edges are selected as edges to be kept. The selection of the edge to be filleted (in red) then includes two additional edges

Selection of the edge to fillet and of two edges to be kept


If an Error Message is Issued...

In case you have specified no edges you want to exclude from the fillet operation, the application may sometimes detect that some edges cause trouble during the fillet computation. The application then issues an error message asking you if you wish to select the edges you do not want to fillet.

There are two ways of specifying the edges you want to keep:

  • By explicitly specifying these edges
    This means that you need to click Yes in the Feature Definition Error dialog box. Then you just need to click the Edit button from the Update Diagnosis dialog box that appears, click the Edges to keep field from the Edge Fillet dialog box and select the edge in the geometry. The application then displays the selected edge in pink meaning that the edge will not be affected by the fillet operation. The fillet is eventually computed and does not affect the "keep" edge.
  • By letting the application find a solution
    If you do not wish to explicitly select the edge you do not want to fillet, just click No in the Feature Definition Error dialog box. The application then tries to find a solution.

Both methods may not give the same result depending on the geometry. If you prefer to let the application find a solution, the application finds an appropriate physical edge in the geometry, then considers it as the edge to be kept. If no edge can be found, then it finds a solution by itself.

Ignoring Edges

When the update process detects that sharp edges (edges are considered as sharp when the angle between the two faces is greater than 0.5 deg) interrupt fillet operations, it is possible to continue filleting just by selecting an edge adjacent to the edge to be filleted. In the example below, the application displays the edge causing trouble in yellow:

An error message is issued, prompting you to select an edge adjacent to the filleted edge. Just by selecting both edges to the right and the left of the previewed fillet, the application can then compute the whole fillet properly:

Trimming Ribbons

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

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.