Face-Face Fillet

The Face - Face Fillet command can be used when there is no intersection between the faces or when there are more than two sharp edges between the faces.

Open the Face_Face_Fillet.CATPart document.

Click the Face-Face Fillet icon .
The Face-Face Fillet Definition dialog box is displayed. Default options let you define a Smooth Extremity.
Select the faces to be filleted. When you select the two faces, a warning is displayed as shown below. Click Yes to continue.
Enter a radius value of 60 mm in the Radius field. Then click OK. Note that the fillet has been automatically propagated to the internal walls of the shell.

	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.
	Conical fillets do not handle twist configurations. If a twist is detected, the fillet operation fails. Conical fillets may produce internal sharp edges due to a curvature discontinuity of the fillet supports. Healing is used to smooth these sharp edges. 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.
	Face-Face Fillet Dialog Box In this dialog box you can define face-face fillets using the following options: Limiting Element `Limiting element` lets you define a trimming element. Once you have selected that element, an arrow appears on it to indicate the portion of material that will be kept. If you wish to keep the opposite portion of material, just click this arrow to reverse the direction. You can select the 2Doutput Sketches, 2Doutput Profiles and 2Dlayout Profiles as limiting element. Contextual commands creating the limiting elements you need are available from the `Limiting element` field: `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 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` field. Clicking this icon enables you to edit the element. Hold Curve Instead of entering a radius value, you can use a "hold curve" to compute the fillet. Depending on the curve's shape, the fillet's radius value is then more or less variable. The curve must be sketched on one of the selected faces. The Generative Shape Design product license is required to access this capability. Contextual commands creating the curves you need are available from the `Hold` `Curve` field: `Create Line`: For more information, see Creating Lines `Create Join`: joins surfaces or curves. See Joining Surfaces or Curves. `Create Boundary`: see Creating Boundary Curves. `Create Extract`: see Extracting Geometry. `Create Intersection`: see Creating Intersections. `Create Projection`: see Creating Projections. If you create any of these elements, the application then displays the corresponding icon in front of the `Hold Curve` field. Clicking this icon enables you to edit the element. Spine The `Spine` capability provides a better control of the fillet. The spine you select can be a wireframe element or a Sketcher element. To compute the fillet, the application uses circles contained in planes normal to the spine. It is then possible to control the shape of the fillet. Contextual commands creating the spines you need are available from the `Spine` field: `Create Line`: For more information, see Creating Lines `Create Join`: joins surfaces or curves. See Joining Surfaces or Curves. `Create Boundary`: see Creating Boundary Curves. `Create Extract`: see Extracting Geometry. `X Axis:` the X axis of the current coordinate system origin (0,0,0) becomes the direction. `Y Axis:` the Y axis of the current coordinate system origin (0,0,0) becomes the direction. `Z Axis:` the Z axis of the current coordinate system origin (0,0,0) becomes the direction. If you create any of these elements, the application then displays the corresponding icon in front of the `Spine` field. Clicking this icon enables you to edit the element. Edge(s) to keep You can specify the edge(s) of support body to be kept and create Fillet Surfaces with Hold Curve and Keep Edge as support wherever necessary. This helps in two different situations: Initializing the fillet ribbon when no portion of ribbon track lies within the limits of the provided support face. Computing the fillet surface(s) with keep edges as supports, whenever the default fillet ribbon track crosses the edge(s) to be kept. `Edge(s) to keep` field is defined in the `Face-Face Fillet Definition` dialog box which is not selectable by default. If a hold curve is selected, the `Edge(s) to kee`p field becomes selectable. As soon as an edge to be kept is selected, it turns purple.
	It is possible to perform Thickness, Shell, Boolean operations on the resulting fillet surface. It is possible to specify limiting element. Keep Edges of type “Round Corner” is not supported. The Keep edges should be specified explicitly. The fillet ribbon has zero radius at the points where the Keep edge(s) intersects the Hold Curve. There can be maximum two such points in a fillet ribbon i.e. one at each end of the fillet ribbon. Fillet operation may fail in cases where keep edge intersects the support face of Hold Curve. Keep edges cannot be border edges. The keep edges should be sharp. Fillet operation fails if twists are encountered.