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This task shows how to create a face-face fillet.
The fillet surface is obtained by rolling a sphere, which radius is larger
than the distance between the selected elements, between the selected
surfaces.You generally use the Face-Face fillet command when there is no
intersection between the faces or when there are more than two sharp edges
between the faces. |
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Open the
FaceFillet1.CATPart document. |
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Click Face-Face Fillet
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The Face-Face Fillet Definition dialog box appears.
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Select the two Faces to fillet.
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Select the Extremities type, that is the
relimitation mode.
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- Straight: no tangency constraint is imposed at the
connecting point between the fillet and the initial support,
generating sometimes a sharp angle
- Smooth: a tangency constraint is imposed at
the connection between the fillet surface and the support surfaces,
thus smoothing the connection
- Maximum: the fillet surface is limited by the
longest selected edge
- Minimum: the fillet surface is limited by the
shortest selected edge
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(Refer to Shape Fillet) |
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Enter a radius value in the Radius field if
you are not satisfied with the default one. This value must be greater
than 0.
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Click Preview.
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You can check Trim support elements to relimit
the support elements and assemble them to the fillet.
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Click OK.
The faces are filleted. This fillet is indicated in
the specification tree. |
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Note that
the selection of the feature prevails over the selection of the
sub-element.
To select a sub-element, you need to apply the ''Geometrical
Element'' filter in the User Selection Filter toolbar.
For further information, refer to
Selecting Using A Filter in CATIA Infrastructure User's Guide. |
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Limiting Elements
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While creating the fillet, you can limit it by
selecting an element (plane or surface) that intersects it completely in
the Limiting element field prior to selecting the trimming
element.
Once the edge to be
filleted has been selected, and the radius keyed in, click
Preview then More>>.
For further details, refer to
Limiting Fillets. |
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Hold
Curve
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Instead of entering a radius value, you can use a "hold
curve" to compute the fillet. Depending on the curve shape, the fillet
radius value is then more or less variable. |
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- Select both
faces as shown below
and click More>>.
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Select
Join.2 as the hold curve.
The curve must be sketched on one of the selected faces. |
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Select Sketch.7 as the spine.
The spine provides a better control of the fillet. |
The spine 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. |
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Preview the fillet:
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Repeat the operation and select
Sketch.3 as the spine:
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Click OK
to create the fillet.
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For more information, refer to Part Design User's Guide. |
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Filleting Volumes
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Open the
FilletingVolumes1.CATPart document. |
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Click Face-Face Fillet
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The Face-Face Fillet Definition dialog box appears. |
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Select the two Faces to fillet.
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Set the Radius to 10mm.
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Click Preview.
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Click OK to create the fillet volume.
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Extremities and
Trim support are grayed out, they cannot be used with volumes. |
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