![](../icons_C2/common/atarget.gif) |
Variable radius fillets are curved surfaces
defined according to a variable radius. A variable radius corner means that at least two
different constant radii are applied to two entire edges. This task shows how to create
a standard variable radius fillet. After performing the scenario, see also Variable Radius Fillets
Using a Spine. |
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Open the VariableRadiusFillet1.CATPart
document. |
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1. |
Click the Variable Radius Fillet icon . The
Variable
Radius Fillet Definition dialog box appears.
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2. |
Select the edge to be filleted. You can define variable radius fillets on closed
edges. See Variable Radius Fillets Using Closed Edges. CATIA detects both vertices and displays
two identical radius values.
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![](../icons_C2/common/ap2.gif) |
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Optionally,
click Preview to see the fillet to be created.
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![](images/bt281.gif)
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3. |
Enter a new radius value to
simultaneously change the radius of both vertices. For example, enter 12mm.
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The new radius value is displayed
on both vertices. The preview is modified accordingly. |
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![](images/dbfillet3NLS.gif) |
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Two propagation modes are
available:
![](_themes/v5r5/ul1.gif) | Minimal: the application does not take any tangencies into account.
If filleted edges overlap, the application trims the fillets and
creates a sharp edge. |
![](_themes/v5r5/ul1.gif) | Tangency: tangencies are taken
into account so as to fillet entire edges. |
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If you set the Tangency mode, the
new option "Trim ribbons" becomes available: you can then trim
the fillets to be created. For more, refer to Trimming
ribbons. |
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4. |
To add a point on the edge to make the variable radius fillet more
complex, click the Points: field.
You can also add points by selecting planes. For more information, refer to the end of
the task.
You can add as many points as you wish. |
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5. |
Click the Points
field then a point on the edge to be filleted. CATIA displays
the radius value on this
point.
Note that to remove a point from the selection, you just need to click this point.
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6. |
Enter a new radius value for this point: enter 4.
The new radius value is displayed.
This is your preview: |
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![](images/bt282.gif) |
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7. |
The propagation mode is set to Cubic: keep this mode. To see the Linear
propagation mode, refer to "More About Variable Radius Fillets".
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8. |
Click OK to confirm the operation. The edge is filleted. The
specification tree indicates this creation.
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![](images/bt283.gif) |
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9. |
To edit this fillet, double-click
EdgeFillet.1 in the specification tree. |
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10. |
Expand the
dialog box by clicking More.
Four additional options are available.
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![](../icons_C2/common/ainfo.gif) |
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To know how to use: |
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![](../icons_C2/common/anew.gif) |
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![](images/dbfillet7NLS.gif)
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Limiting Elements
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11. |
Click the
Limiting element field and select Plane.1as the plane that will trim the
fillet.
An arrow appears on the plane to indicate the portion of material that
will be kept.
This capability is supported on Part Design P2 only. |
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![](images/bt447.gif)
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It is now possible
to use one or more limiting elements. |
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12. |
Click this arrow to reverse the direction and
therefore specify that the portion of material to be kept will be
the opposite one. |
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13. |
Click OK.
The variable radius fillet is trimmed to Plane.1. The final part looks like this: |
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![](images/bt448.gif)
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![](../icons_C2/common/anew.gif) |
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You can now create limiting
elements just by clicking on the edge to be filleted.
The application displays this element as a blue disk: |
![](images/bt187.gif) |