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Grooves are revolved features that remove
material from existing features. This task shows you how to create a groove, that is how
to revolve a profile about an axis (or construction line). |
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You can use wireframe
geometry as your profile and axes created with the Local
Axis capability. |
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Open the Revolution.CATPart
document. |
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1.
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Click the Groove icon
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2. |
Select the profile.
The Groove Definition dialog box is displayed
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The application displays the name of the selected sketch in the
Selection field from the Profile frame.
The Selection field in the Axis frame is reserved for the
axes you explicitly select. For the purposes of our scenario, the profile and the axis belong to the same sketch.
Consequently, you do not have to select the axis.
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The system previews a groove entirely
revolving about the axis.
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About Profiles
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can create grooves from sketches including several closed profiles. These profiles must not
intersect and they must be on the same side of the axis. |
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needed, you can change the sketch by clicking the Selection field and by
selecting another sketch in the geometry or in the specification tree. |
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Clicking the
icon
opens the Sketcher. You can then edit the profile. Once
you have done your modifications, the Groove Definition dialog box
reappears to let you finish your design. |
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If you launch the Shaft command
with no profile previously defined, just click the icon
and select a plane to access the Sketcher, then sketch the profile you need. |
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3. |
The application previews the limits LIM1 and LIM2 of the groove to
be created.
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You can select these limits and drag them onto the desired value or enter
angle values in the appropriate fields. For our scenario, select LIM1 and drag it onto
100, then enter 60 in the Second angle field. |
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4. |
Optionally click Preview to see the
result. Just a portion of material is going to be removed now.
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5. |
Click the Reverse
Direction button to inverse the revolution direction, or use the Reverse
direction contextual command available from the arrow.
As an alternative, click the arrow to obtain the direction as shown:
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6. |
Click OK to confirm the operation. CATIA removes material around the
cylinder. The specification tree indicates the groove has been created.
This is your groove:
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6. |
The option Reverse
Side lets
you choose between creating material between the axis and the profile,
which is the default direction, or
between the profile and existing material. You can apply this option to open or closed profiles.
Double-click the groove to edit it. Now, you are going to remove the material surrounding the profile.
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7. |
Click the Reverse Side button or alternatively click the arrow
in the geometry. |
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8. |
Enter 360 as the first angle value and 0 as the
second angle value. The application
previews the new groove. |
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9. |
Click OK to confirm.
The material surrounding the profile has been removed. |
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