Revolve

A revolve is obtained by a rotational sweep of an open or closed profile. The rotation is based on a desired sweep angle around an axis.

This task shows you how to define a revolve.

Open the Revolve.CATPart document.

 

 

  1. Click any icon requiring a shape definition. For example, launch the Shellable capability , then click the Revolve icon.

    2. Profile/Surface

    All the Shape features have a Profile/Surface as part of the Revolve geometry definition. You can select an existing sketch, a sketch output, a sketch output profile profile or surface as a Profile/Surface of the Revolve definition. 

    If you launch the command with no profile previously defined, you can access to the Sketcher by clicking the icon available in the dialog box and sketch the profile you need.
 

    You can also select any face originated by Functional Features of any Functional Body. In this case, the face needs to be the original untrimmed (unmerged) of the feature.

    You can also select any topological (trimmed) face of any Part Design body that is not the Part Body containing the active Functional Body.

  1. Select Sketch.2 as the profile you wish to revolve.

    Limits

    By default, the application specifies the length of your revolve feature and previews limits. LIM1 corresponds to the first angle value, and LIM2 corresponds to the second angle value.

  2. The first angle value is by default 360 degrees. Enter the value of your choice in the First angle field if you wish to define a different angle value. For example, enter 100 degrees.

  3. Enter the value of your choice the Second angle field to define the second angle value.

    The Selection field in the Axis frame is reserved for the axes you explicitly select. 

    Clicking the Reverse Direction button reverses the extrusion direction. Another way of reversing the direction is by clicking the arrow in the geometry area.

    Fillet

  4. Click the Fillet tab.

  5. Check the Lateral radius option if you wish to fillet lateral edges. Then, you merely need to set the radius value of your choice.

  6. Check the First radius option if you wish to fillet top edges. Then, you merely need to set the radius value of your choice.

  7. Check the  Second radius option if you wish to fillet bottom edges. Then, you merely need to set the radius value of your choice.

    To add an intersection fillet, you can choose between Intersection with Core/Cavity, Intersection with Core or Intersection with Cavity from the Intersection Fillet list. In this case following three options are available:
    • The Fillet radius option enables you to add material to the feature.
    • The Round radius option enables you to remove material from the feature.
    • The Preserve Thickness option enables you to keep the thickness applied on the part.

    Thick

  8. Check the Thick option. This option enables you to add material to both sides of the profile.

    Three additional options display:

  9. Enter, for example, 6mm in the Thickness1 field and click Preview. Thickness is added to the inside of the profile.

  10. Enter 3mm in the Thickness2 field . The application previews how the thickness is added to the outside of the profile.

  1. To add material equally to both sides of the profile, check Neutral fiber. The application previews the result. The thickness you defined for Thickness1 is evenly distributed.

    Core (Specific to Shellable Features)

    The Core capability enables you to define a core body (offset) for a shellable feature.