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MichaelWittig1-Visitor
1-Visitor
September 2, 2010
Solved

When doing a revolve, is there a way of turning a radius dimension into a diameter dimension in the sketch?

  • September 2, 2010
  • 5 replies
  • 27129 views

Hello,

Lets say I am drawing a washer using a revolve. I draw a rectangle above the axis of rotation. The only way I can dimension the washer seems to be by dimensioning to the axis. Is there a way of converting these dimensions to diameter dimensions instead of radius dimensions in the sketch?

Thanks,

Mike


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Best answer by Kevin

Depending on the version you're using you can also use sketcher_dim_of_revolve_axis (added in WF4) to automatically create a diameter dimension when creating revolve features.

5 replies

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DavidButz1-Visitor
1-Visitor
September 2, 2010

Yes, pick the axis, pick the radial point, pick the axis again, and place the dimension. (It can also be done, point, axis, point, but the first way is generally easier.)

    M
    MichaelWittig1-VisitorAuthor
    1-Visitor
    September 2, 2010

    I can't get this to work using wildfire 3.0. Do I have to pick an axis or can I use Line (Reference)? If so, how do I hide the Line (Reference) so I can pick the axis?

    A
    ArvinParmar1-Visitor
    1-Visitor
    September 2, 2010

    pick the axis, then the parallel line, and then the axis again.

      K
      Kevin1-VisitorAnswer
      1-Visitor
      September 2, 2010

      Depending on the version you're using you can also use sketcher_dim_of_revolve_axis (added in WF4) to automatically create a diameter dimension when creating revolve features.

      B
      BrentDrysdale12-Amethyst
      12-Amethyst
      September 2, 2010

      Hi Mike,

      I think the thing that you may be missing is for you to have a sketched centerline created in the sketcher (or use edge and select the pre-existing axis). If you try and create the diameter dimesion just using a sketcher reference it will not work but as soon as you have the "centerline" in your sketch this should work. Has worked this way since at least WF2

      Hope this helps.

      Regards, Brent Drysdale

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      MichaelWittig1-VisitorAuthor
      1-Visitor
      September 3, 2010

      For anyone else that finds this thread...the procedure is...

      1) choose the centerline (dashed line) from the line flyout on the sketcher toolbar

      2) draw your centerline

      3) draw your profile

      4) choose the dimensioning button on the sketcher toolbar

      5) select the entity on the profile you are dimensioning to

      6) select the centerline

      7) select the entity on the profile you are dimensioning to AGAIN (MUST DO THIS)

      😎 use the middle mouse button to place the diameter dimension

      Mike

      E
      ebeattie1-Visitor
      1-Visitor
      May 14, 2015

      This is how I have always done it, by selecting the entity then the center-line then the entity again and placing the dimension. Works every time.

      J
      JASONBONIFACE1-Visitor
      1-Visitor
      November 26, 2012

      You could try the following config option:

      sketcher_dim_of_revolve_axis

      (if this option is set all dimensions created by intent manager to axis of revolution will be diameter dimensions).

      and set to yes.

      Works a treat for me!

        R
        rmarion1-Visitor
        1-Visitor
        May 14, 2015

        Another option is to add your Centerline entity using the Two-Point Geometry Centerline option over on the left side of the Sketcher ribbon. When you add dimensions with their dimension lines oriented normal(perpendicular) to the Two-Point Geometry Centerline entity they will automatically be added as diameter dimensions. Most users add their Centerline entity for a Revolve feature using the Two-Point Construction Centerline command.

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