topic Re: When doing a revolve, is there a way of turning a radius dimension into a diameter dimension in the sketch? in 3D Part & Assembly Design

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

MichaelWittig — Sun, 13 Dec 2020 04:06:23 GMT

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

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

DavidButz — Thu, 02 Sep 2010 00:31:06 GMT

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.)

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

Kevin — Thu, 02 Sep 2010 06:48:55 GMT

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.

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

MichaelWittig — Thu, 02 Sep 2010 15:58:35 GMT

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?

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

ArvinParmar — Thu, 02 Sep 2010 17:20:06 GMT

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

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

MichaelWittig — Thu, 02 Sep 2010 21:24:40 GMT

using wildfire 3, this doesn't seem to work. I tried selecting an axis while in a sketch and I cannot; therefore I tried selecting the "Create defining dimension" button on the toolbar, selecting the Line (Reference) running horizontally along the screen, then select the entity I am dimensioning to, then select the Line (Reference) again, then clicking the middle mouse button. No dimension shows up. Then I tried deleting the Line (Reference), using Sketch, References, and creating a reference line off an axis I created before the sketch, then repeated the procedure above. It still didn't work. Can anyone confirm that this should work on wildfire 3?

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

Kevin — Thu, 02 Sep 2010 22:19:37 GMT

The axis you select needs to be a sketcher centerline. You can can also try selecting the line, centerline, and line again them MMB to place the dimension.

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

BrentDrysdale — Thu, 02 Sep 2010 22:43:37 GMT

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

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

MichaelWittig — Fri, 03 Sep 2010 00:42:32 GMT

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

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

JASONBONIFACE — Mon, 26 Nov 2012 10:28:32 GMT

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!

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

rmarion — Thu, 14 May 2015 17:20:41 GMT

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.

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

ebeattie — Thu, 14 May 2015 19:02:04 GMT

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.