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Diameter dimension setting

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Participant

Diameter dimension setting

I have been trying to find the setting to change a default Radial dimension on a drawing to read in Diameter or vice versa. I figured it should be a right click or somwhere under Properties but I have not found it. Can someone direct me how to do this?

5 REPLIES 5
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Re: Diameter dimension setting

Typically is is how the dimension is measured. Is this a dimension that you are adding to the drawing or one that done through the development of the model. If it's radius in the model, it'll be radius in the drawing. Same for diameter.

If you are adding a drawing, you need to click the radius, the ctrl-click the radius again to have it be a diameter dimension.

No toggle that I am aware of.

Thanks, Dale

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Re: Diameter dimension setting

Some are revolve dimensions in the model. Thanks

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Re: Diameter dimension setting

You cannot flip from a radius to a diameter or the reverse. You need to delete the dimension and recreate it.

If the dimension is a model dimension rather than a dimension created in the drawing,(it's a sketch dim, which is likely) you can use the 'replace' command in sketcher. In Creo Elements Pro 5 / WF5 and earlier, it's under the 'edit' menu in sketcher, in Creo 1 and newer it's under the Operations area of the sketch tab.

You select replace, select the old dim and then create a new one. The new dim will take the ID of the old one, so all notes attached to it and any place it is displayed in a drawing should be the same.

--
Doug Schaefer | Experienced Mechanical Design Engineer
LinkedIn
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Re: Diameter dimension setting

Not the "EASY" button I was looking for but helpful. Thanks Doug. All are in the model creation for the most part.

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Re: Diameter dimension setting

It is certainly version dependent but generating radial dimensions vs diameter can be managed when they are 1st defined.

  • Clicking the arc/radius twice before placing the dimension will create a diameter dimension. This is true on drawings and in sketcher.

  • Creating a centerline in a revolve sketch allows you to define a diameter if you 1st click the feature, then the centerline, and the 1st feature again. In Creo 2, if you have a datum centerline (as opposed to a general CL), sketcher will self-assign diameters for the revolve section.

  • Doug's "replace" tip is also great.

This has been basic functionality since Pro|E with a few enhancements in Creo.

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