Minimum distance dimension?

[edgray]

I cannot figure out how to create a dimension that is the minimum distance between two holes or other approaching curved shapes. I can get the value via analysis->Measure Distance but I would like it on a drawing.

 

[JohnRBaker]

You can't really dimension between 'faces' in drafting, only curves/edges, however...

You say that you can find the minimum distance with no problem using Measure Distance. OK, using Measure Distance, select the two faces of interest and when you see the result displayed on the screen, expand the section of the dialog titled 'Results Display' and select the Annotation option 'Create Line' and hit OK. Now make sure that the line is included in the Model Reference Set so that when you make your drawing it will be visible and selectable, which is what you DIMENSION in the Drawing. When finished, Hide the line and you're all set.

However, there is one issue to remember, even if you had toggled ON the 'Associate' option when doing the measurement, the line which was created will NOT update.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

To an Engineer, the glass is twice as big as it needs to be.

 

[edgray]

I am talking about working only in drawing mode. So when I use the Measure Distance function a am picking two drawing elements in a section view. It seems to me that since the system can resolve the distance value it would not be that big a step to create the output as a dimension.

I have used the create line work around in the past, I was hoping for an actual function.

This is not something I do that often but it sure would be handy when I need it. I personally try to stay away from drawings. I use them mostly for checking the fit of my assemblies. Hence the desire to document clearance.

 

[cowski]

Looks like a good candidate for an enhancement request.

 

[JohnRBaker]

If you're working in a Section View then all you have are curves. Have you tried using Parallel Dimensions setting the Snap Point to only 'Tangent Point' when dimensioning between non-linear objects, such as the two holes shown in the attached image?

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

To an Engineer, the glass is twice as big as it needs to be.

 

[edgray]

That worked great John. Thank you. I thought there ought to be a way.