diameter dimension on detail view

[teookie]

I would like to put a diameter dimension on a feature located in a detail view. The feature is very small, so I need the detail at 4/1 scale in order to see it. The "other side" of the diameter is located off view. Is there a way to add this type of diameter dimension in NX? Example picture attached.

Thanks.

 

[JohnRBaker]

What version of NX are you using?

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

http://www.siemens.com/plm

UG/NX Museum:

http://www.plmworld.org/p/cm/ld/fid=209

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

 

[teookie]

Sorry I forgot to mention that.

6.0.5.3

 

[Xwheelguy]

John might have a simpler way of doing this, but what I used to do was expand the detail view boundary to show the geometry from which the centerline of that diameter you're showing is derived. I would then Expand the view and place the centerline in the view (2D Centerline or 3D Centerline). Unexpand the view and using a cylindrical dimension, dimension from the centerline out to the geometry - the value should double if you have your defaults and preferences set correctly. From there, it's a matter of manually placing the dimension close to your detail view geometry, turning off the first extension line, and changing the arrowhead type for arrow 1 to double arrows. Lastly, fix your detail view boundary. You cannot shorten the side with double arrows, so either leave it as it is or turn it off via Style. If you MUST have it, then either create a custom symbol for the side that won't shorten or create it as view dependent geometry (old school). If you make a custom symbol, you can set the origin for it to be associative to the dimension text and it should follow it where ever you drag it.

Hope that's not too confusing.

Tim Flater
NX Designer
NX 7.5.4.4 MP2
WinXP Pro x64 SP2
Intel Xeon 2.53 GHz 6GB RAM
NVIDIA Quadro 4000 2GB

 

[teookie]

xwheelguy that makes sense. I did have to read it twice though Thanks for the help.

 

[Xwheelguy]

No problem, teookie.

Looking at some drawings we have onsite, I'd recommend making symbols, User-Defined or Custom, with at least one pointing up and one pointing down. For maximum flexibility, I'd recommend making a few with varying dimension line lengths for the double arrows; say 6-8 in total.

I did some playing around and you don't necessarily have to go through that whole process - you can dimension to any other view's Centerline that is parallel to your detail and it will double the dimension - just make sure it's the SAME Centerline as you'd have used in the above steps, just in another view. The Centerline doesn't have to be View Dependent either. Hope that isn't even more confusing.

Mess around with a Cylinder (maybe with a hole in it) and create a Detail view of one end. Throw a 2D or 3D Centerline on the parent view, then dimension to the cylinder's outer diameter (furthest edge from the parent view's Centerline).

Tim Flater
NX Designer
NX 7.5.4.4 MP2
WinXP Pro x64 SP2
Intel Xeon 2.53 GHz 6GB RAM
NVIDIA Quadro 4000 2GB