Dimensioning to Section View Background Objects

[ChaseWichert]

I have a part that I have a section through; however, I need to dimension and angle from a center of a circle to a center of a line, to another line. The circle is on a background object, the section line isn't going through the object, and I am unable, in anyway that I can find to try, to create a point or a line that I can use as a reference to show the line from the center of the circle to the center of the line. This line is imaginary and I need to show it, but nothing will snap. Any Suggestions?

Thanks,
Chase

 

[JohnRBaker]

What version of NX are you using?

Irrespective of that, try creating a Sketch in the context of the Drawing view itself (select the view, press MB3 and select 'Active Sketch View'). Now with the 'Selection Scope' option on the Selection Bar set to 'Entire Assembly', you should be able to select points even in the background area of the Section View, when creating your sketch curves.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

 

[ChaseWichert]

Sorry, 7.5. I tried that and it didn't work. I had a colleague tell me about Extract Curves in View Style, and turning it to Associative instead of None.

 

[JohnRBaker]

If you're just wanting to select 'Snap Points', such as 'Arc Center', 'End Point', etc., when creating Sketch curves, extracting edges is NOT necessary. However, you MUST be Sketching in the context of the VIEW and NOT the Drawing, and the 'Selection Scope' must be set to 'Entire Assembly' if you're working in Master Model mode.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

 

[ChaseWichert]

Entire Assembly is the answer. Thank you!