Diameter dimension on detail

[cubalibre000]

Hi,
how can I dimension a diameter in a detail view if I can pick only half part ?
See attached image.

Thank you...

Using NX 8 and TC9.1

 

[CAD2015]

Select dimension → Style → Dimension → Click on Disply Arrow and Extension Line on Side 1 or 2 (on the upper left corner)

MZ7DYJ

 

[cubalibre000]

Hi MZ7DYJ,
how can I dimension a diameter in a detailed view if I can only pick half shape ?
Understand ?

Thank you...

Using NX 8 and TC9.1

 

[cowski]

Start the diameter dimension, pick the side you want to dimension to in the detail view, pick the other side of the diameter in the parent view (or other view where it shows up). Now hide the dimension line that you don't want using mz7dyj's method.

www.nxjournaling.com

 

[Xwheelguy]

You can also use a Cylindrical dimension and pick any type of Centerline (2D or 3D - from the Utility Symbols, not a 2D Line element), then the Face or Edge that makes the diameter and it should double the dimension value. There might be an Annotation preference or Customer Default that needs to be set in order to double the value. Been too long since I've had to admin a seat of UG/NX.

Tim Flater
NX Designer
NX 8.0.3.4
Win7 Pro x64 SP1
Intel Xeon 2.53 GHz 6GB RAM
NVIDIA Quadro 4000 2GB

 

[ewh]

Tim's method is my preferred one. As long as you can get a centerline on the correct axis, the only other thing that needs to be done is turning off one extension and dimension line. If none are handy, I create a new centerline for the dimension, often by increasing the boundary of the view and placing the centerline in the view. After the dimension is placed, it is a simple matter to resize the view bounds to their original size. Many ways to skin a cat...

“Know the rules well, so you can break them effectively.”
-Dalai Lama XIV