You'll need to use the Linear dimension command, but set the Measurement method to Cylindrical. You'll also need to create a 3D centerline that you'll need to select as the first object when you create the dimension. Here is my recommended method:
- First, use the 3D Centerline command to create a centerline for the section cut view (you can select the curve in the section view that references the revolved edge of the part. NX will recognize it as a face).
- Next, select the Linear dimension command, and make sure to set the Measurement method to Cylindrical.
- Select the 3D centerline as your first selection (make sure to select the centerline FIRST, or you'll get the wrong measurement)
- Then, select the edge of the part that you want measured.
- Before placing the dimension, right-click and select Edit.
- Click the "Arrow Line" hotspot on the arrow you want to remove from the fiew. This displays the edit options for the arrowhead display.
- From the Arrow Line edit options, click the Settings button to open the Settings dialog box and change the display settings for the arrow line you do not want to be visible. Don't forget to click the main Edit button again (to exit the Edit mode) before you try to place the dimension.
I was having a problem using a baseline (which is the centerline in your example).
It is not in the view because the part is large. You have to name the centerline
so you can reference it by using the name selection bar (new to me) as your first pick.
The entities you pick to create a dimension do not have to appear in the same view. If the center of the part shows up in a different view, you can select it there when creating the dimension.
None of my views have centerlines in them. Not even close, so we always named the centerline
"CLINE" or something like that and then used baseline in the cylindrical dimensioning. Now, in NX9, under the linear dimension there is a toggle called "use baseline". But for the life of me I couldn't figure where to enter the name of the baseline.
I found this note in the NX 9 Drafting Help collection for Linear dimensions: Does this help?
If you create a name for the line using the Name property on the General tab of the Properties dialog box, and then make the line invisible, you must type the name in the Name Selection text box in the Selection bar to select the line
"None of my views have centerlines in them."
Do any of your views show the circular edge of the hole? The centerpoint can be used in lieu of a centerline.
Regarding entering the name in the selection bar: you may have to customize the selection bar to add the "name input" control, I don't think it shows up by default.
That's exactly what the problem was. The Name Selection box was not visible on the
selection bar. I added the Name Selection box to the selection bar, typed in "CLINE" (the name of my centerline) and that's my first pick. Then you can pick any line on the cross-section and
it gives you the diameter dimension. Thanks, guys.