NX10 Drafting dimension issue 1

[41EX]

Hi everyone,
I'm currently working on a drafting and I'm currently having an issue with a dimension.
I need to size a rectangular feature of which its sides aren't aligned with the horizontal and vertical axis (as shown in the attached document). The features are a line and a point. The reason why we use a point is because it's positioned on a face that is hidden by the view. We usually hide one of the extension lines and add the note "FROM DATUM X" (yea, I know we could do it another way but this is the common practice we're suppose to follow).
I tried several ways:
-Inferred (this doesn't work since NX won't allow me to select a 2nd feature even when I click on the "select 2nd feature button". NX switches right away to "placement location" tool instead of letting me choose my 2nd element)
-Linear dimension (this doesn't work since NX won't allow me to select a 2nd feature even when I click on the "select 2nd feature button". NX switches right away to "placement location" tool instead of letting me choose my 2nd element)
-Perpendicular dimension (I can at least select two features but NX won't accept place the dimension "in line" (or parallel, if I might say) with the line I selected. It snaps one of the line's end point and I make circles with the mouse around the feature location to try to have the orientation I want (parallel to the line I selected) and NX can't seem to understand the orientation I want.

I don't know if anyone else has experienced such issues with dimensions in the drafting but I would appreciate having suggestions.

Thanks
Alex

 

[JohnRBaker]

There was no "attached document".

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

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

 

[41EX]

Oops, I thought the file had uploaded.
I think it should work this time.

Thanks!

 

[cowski]

When using the "inferred" option, ignore the temporary dimension displayed after the first pick and continue on to your second pick. When selecting the line, I'd suggest clicking on it away from the control points (don't pick on the end or mid point of the line); this will help NX to infer that you want a perpendicular dimension.

www.nxjournaling.com

 

[41EX]

Thanks for the tip but it's not working.
Perhaps I should mention that the view shown in attachment is a projected view of a cylindrical surface.
When using an inferred dimension, it giving me a radial dimension and I can't select any other line.

However, I was able to use a turnaround; point to point.
I picked the point and the line's midpoint. The only issue there is that the extension line will have to be updated manually if the pocket size varies later in the design.

Thanks

 

[cowski]

So the "line" that you are selecting is actually a "drafting arc" which represents the circular edge of a planar face of a cylinder?

If so, try dimensioning from the face to the point object instead of using the line/arc object. You can select the face by using the "quick pick" list or by changing your selection filter. Dimensioning to the face should be more robust if/when the feature changes size.

www.nxjournaling.com

 

[SDETERS]

Here is a quick example. Cowski hit the nail on the head.

But this still does not take into account how frustrating it is to dimension a completely filleted part. How many times I have had to change the selection filter to Face to dimension a part.

try to dimension the width of the part. Do not select the center points that makes it to easy and not correct. This is a NX10 part

 

[41EX]

Cowski, you've just earned yourself a STAR.

I was able to select the face (something weird though, I could see the element being highlighted after I selected it) and I was able to get the dimension in the proper direction.

Thanks!