Help! Cant find an important setting....

[Kenja824]

When we switched to NX9, we had a problem with all of the views in drafting being unselectable due to all edges were extracted lines.
There was a setting we changed, I believe in Customer Defaults, that fixed this. It seems to me it was something to do with making NX compatable to pre-nx8 or something like that.

I think we need to change that on someones computer now and I cant find where that setting was now. Can someone please help?

 

[Kenja824]

Ok, never mind. We found it. lol

Under Preferences - Drafting - View - Common - Configuration.
Representation needs to be set at "Exact (Pre-NX8.5)"

I am not sure if all the other settings do it, but we had at least one setting cause this problem. The modelers would model up a job and when the detailers placed views on the drafting side, they could not select any edges of the bodies. If you hover over the edges, it says "Extracted Line". Once switching this setting to "Exact (Pre-NX8.5)", anything we made after that worked fine.

This problem may only happen with particular programs from GM, like their Assembly Labels and such. I didnt dig far into it once we got it working right.

 

[JohnRBaker]

There is no reason why extracted edges should not be selectable. This only occurs if a view is added as a simple 'Lightweight' view. Starting with NX 8.5 we added two new view options, 'Exact' and 'Smart Lightweight', in either case, all edges should be selectable. There is NO need to revert to pre-NX 8.5 style views when creating NEW drawings. You should only expect to see pre-NX 8.5 views when you've actually opened an older Drawing. I woudl set your default to 'Exact' if your Models or Assemblies are not very large and if they are, that is Assemblies with thousands of Components, then I would opt for 'Smart Lightweight'. Note that you edit Drawing views and switch them between 'Exact' and 'Smart Lightweight' as needed, but once you create a Drawing view which has been set as Pre NX 8.5, you're stuck with it. If you would like to modernize the view to take advantage of new behaviors which depend on they being either 'Exact' or 'Smart Lightweight', you're out of luck.

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.

 

[cowski]

While writing journal code, I've run into at least one situation where the code works for "pre-NX 8.5 exact" views, but not the "exact" NX 8.5/9 views; and there were no commands added to the API to cover the lost functionality. I opened an IR with GTAC and found out that it won't be addressed until NX 10 (or possibly later). Once it is addressed, I can re-write the code to take advantage of the new commands, but those using NX 8.5/9 'exact' views will simply be left out.

I appreciate the 'continuous improvement' being made in NX, but sometimes it is worth holding on to the older methods until the bugs are worked out of the new stuff...

www.nxjournaling.com

 

[Kenja824]

Recently, we have had someone do a save as to an older file. It acted similar to the problems I mentioned before in this thread. However, it was more specific.

In drafting views, he could dimension it and everything just fine. But when he tried to add assembly labels they would not attach to the edges. It was as if the entire assembly was unselectable. He could select the component, and select where to position the label, but when he tried to select an edge to attach the label, nothing was selectable.

I noticed again, in this view, the edges said "Extracted Line" when you hovered over them. It seems that whenever there is a problem with selecting an edge, it is alwas when the edge is an extracted line rather than an edge of a body. But we never extract edges to create this problem.

I had orignally thought it had to do with the Exact Pre-8.5 setting. When I had him go to where that setting is, it just said "Exact". So it seems that when we have this problem it always has to do with the file being made with the "Exact" setting. I also noticed that switching the setting after the file is made does not help. If it is made in exact, we seem to have a problem with Assembly Labels attaching, even if we switch it to Pre-8.5. If it is made with Exact Pre-8.5, we are fine.

One other thing I notice is that the top of our NX says "Unigraphics NX 8.0 (UG PDL 8)". Though we are using NX9 with the ribbon setups. Could this mean their was a problem in installing NX that may be causing this problem?

 

[Kenja824]

Well, this problem has been remedied, and I must say, it is embarrassing.

Originally I thought we needed to have this setting....
Under Preferences - Drafting - View - Common - Configuration.
Representation needs to be set at "Exact (Pre-NX8.5)"

However, our problem and cure, seems to have been hiding right before my eyes. In that same place for the PRE-NX8.5 setting, right below it is a check box "Extracted Edges". We had that chacked! When this is checked, GM labels will not attach to the edges. Uncheck it and everything seems fine.

Appologies for my stupidity. lol I only point this out in case someone else in the future misses such an obvious fix themselves. lol

 

[asrura1]

I don't think you should apologize for your "stupidity".

I appreciate you posting your problem and also the solution for it. Although I did not encounter your problem, I did learn something and checked off "Extracted Edges" a moment ago.

Thank you, sir, for taking the time to write up your solution. Really appreciate it.