Drafting View Edit?

[zora65]

Need advice on how to accomplish a tweak to an assembly view in drafting. I have an assembly which is basically a stack of aluminum sheets with an attached foam backing. The aluminum extends past the foam backing on two of the edges. The stack consists of 10 or more layers and then all the layers of aluminum are pinched together and welded on the two ends. The welds are centered vertically on the stack. My assembly model shows the stack of aluminum foam sheets prior to pinch and weld operation (so they are all identical). In the drawing, I have a top view that will work fine but the problem is how to handle the end view that will show the pinched together edges.
What is the best way to handle this situation? Is there a way to edit the view and add the required curves? I would like to avoid creating multiple models with the different curves required to get this view and hope there is a better way. Any advice or tips on what others do in similar situations is appreciated.

I’m using NX3 with Teamcenter Eng
No help files installed
Maintenance agreement expired
They laid off the guys with experience in UG


BSilk
Senior Designer

 

[JohnRBaker]

With the drawing open, go to the view that you wish to make changes in and select it and press MB3 and select "Expand Member View". Now you can make any sort of edit you wish, removing objects using View Dependent Edits and adding objects using curves. Once you have it looking the way you wish, just unexpand the view and you're back in your drawing but with a modified view(s).

John R. Baker, P.E.
Product "Evangelist"
NX Product Line
UGS Corp
Cypress, CA
Phone: 714-952-6032
FAX: 714-952-5758
John.R.Baker@ugs.com

 

[Xwheelguy]

One thing John failed to mention is that you can't be zoomed in too close to the view or else the view won't expand....at least that is what happens to me most of the time, if I cannot see the view border when zoomed in.

Tim Flater
Senior Designer
Enkei America, Inc.

http://www.enkei.com

 

[fgbrender]

Didn't you know you don't need experience to run NX?

I'm sorry, that was sarcasm being one of those laid off. I'm happy to report I found employment at a company that respects experience...

Now that I got that off my chest, I'm curious why you would not create an alternate representation of the parts to show their final geometry. In my experience it is just as important to the final product. Being that I'm not familiar with what your product is, it may not be nessesary and John's suggestion would work just fine. Of course this meens your drawing does not accuratly reflect your model and your model does not accuratly reflect your finished product but again not knowing your product, this may be perfectly OK.

 

[JohnRBaker]

That's correct. The only reliable mechanism for selecting a view is by selecting its border/boundary. If you can't see this, then it's going to be difficult, if not impossible, to actually select the view.

John R. Baker, P.E.
Product "Evangelist"
NX Product Line
UGS Corp
Cypress, CA
Phone: 714-952-6032
FAX: 714-952-5758
John.R.Baker@ugs.com

 

[fgbrender]

I almost forgot...

You could also use the "Part Deformation" functionality to do this. Basically it allows you to create your model "as designed" and add it to an assembly "as assembled".

It seems a bit complicated at first but is actually quite easy and better represents the actual product from single parts to complete vehicle or whatever you are creating.

When I get a chance I'll post an example.....

 

[mjcole]

Can't you also select the View fron the Model/Drawing navigator and expand it that way?

Michael