Need to update drawing after moving models?

[Tablor]

Hi,

So I had a bunch of parts that were created at 0,0,0 and put on a drawing. They were subsequently moved to their correct aircraft coordinate which causes them to appear incorrectly on the drawing sheet. I'm sure this is something everyone is familiar with. I'm new to UG and was wondering if this can be fixed easily. The drawing views were created from saved model views. It seems like you ought to be able to update the orientation of the saved views and the drawing views would update to reflect those changes. Any help is much appreciated.

 

[Tablor]

Sorry, I should have added I'm on NX6.0.

 

[jerry1423]

Are you using "master model" ?
In other words is there a seperate model and drawing file?

 

[jerry1423]

If you are using "master model" then it is not a big deal to move the part back to 0,0,0 in the model space of the drawing file. Just using the "move component" command.
Just make sure your drawing file is the work part.

 

[Tablor]

Yes, all of the parts in the installation are in their own file. The drawing is created in a separate file with all of the parts as components in that part.

 

[Tablor]

Our drawing standards would make moving the file back to abs 0 against the rules. So I guess the question remains, is it possible to update the view orientation from the drawing view?

Thanks for the help - my resources are limited.

 

[jerry1423]

I guess it depends on how far the part was moved ...
Make the drawing sheet really, really big and then do a drawing view update - The drawing border will look small, but that is OK. The views may be outside of the border, but that is OK too, just move the views back inside. Put the drawing sheet back to the proper size when you are done, and the border will look fine.
The views are listed in the part navigator, so click on them in there to see if they highlight on the drawing. If there are some in "black space" someplace then pick it in the navigator and try to move it onto the drawing.
Airplanes can be really big, so it really depends a lot on how far it was moved.

I hope someone else can help you more, and have a better solution.

 

[jerry1423]

When you make the drawing sheet really, really big you will need to click on "custom size" instead of scrolling to the size.

 

[Tablor]

Thanks Jerry,

That works sometimes if the orientation of the part wasn't changed, but it's more likely that the part has been rotated on a couple of axis. I haven't been able to change the orientation of the part in the drawing view after moving the model.prt.

 

[jerry1423]

I was going to mention that if the orientation has changed then you are out of luck.
I really hope someone else has a better solution for you.

 

[JohnRBaker]

Drawing views are COPIES of the original Model views with no associative links.

OK, try this. Select a view you wish to 'fix', press MB3 and select the 'Edit' option. When the dialog comes up, int eh section titled 'Model View', select the 'Orient View Tool' button. A separate window will be displayed showing the part as it currently appears on the drawing. Now I suspect that one of your problems might be that you can't even see the Part at all, so in that case, the first thing you do when this window comes-up is place your cursor in the window and press MB3 and select 'Fit', just like you were back in modeling. In fact, while this window is open, you can rotate the model around using either your Spaceball or Mouse gestures, again just like you were back in modeling. Now you can either eyeball it until the model looks correct for this view or you can select references under the Normal Direction and the X Direction steps to align the model the way you wish it to be aligned. Once it looks right, just hit OK and that will become the new orientation for this view. Now just repeat as needed. Note that Section Views will probably take care of themselves once the parent view has been moved back to it's original orientation.

Now that will take care of the views, but the annotation is another thing as you will have to decide whether it easier to delete and recreate or if it's just a few Dimensions and Labels you can just re-associate them.

Anyway, that's how it's currently done.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

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

 

[ewh]

John,
That only seems to work on base views, and not projected views.

"Good to know you got shoes to wear when you find the floor." - [small]Robert Hunter[/small]

 

[Tablor]

John,

That does the trick. Thanks very much, it's quite a few parts that need to be fixed. I'm pretty sure this will be quicker than recreating all of the views. Reassociating the dims in NX6 is much better than what we had in NX3 so that won't be too much trouble.

I had been using VIEW-ORIENT to save the view in modeling that I wanted to have on the drawing. Using this edit option it's a different tool to orient the view. Is it possible to get the other tool? I was able to use VIEW-ORIENT-TYPE-INFERRED very easily, but it doesn't look like that's an option in the dialogue you've sent me to.

It works though and is just a couple more clicks. Thanks again.