Unlink View in UG Drafting

[Jamziee]

Hi Guys,

Is there a way to unlink a Detail View from it's parent view in UG Drafting?

I'd like to modify the model but ensure the detail view remains unchanged.


If there is no easy way, is there a way I can export the Detail View as a DXF, and re-import it as a seperate entity?


Cheers,

Andy James
Draughtsperson

 

[cowski]

I don't know of a way to unlink a detail view, but you have made me curious; why would you want to change the model and not have a detail view show the latest change?

 

[Azrael]

Good question Cowski, why would you want it?

But if you want it you can just turn the view to "reference" in the view style meny (general tab).

Note that the view will not be visible in UG but will when plotted.

 

[Jamziee]

Hi,

The reason for this was to have "before" and "after" machining views.

I was going to copy the detail view so there would be two of them. The intention was then to 'unlink' one of them before I modified the model to show the after effect.

(I don't want to create 2 large models for this minor change in views)

I have tried exporting to a DXF file, but does not export the detail views..... any ideas?

P.S. I'm using UG v18.

Thanks,

Andy.

 

[Azrael]

OK, try this, it should work.

1)Go to drafting.

2)Make a layer to work were you want the before parts to be.

3)Expand that view

4)Choose "extract curve"->"all in work view"

5)Go out from expand

6)Use "visible in view" on that view and make only the layer you chosen earlier to visible.

 

[Xwheelguy]

Along with Azrael's steps, you may have to re-associate any dimensions from the model curves to the newly extracted curves created in the steps above.

I wonder if turning the view into a Reference View would work? I don't have any experience working with Reference Views, so I'm taking a shot in the dark here.

Tim Flater
Senior Designer
Enkei America, Inc.

http://www.enkei.com

 

[cowski]

I think a promoted body could do what you want. You could have the primary version of the part then promote it and do the secondary operations on it. Search on the term 'promote' in assembly help it should be fairly easy to find. It also mentions wave linking. I don't have experience with promotions or wave linking, but maybe someone else here does and can give you some pointers.

 

[ewh]

Using wave or promoted geometry would probably be the best and cleanest way to do it. Unless you are modifying many parts, the file size should not be greatly affected.

Move the solids that are going to be modified to their own layer. Extract wave or promoted bodies from them on another layer. Perform the machining operations on the promoted or wave bodies.

In your "before" detail view, make the promoted or wave layer invisible. In the "after" view, make the original bodies layer invisible.

Hope that helps!

 

[vrn72]

If the view is going to be only for reference, you can take a round about way to achieve this.

1. Create a new drawing Drawing->New.
2. Move the required view to the created drawing sheet.
3. Export the Sheet as CGM ( or you can choose the display)
4. Open a new UG file
5. Import the CGM and save the file
6. Import the new UG file into the drawing where you want to use the view as reference.
7. If you are happy with this, goahead and modify your model and update the drawing.

This is one of the ways !!

Best of luck

 

[ewh]

One of the best reasons for using wave bodies is that they will update should the parent parts be changed or updated. I feel it is a waste of expensive software to simply use it as an electronic drawingboard. You could use AutoCad for that.

 

[64polara]

I'm with vrn72 on using the CGM method. We do this when we have to create Engineering Change Notices to show a was is.
Also sometimes the designer would like to show an assembly of a latch for example in both the extended and retracted positions. Do what vrn72 suggested it works for us I'm sure it will work for you also.

Wayne Huseby
Drafter/Checker
Goodrich Corp
Jamestown, ND 58401
701-253-7799

 

[cowski]

Keeping a copy for a revision or engineering change notice is one thing, but going through that process just to show a before/after of a machining operation seems ridiculous to me (although it IS a way to get what you asked for in the original post). I agree with ewh that you want to keep the associativity and use the tools available in Unigraphics. Think what happens if (and more likely when) the base part changes; now you have to suppress back to the before machined state, make your view, export it, import it, unsuppress your part, and update the rest of your views. Seems like a lot of work when wave link or promotion will get what you want and update automatically.