Component disappears in one view after updating a drawing (UG/NX)

[Kasey7]

Hola!
I'm using NX7.0.0.9. I have a drawing assembly that consists of a finished component displayed with an in-production component. The first view of the components was sectioned, and the section view was used to create a detail view. Some view dependent editing was applied to the sectioned view where any curves of the finished component that appeared within the production component (ie, not yet machined) where changed to hidden lines. Since some of these hidden lines were datum faces, they were used to construct reference dimensions to the machined faces of the in-production part.
Somewhere along the line, one or both of the components was resaved (were they edited? I don't know). No prob. I simply have to update the drawing. My problem is that updating causes the finished component to disappear from the sectioned view, and no other view. All my dimensions obviously have lost their assiciated curves and need to be reassociated. The weird thing is that the detail view still displays the finished component, and I can add dimensions to it.
Why would a component no longer appear in one view after an update, but not all? I don't believe it is blanked, but I'm at a loss as to how to get it to reappear in the sectioned view.

 

[jerry1423]

The best thing that I can think of is that the layer is no longer visible in that view. Maybe something funky happened in V7 and some entites got moved to a differnt layer.

format > visible in view > select view > reset to global

Then see if it appears.

You probably don't want to save the part until you understand what layers were invisble in that view, and why they were invisble.

 

[Kasey7]

Drat! That didn't work Jerry.

I should have mentioned that all the actions, from making the models, creating the assembly, and finally the drawing were performed in NX7.
Incidently, I was able to modify the models, and update the drawing assembly without any problems a few days ago. Just for some reason this week when I opened the drawing my views were out of date. Updating the views now causes the loss of the model on the one view.

 

[jerry1423]

I think I remember that happening to me a long time ago. It may have something to do with the clipping planes. I will look that up and see what I can find.

 

[jerry1423]

try this

rmc the drawing view > style > perspective

both my front clipping plane, and back clipping plane, are unchecked - maybe see if yours are too. If they are checked then do a "fit to extents" , or maybe just uncheck them.

 

[hudson888]

It could also be an out of date reference set in a component. A layer mask that you weren't aware of, such as visible in view mentioned earlier, but caused from the component side equally as likely as it could be per the assembly. For all we know something is just blanked, or "hidden" in modern parlance (did we get a vote on that by the way, I much preferred the old). Try going into the modelling application from the drawing side and just checking what you see from there you need to confirm that the component is 1) visible, and 2) on a layer shown in all the drawing views.

Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum

 

[Kasey7]

Jerry,
Took awhile but I finally figured out rmc means Right Mouse Click. I should have known that. 9.9
The clipping planes were unchecked. I checked them, which generated an automatic update. Once again the finished part disappeared. Fit to Extents didn't help. (I'm not saving the file when the component disappears, so I'm able to try various things.)

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Hudson,
Both components are visible in the modeling app. I checked, and tried different reference sets as well. Again, everything was fine after drawing updates last week. It's also weird that the component disappears from one view (the section view) after updating the drawing, but not the detail view, which is coming from the section view.

BTW, all modeling elements are on their default layers as well (solid on L1, sketches on L21, etc).

 

[jerry1423]

Check if the part that is disappearing is interfering with another part.
When working with press fit pins the same problem may occur that you are experiencing, because one solid body is inside another solid body.

Maybe move the part (a little bit) in the assembly to a differnt location to see if it will show up in the view.

 

[jerry1423]

Also turn on all hidden lines in that view to see if the component appears (as hidden). If it does then there is some sort of interference.

 

[Kasey7]

The parts are overlaid on top of one another and constrained (fixed). I even tried moving them apart so they were not touching to see if the one "missing" component would reappear, it didn't (at first, see below).
Turning on hidden lines does not display anything of the missing part either.

----------

Okay, I just tried something.
I must have done something wonky with View Dependant Edit to have caused all this. What I just tried is I separated the parts in the modeler and returned to the drafting app. I selected View Dependant Edit and Deleted Selected Erasures, then slected All. The part has reappeared. When I overlay the parts again, the missing part is visible now. (It wasn't visible the first time because it was moved off the displayed portion of the drafting sheet.)
Somehow, somewhere, I, or someone else accidently thought we were erasing a curve, when we erased the model. Is that possible?
Any way, I can see and the dimension the model now, but all the view dependant edits are gone. No biggie.


Thanks for your suggestions.

 

[jerry1423]

yes it is possible to erase the whole model, your filter may have been set to "solid body"

One this thing about this forum is that we learn from other people, and if this problem comes up again (here or anyplace else) I will know what to do.

 

[hudson888]

Yep that would have been my lucky last guess. How the heck you managed to do that by mistake we may never know.

Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum

 

[man2007]

It is best practice to set Curves, Edges in Type filter while using VDE, instead of picking the geometry from the screen directly, since there is chance of selecting Face or Solid Body instead of Curves and Edges.