Solved: Re: Detailing issues Creo 3.0

jschutte · ‎Sep 23, 2016

This is a complicated small plastic plastic part that has three separate parts insert molded into it. One of the other parts is plastic, one is brass, plus an o-ring. Rev A & B was created in Creo 2.0 M090. The model is actually an assembly of all four parts. All I need to do is add a spec to a note in the drawing... that's it, a simple note change. I open the drawing in Creo 3.0 & find that over 1/2 the dimensions are missing. Since yesterday afternoon I've been working on putting all the dims back into the drawing. I did get copies of Rev A & rev B in other workspaces just to see & yes, the dims are missing there also.

OK so yes, this is mostly a rant & I do not expect someone to tell me what the heck happened here, I just gotta re-create have the drawing. However I do have a question. No matter how many times I regenerate the models/assembly I get an error "Model is not regenerated" when I save. 9 times out of 10 saves, I get that error. What gives? Funny thing is there are no geometry changes at all yet I can regenerate over & over again.

As I said, this is mostly just a rant. I am not at all pleased with Creo 3.0 but I am really glad we waited for M100. The only reason we moved to 3.0 was because we had to migrate our Windchill server to 11 due to security issues. I really miss the days when a new release was a huge improvement. Or maybe I'm just becoming a curmudgeon.

Regards,

Joe S.

mender · ‎Sep 23, 2016

If the drawing retrieves with the dimensions shown in Creo 2, and missing in Creo 3, that's a serious problem, and I would request you file an SPR on it, so we can fix up the problem.

If 'something was done' with the drawing/model, and now dimensions are missing, the most obvious things to check would be:

1) Were the views oriented using geometry that wasn't stable, and this geometry has shifted, rotating the views? If so, best to orient views using rock-solid fundamental geometry (typically the three starting datums).

2) Are the dimensions erased, or merely blanked by layer? In particular, if you set a layer to isolated, then all other layers are implicitly ordered to be blanked.

3) Did you roll back changes to the solid model without rolling back the drawing as well? If, for example, you made a bunch of driven dimensions from drawing mode that live in the solid, then checked the solid+drawing into Windchill, and found the solid in conflict with someone else's changes, and discarded the drawing user's changes to the solid while keeping the drawing, the drawing will have an attempt to show dimensions that never existed. (Side note, you can use config 'create_drawing_dims_only yes' to avoid this, by making the dimensions live in the drawing. The only downside that I recall offhand is that you can't include them in an ordinate dimension chain alongside feature dimensions from the solid.) Or if you made a version part.prt.3 with some new features, showed their dims in the drawing draw.drw.3, then deleted the file part.prt.3 (but kept draw.drw.3) and made different new features, then you'll be in similar trouble.

If you aren't sure what happened, but would like any advice on what it might have been to avoid the problem in future, you can send in an SPR and I'll take a look.

View solution in original post

mender · ‎Sep 23, 2016

If the drawing retrieves with the dimensions shown in Creo 2, and missing in Creo 3, that's a serious problem, and I would request you file an SPR on it, so we can fix up the problem.

If 'something was done' with the drawing/model, and now dimensions are missing, the most obvious things to check would be:

1) Were the views oriented using geometry that wasn't stable, and this geometry has shifted, rotating the views? If so, best to orient views using rock-solid fundamental geometry (typically the three starting datums).

2) Are the dimensions erased, or merely blanked by layer? In particular, if you set a layer to isolated, then all other layers are implicitly ordered to be blanked.

3) Did you roll back changes to the solid model without rolling back the drawing as well? If, for example, you made a bunch of driven dimensions from drawing mode that live in the solid, then checked the solid+drawing into Windchill, and found the solid in conflict with someone else's changes, and discarded the drawing user's changes to the solid while keeping the drawing, the drawing will have an attempt to show dimensions that never existed. (Side note, you can use config 'create_drawing_dims_only yes' to avoid this, by making the dimensions live in the drawing. The only downside that I recall offhand is that you can't include them in an ordinate dimension chain alongside feature dimensions from the solid.) Or if you made a version part.prt.3 with some new features, showed their dims in the drawing draw.drw.3, then deleted the file part.prt.3 (but kept draw.drw.3) and made different new features, then you'll be in similar trouble.

If you aren't sure what happened, but would like any advice on what it might have been to avoid the problem in future, you can send in an SPR and I'll take a look.

habdul · ‎Sep 23, 2016

Joe,

Of course I don't know all the details so I'll make general comments.

When PTC releases a new version, that's usually accompanied by adding/removing/replacing config options. I'd ask your CAD admin to investigate what have changed in config.pro options. There may be something that has to be reset to bring things to normal.

As for regenerating the model, maybe there's external referencing to models that are not in session and they are not retrieved automatically. Options like the following (and more) may affect retrieval of external refs

retrieve_data_sharing_ref_parts

regenerate_read_only_objects

retrieve_merge_ref_parts

mender · ‎Sep 23, 2016

Good thoughts on possibly external references. Config options should not (with certain exceptions, for example auto_drawing_update) affect retrieval stability.

Inoram · ‎Sep 23, 2016

When you first loaded it in CREO3 and saw stuff missing did you stop and try reloading it in creo2 to see if it was OK in 2? Just curious, I know this may be a hindsight thing, but it would show if it is a 3 vs 2 issue or something else.

jschutte · ‎Sep 23, 2016

Thanks everyone for your replies!!! All good stuff, unfortunately our Windchill server decided to have fits after some Microsoft patches. It seems to be working now but it blew my whole afternoon.

Come Monday I am planning on taking the time to try some things & answer all questions.

Thanks again,

-joe

jschutte · ‎Sep 26, 2016

OK so this morning I did a lot more investigation of the problem of the dims falling off the drawing.

"I the drawing retrieves with the dimensions shown in Creo 2, and missing in Creo 3..." When I got a copy of Rev B, the dims were missing. Why they fell off, I do not know but for all I know they were checked-in & released like that. I got a "proper" copy of Rev A being sure that all the parts were all rev A, not an easy task in Windchill (quite easy in Intralink 3.4) & all the dims were present. On Friday I do not think I got all the rev A parts in my workspace so it showed the missing dims.

No, "nothing was done", I had just got the copy of the drawing (& it's supporting prts) in my workspace, upped the rev level from B to C, then checked it out. However, I have no way of knowing the condition of the drawing when it was checked in. So this turns out to be a non-issue for now.

Thanks everyone for your replies. It appears I jumped the gun on blaming it on Creo 3.0.

ptc-396954 · ‎Sep 12, 2018

Joe,

I have seen this is happening more often especially when related to multi-page prints and very old (Pro-E R2001) models. When they are used as a starting point for a new project in Creo 3.0.