Drawing dimensions disappearing

[Jgetrum]

I am working on a drawing that I hadn't touched for a couple of months, and when I opened it up today I found that most of my dimensions had vanished.

Pro E wildfire 5, 64 bit.

Assemblies have no dimensions anymore, parent parts have no dimensions, but the family instances have their dimensions still for the most part. Since I had not been on this model for a few months I have no backups from before this happened. And I don't really want to have to redo the dimensions on 40 pages of drawings again.

I did find a few references to the "save_display" setting that seem to have fixed this in wildfire 4, but that doesn't do anything in 5 apparently.

If anyone knows a quick fix for this I'd appreciate it. Otherwise I expect to be on the phone with ptc support all afternoon, and probably at work till midnight trying to get this fixed.

ETA: This is actually the second time we have had this happen in my office. Another user had the same thing happen, but fortunately he caught it the same morning and was able to restore from the earlier file.


Edited by: Jgetrum

 

[dr_gallup]

Created or shown dimensions?

Created dimensions can be lost if they are saved with the models and you have a different group making the models than making the drawings. To prevent that you need to save created dimensions with the drawing instead of the model. Then they just turn purple.

Shown dimensions will always be there unless feature sections are redefined and the old dims deleted. This can be prevented by using replace instead of delete during the redefine.

 

[Jgetrum]

These were all dimensions created in the drawing, as I find it quicker to snap a dimension to the points bits on the drawing than to try to sort through every dimension that was used to create the part to find the few I need.

I am used to dimensions turning purple when I screw with the features that they are on. But I hadn't seen them disappear wholesale before.

As I thought, Tech Support wasn't helpful. If I had caught this the day that it happened, instead of two months after, I could have actually had something that showed a problem, but it's rather hard to show anything when you just have part views with snap lines around them left.

If only this model wasn't over a gig already, then I'd have room to not have to purge all the backup files it creates.

 

[dross]

Have you tried show/erase to see if they are just erased?

 

[survey]

I've hada similarproblem about 4 times in the last 6 years. It always happened when I was renaming parts. All the drawing file instances in the folder were corrupted. I backup my files everyday,so I could grab the same instance off my server and all the dimensions would be there. I breifly pursued it with PTC, but there was not much they could tell me. Not that their support was bad, I justdidn't put too much effort intoit since it doesn't happen that often.

 

[Jgetrum]

This may have happened after I renamed a bunch of parts.

I spent a few hours and put all my dimensions back on, so that drawing is fixed. I guess I'll just be more paranoid about what I'm doing and not delete my backups until I know I've opened the model again to check.

 

[Jgetrum]

Had it happen again, but this time I hadn't been cleaning my directory for a month out of paranoia.

I tracked it down to a specific part in the model.

For some reason when the most current version of this one part is in the directory, all my dimensions in the drawing disappear.

Remove that part again, and reopen everything and the dimensions are back, as long as the drawing hadn't been saved.

I had not edited the part the day this happened, I hadn't actually even changed any parts, I was just reformatting drawing pages when I noticed that all my dimensions had disappeared again. So when I saved the drawing, a new version of a part was saved, which then removes all dimensions from the drawing it is in.

So as advice for anyone hat has this happen, you have to go and remove recently changed models, and test opening the drawing, over and over and over, until you find the part that corrupted your drawing. If only my assemblies and drawings weren't so monstrous in size, then I might not run as high a risk of this random corruption.

Anyways, the entire thing is off to PTC tech support, with the bad model that when dropped into the directory causes the dimensions to disappear. Nice to have the problem demonstrably repeatable. Now if only they fix the problem so that this doesn't happen to me any more.

 

[Jgetrum]

Just one more thing:

In my experimentation to find the source of the problem, I first had gone through removing the most recent version of the drawing to try to find one which still had dimensions. This does not work, the corrupted part removes the dimensions on the drawing when it is opened, so no matter how far you go back, as long as the drawing includes this part, you are not going to get your dimensions back.

You have to first remove the part that is causing the problem, and then you can open a drawing and have dimensions again. But if the drawing was saved after the dimensions disappeared, then you are also going to have to go back to a prior version of it as well. The strange thing was that all the thumbnail previews still showed dimensions that weren't there when the drawing was opened, but at least that makes it easier to know that the drawing had dimensions when it was last saved.

 

[jdurston]

Created or shown dimensions?

Created dimensions can be lost if they are saved with the models and you have a different group making the models than making the drawings. To prevent that you need to save created dimensions with the drawing instead of the model. Then they just turn purple.

Shown dimensions will always be there unless feature sections are redefined and the old dims deleted. This can be prevented by using replace instead of delete during the redefine.

How do you change the storage of created dimensions to the drawing instead of the model? I didn't know this was an option. I was going on the assumption that created dims were stored in the model (counter intuitive but I got used to it.) Is this a config setting? Please advise.

 

[Jgetrum]

Created or shown dimensions?

Created dimensions can be lost if they are saved with the models and you have a different group making the models than making the drawings. To prevent that you need to save created dimensions with the drawing instead of the model. Then they just turn purple.

Shown dimensions will always be there unless feature sections are redefined and the old dims deleted. This can be prevented by using replace instead of delete during the redefine.

How do you change the storage of created dimensions to the drawing instead of the model? I didn't know this was an option. I was going on the assumption that created dims were stored in the model (counter intuitive but I got used to it.) Is this a config setting? Please advise.

In your config file add:
create_drawing_dims_only
and set it to yes.

PTC tech support just told me to do this, but also says that it only takes effect when making a new drawing.

 

[dr_gallup]

Not just a new drawing, it cna be an old drawing but only newly created dimensions. There is no way to move created dims stored in the model to the drawing.