I have a sheetmetal piece which has many external references for connector cutouts. The external references are based on the connector placement on the board in the assembly.
Anyway, if I open up the sheetmetal piece and don't manually retrieve the references, I can get issues when working on the parts - especially with REFERENCE patterns.
Is there an option to have ProE automatically retrieve references for external references, similar to retrieve_data_sharing_ref_parts for data sharing features like Copy Geometry and Merge?
You must not be using Windchill and you probably do not have search path statements... or even a managed library system.
Since I work in Pro|E on the fly for many clients, I try very hard to manage files without using external references, even sheet metal punches I create on the fly within the part (quilt forms).
It all comes down to the resources and understanding you have about how the system finds references. And then developing a policy and file management system to ensure trouble free operation commences.
There is no automation like this for regular reference (as you mentioned, it is there for data sharing features). When you have a part that has multiple external references by design it might be better that you open respective assembly, activate this component and work on it.
if you are on Windchill, checking out this part will also suggest bringing its reference assembly.
We do use Windchill 9.1. I don't see what this has to do with anything? Even if the items are in your workspace, ProE will not load them into session when the part is opened.
So what technique do you use? If you do model on-the-fly then you do have external references. If you break them, then you loose the whole point of the items updating properly if the referenced items move. If you don't break them then you run into the risk of ProE behaving all honky when the items are not in session.
Thanks for the comments. Unfortunately, many different people besides engineers use the models. For instance, the modelshop will open a part and use it to generate a prototype. For the situation that specifically caused me to generate this posts; the modelshop guy opened a sheetmetal items with many connector cutouts. He checked the K/Y factors and they were wrong. He updated them which caused a full regeneration. Since the external references were not in session ProE went loopy on the reference patterns for some of the LED cutouts and they disappeared. There weren't any popup error messages - just a few leds disappeared. Since there were many cutouts he didn't notice and spent hours making a prototype that didn't work. This is what we are trying to avoid.
I've spoken with PTC before about other issues with patterns not behaving well when the external references are not brought into session. Their basic response was to bring it into session... which doesn't really help. There are many times when users can't work all the time within the assembly; nor should they if they don't need to. If they made a cut using an external reference, that shouldn't lock them in to always working the part in the assembly for all time to come. It also limits others who need to access the part. This can also be an issue when we send the part to a vendor.. etc.
I see your point Joseph
Unfortunately, there is no miracle - if you use external references you might need these models for full blown regeneration. However, there are at leat 2 things that we can suggest to avoid full ref assembly retrieval :
1. Use geometry backups creating features with external references. Set Ref Control to "None" / "Backup forbiden references" before creating featrures with external references (no cure if the model is already created).. This will make model much more robust when it is regenerated stand alone.
But not in 100% cases - for e.g. Ref Pattern might still have problems.
2. Use Copygeom feature(s) at a start of your model. Copy all needed Geom into yuor part, and only use these Copygeom(s) creating lcoal features. They will clearly survive any full regeneration.
However - Copygeoms do not carry along pattern information either, so you will not be able to create Refpattern on it. You can add pattern Recognition feature on top of Copygeom though if yiu have Flex Modeling license.
Inability of geometry backups / copygeoms carry over pattern information is a known limitation, and any enhancement proposal in this area will be appressiated. We have it on a to do list, but customer call might strees the point further.
Vlad, thanks for your post. 2 Questions:
1) Do you want me to actually call in about the Copy Geometry feature not carrying over pattern info or just make a post on the enhancement forum?
2) Where do I set Ref Control to "None"/"Backup forbiden References"?
1) you are welcome to use any regular way you use for logging / promotion enhancement requests : through tech support, or even placing enhancement request on this forum. So that prioduct manager gets it on his list.
2) File / Options / Assembly / External References Control / Component Permitted == None ; "Use backups For Forbidden ... " = check.
I'm still in Creo Elemenets/Wildfire 5.0, so there is no File/Options for me. Are you talking about the regular options?
Oh, sorry - assumed Creo02 :-)
So you go Tools / Assembly Settings / Reference Control / Objects = None ; Backup = checked.