why can’t Pro-E figure it out?

[michaelpaul]

Why can't pro-E do this?

You have a part.
you have that part in an assembly
you want to modify that part to try some things out but not alter the original so you make a copy of that part.
you then go to your assembly to replace the original version of the part with the newly created and named copy.
all assembly references now fail!

why? it's the same freaking part. as far as pro e is concerned all feature IDs should be the same. the only difference is the part name. why can't Pro-E figure out that if you used the datum TOP in the original part to mate with that you also want datum TOP in the new part as well?

it drives me nuts!

Michael

 

[dr_gallup]

Why don't you just open the assembly then rename your part in memory? It doesn't change the existing part on the disk and your assembly is happy as a clam.

 

[kdem]

For what you are trying to do I'm thinking you want to use an interchange assembly. When you copy and then try to replacethe originalwith the copy ProE is treating it as an unrelated component.

 

[dgs]

I think an interchange is overkill for what he wants. Sounds like he just wants to try some design variations.

There are a couple of easy ways to do what you want, just not the way you're doing it. Dr_gallup's method is one, here's another:

Open the assy, change your working directory to a new, empty folder, select file -> backup. now you have a copy of your assy and all components (all with the same name) in a separate folder.

Do what ever you want, and if it works, back up back into the original folder. If it doesn't work out, delete the new folder.

 

[kdem]

True, it may be overkill but there are those who will insist on using the replace functionality without having to respecify references which is what I took as the issue. And as far as I know the only way to do that is to have parts as part of a family table, interchange, or reference model. Just copying the part and trying to use replace you'll have to respecify the part references because ProE considers the parts two separate ones with no relationship to eachother.


Another option would be to backup as you say, Replace>By Copy, make your changes, rename the part if you like the changes.
Edited by: kdem

 

[dgs]

If you use the 'by layout' replace option (not to be confused with Pro|E layouts), Pro|E will usually figure out the assy refs if the two models are related. However, any later models assembled to it (children) will fail.

 

[JFLORES]

Hey Michael,


Not sure but I think Pro/E might be able to find the feature IDs if you invest the time (probably more trouble than its worth) to save a component interface at the time that you place the component. you would have to define a rule to seach for the ID. I do not define rules, but have gotten into the habit of setting interfaces while creating parts, so that if things go south (and you know they will)I only loose half the references.


I use the Doug's backup techniquealmost everyday and find it very effective, but latly thinking about looking into the replace functionality.


later Jim

 

[lfhunter1]

open the assembly and do a replace by copygive part a new name hit ok and every thing should be good. new part is in the assembly. want to go back to the old version either do a replace or depending on what PDM system you are using you can back up the frames.


lynne hunter


engineering manager


stefens enterprises

 

[kdem]

If you do try and go back to the original part after using replace by copy you will have to specify part references. Although if you don't like the changes you could go back to a previous state using the version files.

 

[Mindripper]

While it is possible tochange the filenamea part in an assembly by using 'Replace' with the 'Copy' option without losing existing alignments, it is NOT possible to do this with a subassembly within an assembly. There are other convoluted ways to do it, however. In any case though, it CANNOT simply replace one file with another without losing all of the alignments. I think this is what michaelpaul is commenting on. Like so many functions in Pro/E, there is a lack of consistency and logic here, plus limited functionality. Of course, every other CAD product on the planet can probably perform all of these simple everyday tasks with ease: I know SW can without blinking even once.


This is symptomatic of what has plagued Pro/E for many years: a corporate sense of complacency and arrogance towards the needs of their customers. They have consistently failed to bring meaniingful improvements to the functionality of their core product (Pro/E)while all of their competitors offer amuch more user-friendlyCAD product now. Pro/E appears to be the very last of the Unix-based CAD packages in the world. I wonder how long PTC will allow itself to fall father and farther behind the rest of the planet before they finally implode or get merged out of existence. Myself, I am definitely waiting for this day to come.

 

[dgs]

Mindripper - Do you have nothing better to do that come here and dig up 6 week stale threads and offer no new solutions to the problem, just anti-Pro|E rants (not based in fact) and pro SW propaganda?

first, he was offered some pretty simple solutions to his dilemma. Frankly, because Pro|E saves a new file each time, it's really a non-issue. Just keep working, trying whatever you want, saving as you go. Just don't purge. Need to go back? Just find the version that you like on disk (make sure there isn't another version in session), open that one and save. Ta-da, old version is now current.

As far as SW being able to do this sooooo easily, go ahead, give us the step by step on how you'd do that in SW. SW lacks a simple rename command, I doubt it's near as easy as you say.

 

[lfhunter1]

well said

 

[vitadj]

I hope that Mindripper get paid for doing this, over and over.

Pro/E is best package for doing assembly.

 

[Knut Fiskergård]

Who get paid from who is always something to consider as these discussions enter "ProE vs. any other cad system" mode. <?:namespace prefix = o ns = "urn:schemas-microsoft-comfficeffice" />


Is proE the best package for doing assembly? Really? In what context, what type of assembly, what do you need the assembly for? Is it just to put pieces together to make a drawing, in the worst drawing app offered

 

[kwyjibo100]

The Replace by Unrelated Component tool in Wildfire 4.0 will allow you to pick up some of the assembly references that are common between the original and new part. If you expland the Evaluation Rules you can see what it will automatically find, and datum planes are axes are included.


If you used model surfaces for you assembly constraints, you can just manually select the same surface in the new part to tag it and then the replacement will be made without any failures. Nice if you've changed the copied part and removed some geomtery that you might have used for assembly constraintes.


The tool has been updated in Wildfire 5.0 to also automtically pick up surfaces based on their ID. So if it isn exact copy, you simply click the Evaluate button and it will find all the same surfaces. You can try it in the C000 pre-production build that has been out since November last year.

 

[michael3130]

Doug,


In SW I'd rename parts in SolidWorks Explorer. I find it pretty effective. It will carry out a search to show where that part is used. I'm not sure if MichaelPaul is basing his rant on how easy it is to replace a part in SW compared to ProE....it is relatively easy and straight forward.


I'm not getting involved in the SW vs ProE rant though.

Just saying that's how I do it in SW. In ProE I do various ways that have been mentioned here.....I don't have any real gripes about it....maybe takes a bit of patience first few times but that's life and then it's easy enough.

 

[Mindripper]

I'm looking forward to the opportunity to work in WF4 (and WF5 when it's released). We are stuck on WF3 and Intra/Link 3.4 here, and will continue to be in this sorry state for at least another year due to corporate dictates. Hopefully this (and perhaps some other) basic functionality will be improved in later releases. And perhaps PTC will one day appreciate the concept of 'easy'.


I just had my system administrator recompile my Intra/Link 3.4 database again yesterday, as saving any Pro/E could take up to five minutes. This has to be done regularly: every six months or so. I have been told that if it isn't done with sufficient regularity or if the database file grows above about 1GB, the entire database on my computer will become corrupted without warning. This is scary.


Oh yeah: this is Rant and Rave, isn't it? I thought I had my radio tuned to the right channel.