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I'm losing stuff, general drawing mayhem

tham

New member
Here's the situation. We are working without people outside of our company to get our detailing done. We send them the assemblies, they send us back the assemblies plus the new drawings. sounds like a plan right? something's not working.



When we open the drawing from the directory they send us, it is fine.



If I move the drawing and assembly (not the reference files) to our directory (because I don't want to overright some things spread all over our directories), I'm losing arrows and balloons, and some of the views are moved around, dims missing, general mayhem.



Is Pro-E not smart enough to pick up the references from models of possibly different versions?



Why am I losing all of this? I'm going to post this in the admin section of this forum because I'm really not sure where it should go.



Thanks for your help
 

proed

Moderator
If the part versions are different, there may be other ids for surfaces, etc - if the model has changed... The drawing may have references to items/features that don't exist in the new version of the model.

For example - in an assy drawing - BOM balloons may disappear if the components are located differently.
 

ProFishent

New member
Proed is correct about the surface ID's, there are other issues as well. It is bad practice to have more than one person working with the same files at the same time! When detailing a drawing you show dimensions, sometimes changing number of digets and tolerances. This requires you to sve the part file. For this reason you should not work on models when you have sent them to be detailed. When you get the details back you should also use the same models.
 

tham

New member
Thanks guys, but I really don't think we are changing the files. And note I'm talking about assemblies here.



When I recieve the drawing file back, I copy it back to the original directory. I've tried just copying the drawing and also copying the drawing and assembly file, in both cases, trouble ensues.



I can usually do this with model drawings with very little trouble. Assemblies are giving me fits.



Thanks for the input
 

bhayden

New member
Todd,



You could look at how the drawing details are created with the file set they return for some clues. For example, if they created datums for dimensioning that reference part geometry you would lose them with what you are doing. Some general best practice principles like referencing surfaces rather than edges or vertices might help in some instances.



Have you tried running model check to see what changed between the models you gave them and the models you got back? You could also use this to see what changes you've made between the version sent out for detail vs. the current version.



It might make sense for the contract drafting firm to only do a general drawing layout (main views, notes, etc.) and then send the whole package back for a clean-up pass when you've ready to release.



You might request the the contractors try setting the part file status to read only before detailing. However, I doubt that would be a very workable solution.



Bernie Hayden

XKL LLC
 

rocknroll

New member
We run into this problem occasionally too. Usually its caused by having an instance of the assembly in the directory you're moving the file to with a higher rev level than the file the other company is sending you. Pro/E uses this extension, rather than the date/time stamp to determine wchich file is the newest and will think the older file is more recent and will open the drawing from that model. Change the number extension on the assembly (assembly.asm.xxx - where the xxx's are the number extension - if you use win2k, you may have to set your folder options to show hidden file extensions) so that it's higher than any of the existing assemblies in that directory.
 

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