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IDF import: .asm in zip or subfolder?

mikehoopes
7-Bedrock

IDF import: .asm in zip or subfolder?

I have generally tried to convert assemblies to parts via Shrinkwrap for the purpose of IDF import. However, in some cases, I cannot get a shrinkwrapped assembly to include all of the necessary features, and quite often the shrinkwrapped file size is many times greater than the sum of the original parts, regardless of the number of repetitions in the assembly.

 

I also don't want to dump all of the files in those assemblies into the flat structure that contains all of the ECAD parts. I want to keep the assemblies in subfolders or zip archives.

 

However, Creo Parametric cannot locate my .asm files in zip archives or subfolders. Is there an option that will enable this?

1 ACCEPTED SOLUTION

Accepted Solutions

I doubt you will find PTC Creo references on managing libraries, that is why they sell Windchill. It sounds like you need some sort of data management tool deployed.

 

Libraries outside of Windchill for Creo are just directories in the absence of any other tools to manage the data.

========================================
Involute Development, LLC
Consulting Engineers
Specialists in Creo Parametric

View solution in original post

8 REPLIES 8

Ecad hint map files support the use of libraries for component models (ECAD symbols and ME 3D models). You have to plan the library and populate it but if you use ECAD/MCAD exchange with IDF it is well worth it. All organizations I have seen using this are large and have librarians dedicated but there are low cost library services available now if you can not support this internally. Library maintenance is a must but the ROI is quickly realized if you use ECAD/MCAD exchange often.

 

One nice thing about the library is that you can store all 3D models set to read only with all datums hidden which will prevent annoying regen of 1000 component ECAD assemblies when working with them in Creo. Should you need to manipulate the features you can always clear the read only status.

========================================
Involute Development, LLC
Consulting Engineers
Specialists in Creo Parametric

Thanks for the quick post. I have used hint maps in the past, and am willing to do so again if it enables my intent. However, I have 1:1 correspondence with footprint/model names, so the hint map hasn't been necessary. This includes my .asm files; if import the IDF with my assemblies in session, they pull in, no problem.

 

Creo just cannot find them if they are in not the exact folder specified in my search_path configs. Is there a way to get search_path to support subfolders of those paths, or zip files contained in the paths? Or is there a way to *easily* reconfigure those assemblies so that the .asm goes in the search_path folder, and references the rest of its parts in the subfolders?

 

[edit]: By libraries, are you talking about Windchill libraries? Is that supported in PDM Essentials?

Addendum: I moved my .asm files out of the subfolders, then reopened the assemblies, executed "Retrieve Missing Component", then saved. However, when I re-open the assembly file in a new Creo session, including IDF import, it has lost track of the child parts, and I have to retrieve them again, every time.

 

Is there a way to configure an assembly so that it looks in a given subfolder for its children? Can this be done retroactively, or did I have to make the assembly that way in the first place? The latter will not work, in most cases, where I am converting a STEP into a Creo assembly.

A library could be in Windchill but it does not have to be. You could have a library and manage it with search paths.

 

To answer your question directly, Creo search paths are not recursive and will not query zip files to my knowledge. If you want to use search paths to handle this situation, it is possible. You can create a search.pro file with all of the directories you would need.

 

You can use a command shell in Windows to semi automate the creation of the directory paths for you and then create the search.pro file.

 

In a windows command shell try the following from the top level of the directory that you wish to index. i.e. if you want to list all directories under the C drive then navigate to C: in the cmd shell and then execute the following command.

 

The below command will create a file listing.txt with all the directories below the start location.

 

dir /s /on /b /a:d > listing.txt

 

I would advise creating project specific search.pro files and load them as needed as the wait to load files can become a bottleneck if the search paths are numerous.

========================================
Involute Development, LLC
Consulting Engineers
Specialists in Creo Parametric

Yes, I want the library functionality, where parts in common have unique instances in the library. I'm not in favor of project-bespoken parts, or having disparate copies of parts in the system. Unfortunately, the Creo users I've encountered at my current company all cut their teeth on Interlink/Windchill, and when they came to our cost-constrained-PDM-free company, they flailed. I'm TRYING to establish a library structure there - right now we have rogue file copies everywhere.

 

I'm not a fan of maintaining a running .pro folder list that has to updated every time I bring in an ECAD part assembly. Most of those ECAD assemblies are STEP assembly imports, and I'm not in favor of dumping all of those disparate, non-PLM-managed child parts into the same bucket as my controlled, released parts. Thus, ECAD-part-dedicated subfolders or archives seem appropriate to me, since Creo has not seen fit to create a single-file asm, the way SolidWorks has.

 

I don't have Windchill deployed, and just can't find any references to Creo libraries except in Windchill documentation. Could you help me find that?

I doubt you will find PTC Creo references on managing libraries, that is why they sell Windchill. It sounds like you need some sort of data management tool deployed.

 

Libraries outside of Windchill for Creo are just directories in the absence of any other tools to manage the data.

========================================
Involute Development, LLC
Consulting Engineers
Specialists in Creo Parametric

Thanks for the help. If I figure out a way to automate the ongoing generation of the search.pro file (just a listing of the subfolders in my ECAD folder), I'll post it here. Hopefully, PDM Essentials (the one we're willing to pay for) can help wrangle this stuff for us in the future.

Here's a previous discussion of a similar situation. I've written a DOS batch utility that builds a search.pro file by traversing a directory structure - it's referenced in one of the responses.

 

Search path discussion 

 

 

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