Pack and Go (packing designs)

[Sean2]

Hello,

I am a new user to Creo Parametric having come from inventor.

Inventor used a function called pack and go which took and assembly and all its referenced parts and documents and saved them to a new location, it maintained all links.

Is there a similar function in Creo 4.0/5.0?

Thanks,

Sean

[BenLoosli]

Nothing like Pack & Go with Creo.

Your best option is to do a save-as to a clean folder. If you make that folder your working folder and then open your assembly from that new folder, it should find all of the components.

[MartinHanak]

Hi,

maybe Save a Backup is the right command.

[dgschaefer · Accepted solution]

Martin's correct, Save As > Backup will save almost everything needed to the target location.

A couple of things to keep in mind with the backup command in Creo:

1. The newly saved model becomes the active model, much like a "save as" in MS word works.  So, you'll want to save your assy, then do a save as >: back up to the new folder, then close Creo and re-open the original.
2. Some external references are not saved.  For external copy geometry features, they will be if the source part is in memory, but others won't.  Make sure you look for those.

Lastly, Creo itself doesn't keep track of links. Windchill does, but Creo itself does not. It only looks for needed parts in very specific places in a certain order.  First in memory, then in the folder the parent came from, then the current working directory and lastly any defined search paths.  If it can't find it then, it gives up and asks you to find it.  Save as > back up should put all of the needed parts in the target folder, so everything should be found.

[KenFarley]

Another feature of the save as backup is if you have parts that are used by lots of designers, like a library family table model of cap screws or some other hardware, it puts a copy of that family table part into the directory you are saving to. This can be problematic if someone later opens up the backed up assembly, since these "common" components are no longer the ones from the library, but from the copied file. If changes are made to the library part to comply with new requirements or to fix an error, the changes will not be reflected in your backed up assembly.

[dgschaefer]

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@KenFarley wrote:

Another feature of the save as backup is if you have parts that are used by lots of designers, like a library family table model of cap screws or some other hardware, it puts a copy of that family table part into the directory you are saving to. This can be problematic if someone later opens up the backed up assembly, since these "common" components are no longer the ones from the library, but from the copied file. If changes are made to the library part to comply with new requirements or to fix an error, the changes will not be reflected in your backed up assembly.

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Absolutely, this is an issue.  One way around this is to start Creo in such a way that it has no access to the library parts.  For us, that means temporarily commenting the line that pints to the search path file. Then launch Creo and open the assy. Creo won't be able to find the library parts, so when you do a Save As > Backup they won't be put into the target folder.

[rohit_rajan]

saving a backup of assembly does the backup of parts and assembly file not the drawing of parts.

[BenLoosli]

That is correct. If you want the drawings, you need to open them and do the Save - Backup on the drawing file, not the part or assembly.

Lower level drawings of components in an assembly need to be backed up individually, just like the assembly.

It is a PITA, but works and gets your files backed up.

We had a project that was not in Windchill and that is how we made the archive copies. Each component and assembly in a separate folder with a copy of the drawing in PDF format.