Modifications to models does not load on another PC

[yyang-3]

I have been having this issue on my office computers. Whenever I make changes to a model, save it onto the disk and when I load it up on another PC

the modifications made would not load, therefore one cannot carry on from another's work on a different computer.

The models have been saved in the same directory and the folder was copied and transferred onto the second PC.

Does anyone know the solution to this problem? Please give me detailed solution.

Thank you very much.

Yan Yang

[BenLoosli]

Are you clearing your Creo session of all parts before opening the copied file?

This is were a PDM system would save you the trouble as once checked in from user A, user B could then have the latest changes.

[yyang-3]

Hi Ben, thanks for your reply.

No, I have never cleared Creo session files before. Maybe this is the problem.

[pimm]

The downstream PC doesn't have an earlier version of Creo?

[StephenW]

You'll need to verify if you don't have duplicate models in different locations on the computers also.

[yyang-3]

Stephen, thanks for your suggestion.

No, I did not have the same models or duplicates on my computer before I transferred the files.

[Dale_Rosema]

Duplicate discussion:

modifications does not load when open model on another pc

Are you paying attention to the extension at the end of the part (i.e. part123.prt.37)?  If he has the same part on his computer and the extension is .52, it always loads the latest extension, so .52 would get loaded and not .37.

Thanks, Dale

[llie]

Yan,

Dale is completely correct. Also make sure that the other users do a erase not display.

Lance

[StephenW]

Yup, this one will get you every time if you are copying in to the same folder with existing models already present.

[yyang-3]

Hi Dale, thank you for the suggestion.

I had no idea about these part extension before, I will check these in detail. This could be our solution.

[Dale_Rosema]

There is a way to turn the extensions on. Here is a screen shot from my folder:

Thanks, Dale

[yyang-3]

thanks again Dale,

I have found the file version numbers but I need to confirm this is the cause of the problem.

I have also found a way (GrabCAD) to rename file versions to (.1) and tracks the latest version, which seems helpful.

Yan

[yyang-3]

Dale, now I have found out that the same problem happens on the same computer too, if the files were duplicated and moved into a new folder.

I have also tried a purge command to remove older versions of the file and it doesn't seem to work.

For example the labels and dimensions in a drawing only appears if it is opened in its original directory, if the files were moved to another directory, when opened the same annotations would be gone. Do you know why this happens?

Thanks

Yan

[Dale_Rosema]

Part of that depends on search paths in your config file. I am not sure if it search all of the paths to find the lasted iteration of the model or if it goes with the lasted iteration in the first directory it finds the model.

You may need to set a working directory to drive it to the one on which you need to work.

[dgschaefer]

If we are talking about drawings, then you need to move / copy both the drawing file and the part or assy file that goes with the drawing. 

When dimensions are created in a drawing, the dimensions are stored in the part or assy file not the drawing file.  If you create a bunch of dimensions on a drawing while another person is making changes to the part or assy, the drawing dimensions will be lost when the new part or assy file is put with the new drawing file.

There is a config option to change this behavior - create-drawing_dims_only yes.  The downside is that it limits how you can embed model dims & drawing dims in notes or other dimensions.

A reliable way to move Creo files is by opening them in Creo and using the backup command.  This copies the file and brings all parent files along with it to the new location.