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.
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.
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.
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.
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.
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?
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.
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.