Windchill: Opening an assembly from the commonspace causes it to be "modified" in the workspace

[INENG]

Just the act of opening an assembly within my workspace causes it to be modified. 

When I open it, it prompts me to check it out. After clicking "continue", it causes the assembly to show as being modified (blue "+" symbol). 

It also seems to arbitrarily choose other sub-assemblies within it that it prompts me to check out. These also show up as modified after choosing "continue." 

This happens on multiple different assemblies, not just one. And it doesn't always happen. 

Any idea why it would be doing this?

[BenLoosli]

1. This is not the right group for this discussion. Please be careful and select the proper category for your question.

2. Please state what version and build of software you are asking your question about. By placing it in this category, we don't even know if it is Creo!

3. Are these older files from a prior version of Creo? They will be modified when opened as the internal data structure of the file has changed. Changes in GD&T cause files opened in Creo4 and higher to have additional changes.

[INENG]

1. Is there a way to change the group/category? Or would I need to re-post the question?

2. Creo 4.0, M050

3. No, it is from the same version of Creo. In this particular instance, the files had been created by me and recently checked in. They became modified when I created a new workspace and opened them in there. 

[BenLoosli]

Topic has been moved.

Al files create din Creo4m050 should not do that if saved.

Are you using any external links in your files to other files? This will cause a regen and the modified flag.

Are the components in your assemblies fully constrained?

[INENG]

I assume by external links you mean circular references? No, there are none. 

If that isn't what you mean, is there a good way of checking that? i.e. what should I be looking for on the reference viewer?

All components are fully constrained. 

[BenLoosli]

Do you have any GD&T symbols in your assembly on components?

Do you use any special features, like a shrink-wrap or a flexible model?

[INENG]

No GD&T symbols and no special features. It does have weld features from the Creo "Welding" application.

[Tdaugherty]

Can you verify that the version you are retrieving from commonspace is fully regenerated? It sounds like you need to regenerate the models and check them back in.

If you select "continue", you will be allowed to make changes (such as regeneration) in your workspace. After saving, the changes caused by regeneration will cause the objects to be flagged as modified in the workspace.

I think that the "external links" comment was really referring to external references between components or features. They can add a layer of complication when it comes to fully regenerating models. 

[MikeLockwood]

 In general, opening any "parent object" (assembly, drawing) pulls the latest version of each related model.  Any of those could have changed.

If for example, an assembly includes a pin in a hole in a block and since the assembly was checked in, someone changed the block, and removed, the hole, then the assembly will fail and a dimension on the drawing showing how far the pin sticks out of the block will fail.

In general to troubleshoot, add to a new workspace As Stored (not Latest).  See which child objects (e.g. component models) have changed since the parent was checked in by observing the clock symbols in the workspace.

Open in CAD As Stored and verify how it was when checked in.

Then, incrementally use Workspace Update to bring the latest of each to the workspace and see what happened.

Also, it's possible that that data (esp. SolidWorks) was checked in, in a non-regenerated / rebuilt condition, or with missing references or circular references. Until regenerated, rebuilt, or the references fixed, this data will show as being changed on opening it.

Have to build into the release process a disciplined verification that none of these problems exist with the native CAD data.

[DmitryC]

I just want to add another possible reason to this list.

This also can happen if some of the metadata has changed since you last saved the CAD file. For example, its state could change -> Windchill pushed this change in attributes into CAD -> CAD thinks that the file was modified. This is especially true if you have any download delegate customizations.

In order to prevent this case from happening - use automatic locks when you add anything into your workspace.