Windchill Server Status

[KAM]

In the Windchill Server Status column of the model tree, I have two components that show an icon appearing as a red stop sign with a white exclamation mark in the center.  Hoovering over this icon gives the message: "Locked as Read Only Modified in Session".  I have not done any modifications to these components - so what does this mean?  What can be done to correct this?

[StephenW]

Lots of things can cause a part to "change". Do you have any relations that would calculate during a regen? Layer change in the top level that you used save status on that changes a parts layer. Top down design or external references. 

[KAM · Accepted solution]

I ended up unlocking the part, checking it out, regenerating, saving, and checking back in.  That seemed to fix it!

[StephenW]

Likely there is an underlying reason for the "change". I try not the check in items I didn't intend to change unless I can find a reason that I actually did make a change.

For something that worries me, I will check in the assy that uses the part (but not the part that showed modified). Then I will make a new workspace and add that assy to the new workspace and open the assy (or drawing or ??) and verify that everything looks like it should or if there is some discrepancy, I will research further to see what is going on.

Usually these things are benign (layer change/save), but occasonally, you might have inadvertently modified something in creo that doesn't get documented. You or the next user who uses that part may design around and not realize that there was a mistake.

[sacquarone]

Hello @KAM 

@StephenW  is right. It's very hard to provide guidance without knowing the excat use case (in other words, what were the steps leading at the end of the status being at the same time "Locked" and "Modified in session", or "Modified Locally" after save in workspace, WITHOUT HAVING FIRST DONE any manual action in the impacted component).

Just consider that, as a general rule (in the very large majority of situations reported to PTC TS), there is at the end a good explanation for this kind of use cases (and they are therefore usually not eligible to be reported as a SPR to our developers, most of the time). Some ideas come to my mind as follows, but for sure far from being exhaustive (without more knowledge on the background in your specific use case):

For the AUTOMATIC LOCKED Status (without any manual actions in workspace or in Creo Parametric in the impacted model): Most probable root cause is due to preference >Workspace > Add to Workspace and Check Out > Automatically Lock All Objects Added To Workspace set to Yes. Read article 76228 for further technical details. If set to yes:

• it is expected to have objects Automatically Locked in the workspace when being added in it
• They will be then automatically Unlocked if a manual Checkout is done (or if Unlock is manually done in the workspace)
• Purpose of this preference is to have a better control of what is supposed to be checked out (or not), for eligibility purpose of being iterated later on

For the AUTOMATIC MODIFIED STATUS (again without manual actions in workspace or in Creo Parametric in the impacted model): They usually come from actions triggered by External References or External Dependencies. You can have a look at them in Creo Parametric via Reference Viewer accessed from Model Tree in TOP Node of impacted object, and filtering Dependency tab or Reference tab filtered by Scope set to External. Some examples:

• Something changed in parent references, coming for instance from assembly containing this component AND affecting this component, like:
  • Layer Status changed + Save Status and Save for the assembly, with copy_submodel_layer_status set to yes in config.pro
  • Relation driving part parameter, based on assembly conditions
• Something changed in external dependencies, like, an External (or not) Inheritance Feature, or an External (or not) Merge Feature:
  • Whose Options tab is set to Automatic Update
  • With retrieve_data_sharing_ref_parts yes in config.pro
• Or maybe just models which were saved in an Unregenerated state, felt later as Modified after retrieval + simple regeneration

In any of above conditions described above, you may have in your workspace a component which becomes Locked and Modified at the same time (without being checked out then, and without having done any manual action in it). When you face this:

1. Try Manual Checkout of the component. If system allows you (no deny permission on Modify for CAD Documents), just Check it Out and Check it in
2. If Checkout is not granted (due to Released LifeCycle State for instance), you have no other choice to restore in session what was present in commonspace (losing therefore the modifications produced in the workspace, but it's expected to lose them in this situation where CAD Document is not supposed to be checked Out). If you need guidance in this direction, refer to article 44595 for steps to perform this action (Add to Workspace" again, now with Reuse content in target workspace unchecked)

Just to conclude now, I would be surprised to have guessed above the exact situation you're currently facing (again, because too many things in the system can lead into this final observations), but I hope this will give you at least some clearer idea of what happens behind the scene when this kind of situation occurs.

If all guidance provided here is still not enough, I suggest you to open a case to PTC Technical Support, and ideally describe the steps to reproduce the issue in your environment (starting from a state in Workspace WITHOUT any Locked/Modified objects, and leading at the end to a state where some objects become Locked and Modified at the same time, without having done any manual action in them)

Regards,

Serge