Error I Cannot Fix - Need help

[swood]

I have an error in my model. The error showed up while creating some tubing using the Piping application. I worked on trouble shooting it, couldn't figure it out. I deleted everything related, and couldn't figure it out. Unfortunately I worked on too many things to undo checkout and completely roll back to the previous version. I have completely deleted everything that was could have been related to the error. Attached is a screenshot of the error. The text is "ERR: internal datum 9713 of feat 9777 is missing". Neither this datum or feature exist anymore, but I cannot get rid of the error on regeneration.

This model is going to be copied to create 4 other units, and these are the North American standard units... so I want them to be clean and free of errors (even more than I usually would.)

I have removed all Model References that were possible, all unnecessary features, and tried to make the model as "light" as possible. None of this has helped.

Does anyone know something else I can try?

[dschenken]

If the feature didn't exist then the error should not exist. Either that or there is an internal error in the model data and that will require PTC to repair.

The find command should be able to find Feature 9777 using the feature number.

[swood]

Thank you for the reply. The find tool does not find the feature (unless I'm screwing something up.)

I'll contact PTC and see what they can do. If anyone else has ideas, I would still appreciate them.

[MartinHanak]

Hi,

use ID option instead of Number option when searching.

MH

[creodential]

Try this config.pro option and have another look at the Reference Viewer afterwards.

The missing components/references should be marked with a dashed/dotted red line which can be deleted with right mouse click.

When I had this problem, I had to delete them twice w/ saving/regenerating.

not_placed_comp_should_be_shown yes

HTH

P.S. Only works for Creo 2.0 M130 and higher.

[swood]

I fixed my search and it finds the item, but it still doesn't show in the Model Tree (with no filters). I cannot figure out how to do anything with it.

We are running Creo 2.0 M170, so I changed the config setting (had to do in text file as option wasn't visible when searching for it).

Restarted Creo and option still doesn't show.

Reference Viewer only finds this.

This was unrelated, but I managed to fix it.

Still getting error and cannot find F18(Sketch_13).

[StephenW]

Can you upload the models? Error messages are notoriously vague.

[MartinHanak]

Hi,

please can you publish picture of Model Tree related to saaicm200715.asm ? Display Feature # column. I would like to see whether feature number 18 is visible in Model Tree.

MH

[swood]

[MartinHanak]

Hi,

feature number 18 is missing in model tree. I guess it is suppressed. Please modify model tree configuration - enable displaying suppressed features.

MH

[swood]

Yes, it is missing in the tree. No, it is not suppressed. I cannot modify my tree to show it, because to the best of my knowledge, it does not exist any more.

[MartinHanak]

Hi,

suggestions what to check in assembly:

1. look into Info > Model
2. look into Pro/PROGRAM

MH

[swood]

Feature 18 is a Datum Point that no longer exists. Sketch 13 no longer exists. Feature IDs 9772, 9777, and 9778 no longer exist either.

I'm not sure how to fix something that doesn't exist, or how the heck Creo can think there is still an issue with it.

Thank you for the suggestions. This is all good info, and hopefully it points someone to a way of fixing it, cause I have no idea.

[MartinHanak]

Hi,

it looks like Feature #18 (Datum point) has parent = Feature #17 (Sketch 13). What information do you see when you double-click Sketch 13 link ? Can you display information for Feature #17 (similar to Feature #18 report) ?

I guess that Feature #17 (Sketch 13) has parent = Feature #16. What feature is a parent of Feature #16 ?

MH

[swood]

Items 16, 17, and 18 do not exist. Item 16 does not list any parent information.

[MartinHanak]

Hi,

so ... Feature #16 is not real feature, it is Group header (for example Feature #9 is Group header, too). I have no idea, what destroyed this Group header. If you can send your data to PTC Support and your company has active Global Support, then I suggest you to ask PTC Support to repair your data.

MH

[swood]

This is has been looked into by PTC. Apparently they see whatever the issue is (I haven't been given any details), but apparently we have to upgrade our Creo version to fix it. This is an issue because we I believe we are on the highest version we can go without updating our Windchill version (which of course costs a lot of money that wasn't budgetted for this year.)

I'll keep this post updated as I learn more.

[sthangaraj]

Hello Swood, Now I'm also facing similar issue. Exactly like yours. If you found any solutions kindly share.

[swood · Accepted solution]

Yes, I did get feedback and forgot to update this thread.

(video is below, I typed out the steps before realizing I could post the video)

Open your part/assembly with issues.

Ctrl+F to search for the issue. Search by Name, and (the important part I didn't know before) switch to the HISTORY tab. Type your feature number into the Value field and select FIND NOW.

Your feature should show in the box to the left. It will not highlight anywhere in your model because it doesn't exist any more. Use the >> arrows to move it to the right side (which selects it). Now select Close to close the dialog box. Do no click anywhere else! Move your cursor over an open area in your model window and right-click. Select delete. This will most likely bring up a window saying it will delete highlighted features. If it does, select the Options button select all objects shown and change them to Suspend.

Another strange aspect of this...  you are still going to get the same error FOR NOW. If you search again for the same feature you will also still be able to see it. Save the model, close it, and Delete Not Displayed. Reopen the model and everything should be okay.

If this works, please mark it as the Solution so everyone else will know. This worked for me on two different assemblies. Also let me know if you have any more questions.

Unable to play video. Please try again later.

[swood]

Video doesn't seem to be embedding, so I'm trying to attach it to this post.

[ptc-4543048]

Great solution Swood after an hour of trying to get rid of this error in my model I found this thread and it solved my issue.

Nick

[STEVEG]

@swood 

Since you solved the issue can you select the appropriate post as the acception solution?

[creodential]

I can't even find a saaicm200715.asm in that reference view.

I'd expect a more detailed chain of the involved component in text form, just like your very first image, but with the dependencies similar to the pic of the reference viewer. Knowing all these components would be helpful to narrow it down.