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Datum Axis Naming Problem

Buster

New member
I am having a problem creating a datum axis. When creating the datum axis I keep getting the error "Name alreeady exists". At one time there was a datum axis "C", that was attached to the axis of a hole. That hole has been deleted and now I have to create a new datum axis "C".


I have made several attempts to locate the datum with no luck. I have checked everything I can think of to fix this problem. None of my colleagues can seem to find the problem either.


Any ideas?
 
You may have some GTOL attached, some other feature that references datum C. As long as the other references are there, datum C did not get deleted. To check this create a new GTOL and see if you can select C as one of the references. If you can, then it is still there.


The one way that I know of to find where "C" is, is to try and delete features from the model tree. Save your file first!!! Proe will not delete a feature that has a datum attached if other features reference it in GTOL. You will see a note on the prompt line something like "cannot delete features with GTOL".
 
Thanks for the reply. I tried your suggestion and it must be there somewhere, but it will not show up. I can not delete the feature that at one time held datum C. Is there a way to list all datums in a model or drawing, in order to possibly track down where this datum may be?


I did not create this model, it is a revision of a previous model and associated drawing. I have been asked to create the drawing, and the person that created the model is out of town.


Thanks for your help.
 
prouser1,


I appreciate your help, but it is proprietary information, and I would get fired for posting or sending you the model. I know it is almost impossible to diagnose without seeing it. I guess what I am asking, is there a way to find this datum, whether it is by going into the model program or whatever?


It is as if the datum does not exist, unless I try to use the same name on another datum.


By the way I am using Wildfire 2.0
 
If you used an axis of a feature, the feature was probably named "C". Ifa createdaxis was related to a feature and a gtol was related to the axis, Pro will not allow you to delete the feature. You must delete the gtol first. If you do an "Info>Model>Screen" you should be able to see a feature named "C". I have inadvertantly named a feature wrong. Is one of your part features named "C"?
Edited by: donha
 
I ran into this problem not too long ago and the problem is probably with the part file itself. If there are no other datums with that name and all gtols referencing the datum are gone then there is little you can do. I called PTC about this same situation and they indicated the only way to correct the problem was to go into the part file and correct it. If you 'can' send them the file they would look at it but if you cant...too bad...use another name. The partfiles used to be in english and you could go into it and possibly fix the problem yourself. Now the file is coded or compressed and there is little that can be done. I asked if pro toolkit users had that informationsince writing some applications require reading and or manipulating the part file (example-Modelcheck and all it can do). I didnt get a good answer to that so I gave up.
 
Thanks for all of your help. I think I will have to use another name by the looks of things. The person that is in charge of this project and the one who actually created the model will be in today, so we'll have to see what he thinks we should do with it. If we some how come up with a solution, I will post it for everyone.


Thanks again everybody.
 
I faced similar problem with not only axis but also datum.As APPINMI mentioned in his mail, it is definitely due to GTOL.It might happen as below mentioned:
Previously an Axis is made as Datum for GTOL and renamed as C.Later If you try to create an axis with name C, you cann't.And more over you cann't see which axis is C.
The only way you can fix this issue is:
Go to Edit-Setup-Gtol-Clear-Pick all axes in the model one by one.Then you can find C, somewhere.Rename it with diff. name. Then you can create Datum axis with name C.
 
OMG!! You have no idea how much you just saved my sanity! I joined specifically to THANK YOU!

I've recently started with a new company and they use Creo. I've been using Solidworks since 2004 and UG since 2011 and I find Creo soooooo frustrating!
 
Resurrecting this old thread because it comes up in google for this still-current problem with annotations in Creo. To find a NAME you can't find:
File>Prepare>Model Properties>Names: select, then Remove.

This was very helpful. Thank you!

I would also like to add that I had this same problem and I traced the source of the preexisting datum to the fact that my model reference a Merge/Inheritance as the first feature (as in, it is a final machine part which is cut from another rough machine model). The rough machine model had a Datum Axis 'A', and that is the reason why the final machine model would not allow a Datum 'A' to be created. I'm not sure why this problem exists, because in defining the Merge/Inheritance feature, I made sure the option to copy datums was deselected.

Regardless, brouch's trick to delete the name worked, as long as I didn't do anything to cause the Merge/Inheritance to refresh its references before I named my new Datum 'A'.
 

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