How can I remove symbol is reserved or exists already

[ptc-5172728]

I want rename a dimension to A for my family table, in dimension proporties but that symbol is reserved or exits already.

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[TomD.inPDX]

Take a look in your part (and sub) parameters and see if A was assigned to something that is no longer in use. If it is no longer in use, you should be able to delete it with the box next to the in the lower left corner of the dialog.

[Dale_Rosema]

Or if you having trouble deleting it. Rename it to something else that will not conflict so that you can use the "A".

[ptc-5172728]

Antonius, thank you. I am new with creo-2, I looked in my prt and I have no A in the part file. I did rename the parameter from A to Shield_A Dia, now I need to change it back to A.

Dale I tried to rename to "A", ERROR INVAILD SYMBOL, thank you

[TomD.inPDX]

If you can attached the file(s), we can have a look.

[ptc-5172728]

sorry i can't the project I am working is sensitive, is there any way you can walk me though?

[TomD.inPDX]

Understood. Obviously there is a conflict. Something else appear to have the same name at the same level.

Make a note somewhere (model annotation) and make the - &A - and see what it returns. If it returns a value or something else recognizable, now you know where to look. If it comes back with an error, we'll move onto the next step.

I'm still wondering if "A" was accidentally defined but not used anywhere. Which means it can be deleted... but you have to find it 1st

[dgschaefer]

To find it, I'd try a few things.

Open your parameters dialog (tools tab > parameters), sort by name and se if there's a parameter named A. You cannot rename a parameter, unfortunately, but you should be able to delete it and replace it with another. If it's used in relations or in your PDM system that gets more difficult.

Second, to find a dimension use the find tool (also on the Tools tab). In the 'Look For' and 'Look By' boxes select 'All Dimensions' and on the 'Attributes' tab select name and put 'A' in the 'Value' box. Click 'Find now' and if it's a named dimension, it should pop up in the results window. You can rename it. Click the >> button to add it to the selection window and close the find tool. It should remain selected. Right click on it and hold, select properties and you can rename it at the top of that dialog. If it's used in relations (tools tab > relations), they should update automatically but I'd look before and after to be sure.

[ptc-5008082]

Or use Tools > Relations and use the icon to 'Show a specific dimension in the current model" (looks like a create dimension icon in sketcher) that will then show you the dimension on the screen in symbolic state.

Do bear in mind, this will NOT show you dimensions of a suppressed feature, but even if the feature IS suppressed you will not be able to rename any dimensions to names that are used already.

So make sure you don't have any suppressed features.

[TomD.inPDX]

Charlotte Halstead wrote:

Or use Tools > Relations and use the icon to 'Show a specific dimension in the current model" (looks like a create dimension icon in sketcher) that will then show you the dimension on the screen in symbolic state.

...

I did not know that