How to delete parameters from Notebook files (ex Layout)?

[IvanGasparini]

Dear users,

I am very new of PTC Creo (in the past I used other CADs) but actually I am using Creo 3.0 M050.

I am designing an assembly with the Top/down technique: the components and sub-assemblies are driven by parameters defined in a Notebook file (in Creo 3.0 it is still called Layout file).

Obviously, during the work, I did some tests and now my Notebook file presents obsolete parameters.

These parameters are no longer used in any part file, but I can not delete them (in the Tools ------> Parameters menù of the Notebook file).

If I try to delete a parameter that is used in a part (called for instance "xxx") of the main assembly, I get a message that that parameter refers to part xxx (rightly!).

If I try to delete an "old" parameter, the message reports that this parameter refers to the Notebook file and so I can delete it; but this does not seem logical to me, because it is a redundancy.

How can I then delete the parameters defined in a Notebook file? Obviously, not being used in any relationship, I could also keep them, but I would like to have a clean and tidy file!

Thank you so much for the help,
IG

[tbraxton]

Without seeing the files it is hard to say exactly what the problem may be. I suspect it is due to a dependency driven by a declared parameter in the layout. When you declare the notebook to a model then that model is then a child of the layout. If you undeclare the layout in each part referencing it that may let you delete the parameters. You may need to undeclare multiple or all of the parts driven by the layout to delete the parameters. You can declare the layout again for each model after you delete the unwanted parameters.

If this does not work I would need more information (post some of the files) to figure it out.

[IvanGasparini]

Dear @tbraxton ,

thank you for your reply.

I had already tried your hint and it does not work undeclaring the part where the old parameter was used.

I would not like not to undeclare all the parts of the assembly and then declare them again with the notebook; there are so many components!

Unfortunately, I cannot upload the assembly here because it is confidential. However, I attacched a very simple assembly in which the same problem is present: the side of the two parallelepipeds was initially defined with the parameter "A" and then a new parameter "C" was created to replace "A". Also in this case, it is not possible to delete the parameter "A".

Thank you for your feedback.

Best regards,

[tbraxton]

It is related to the fact that you have a table in the layout that has this parameter as an entry in a cell.

Try this, I did it in Creo 4 and it worked.

Open the layout

Delete the top row of the table (containing the parameter A)

Open the parameter tools and delete A

Save the layout

[IvanGasparini]

I apologize for the late reply but I got back to the office only today.

Your suggested solution also works in Creo 3, but only for the simple example that I reported here.

In the assembly that interests me, even deleting all the tables and all the sketches that I have in the layout file, I cannot delete the undesirable parameter.

Trying to open the Parameters menu in the layout file -----> View ------> Where used ------>a window shows that this parameter is used as a "Note" (see picture).

But I have no notes in my layout!

[tbraxton]

You will need to figure out where that note is and delete it or at least remove the reference to the parameter in question. Are you sure that the search results you posted are constrained to the context of the layout only? That is the first thing I would verify to insure I am looking in the relevant file for the note. The term block note would suggest to me that it is used in a title block if I am translating the term correctly. Is there a format in the layout file? If so try deleting the format.

Without access to the data it is difficult to speculate about how to approach this.

[IvanGasparini · Accepted solution]

l solved in this way:

1) I created a new file notebook in the folder of the assemblies, parts etc;

2) I copied and pasted from the old layout, respectively, all parameters and all relations in the new notebook. At this point the parameters become "free" and can be deleted.

3) The new notebook should then be renamed to the same name as the old one (which must be removed, before deleting it permanently I moved it to a support folder and I checked that the parts/assemblies declared when opened retrieve in session the new layout).

It is not the optimal solution, but in this way you can get a final layout file without the parameters of the deleted parts.

Alternatively, if you have Windchill you can use it to solve this problem (but I do not have the license).

[PI_6131154]

Creo 8: New Layout, Create parameter... not possibile to delete it any more. Program error? 

[IvanGasparini]

Sorry @PI_6131154, I have never used Creo 8 so I cannot help you. I suggest you open a new thread referring to this one (maybe with a direct link) and explain that the solution which I found for Creo 3.0 does not work with version 8.0.