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Is there a way to delete, or edit the configuration name to not display the <as welded> or <as machined> descriptor in the BOM?
Categories: Modeling and Assemblies, Configurations∕Design Tables
Good afternoon Mike,
Could you give us a sample part or an example? I would think it has to be user input,
You can double click in the cell and just edit the cell to
show what you want it to say.
Right now to avoid this little nuisance, we use the "User Specified Name" in the BOM option of the configuration. This will let you type in a number and show up correctly on the BOM.
Also, direct editing of the BOM cell breaks the link to the part for that field and I believe in general to be bad practice. This also for us in the past has created a lot of headaches in a large development environment when you have a lot of different engineers or drafters sharing data. If the BOM is wrong then the part is wrong. This is what I teach my drafters. You don’t fudge your BOM to make it look right, fix the part or assembly so it reports right. If you don’t get the part the way you want it and reporting to the BOM correctly, then you will keep having to continuously fight with this setting every time you go to use the weldment/part or assembly in another assembly and call it out on a different BOM.
See also this post:
QTY. vs QTY
Here's the exact article, It deletes the <As Machined> and <As Welded> suffixes.
Hope it helps.
Here is the answer:
2016 SOLIDWORKS Help - Disabling Automatic Creation of Derived Weldment Configurations
As Aleksandr said:
if you have SW2016 you could do this:
Try the attached macro:
Preconditions: A part is open.
Postconditions:1. Turn off option: Assign configuration Description strings.2. Turn off option: Create derived configurations options.3. Delete any <As Welded> configurations.4. Remove <As Machined> from remaining configuration names.
Or just use the document name. Takes the typo problem out since it is linked directly to the part.
This does nothing to my existing weldment parts though. "Configuration Name" still has <As Machined> after my configuration name.
This one worked well. THANKS :-D
If you just disable the "Create Derived Configurations" and then add a new configuration (without changing anything), this works and is simpler, to me, than running a macro (no offense Cuinn).
Then, if you go to your part template and make the same changes, it will come up right from then on.
I just happened to come across your post as I was researching an answer to the same thing...and I tried Wojciech's solution and it worked.
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