Hello
I get an error message that is displayed when updating the part family on solidworks 2019:
the column header "$PROPRIETE@N001_ARTICLE_CODE" contains an invalid function name "N001_CODE_ARTICLE"
N001_CODE_ARTICLE being a custom property of my document
I'd like to make sure that I can move a value back into my custom property based on the room configuration (using the room family)
Thank you for your help
Hello;
Remove your "invalid" column in Excel. (Room Family Edition in new window).
Close Excel.
In a configuration of your component: Enter a new value for your "N001_CODE_ARTICLE" property (specific to that configuration).
In another configuration of your component: Enter any "xxxx" value for your "N001_CODE_ARTICLE" property (specific to this configuration).
Edit your room family again in a new window, taking care to select the property to be seen in Excel: "N001_CODE_ARTICLE".
Edit the cells in this property to your liking in Excel.
Close Excel.
There you go.
Kind regards.
Thank you for these explanations, but unfortunately I can't apply the method!
Is it possible to write a value in a property of the document and not in a property linked to a configuration from our part family (on Excel)?
The family of parts snt capricious, do not leave a column empty (L & M), then put a column (N) with a property otherwise it does not work.
In addition, you have to look in configuration-specific properties.
Hello.
No, all entries made from the part family are for each configuration.
I advise you to remove all " custom" properties, if they exist in the configurations.
(the best, in my opinion, would be to delete them all).
Please note: configuration-specific properties always take precedence over the document property (" Custom ").
Kind regards.
How does this property create in the configuration set?
When I add a property in a configuration, it is not present of all the others!
Can I keep the same property name for configuration and custom?
Thank you
As @sbadenis says so well (we really have to stop answering at the same time 
)
If you leave rows or columns blank, Solidworks doesn't take them into account.
For my part, everything is in custom, unless the property(s) that differ as description, article ref...
But the room family is supposed to handle that for you.
If you empty your property in the custom tab for properties related to the config, no risk of problem.
I have a different approach.
No "Custom" properties, everything is managed by the Excel table and the "Configuration Specific" properties. (dimensions, materials, properties, etc.)
This allows me to save all of my properties and dimensional data in a separate Excel workbook.
@Maclane for my part smartproperties create custom properties and for the configuration specific one then create the room family and config specific properties.
But the 2 methods have the same result in the end.
For @JungV for a simple screw I doubt that confidentiality is important attach your part if version 2020 or inf I would look otherwise maybe @maclane will take care of it.
But surely a character problem in a column that is swarming.
Too late @Maclane just read before you finish answering 
To attach the excel table also if possible or the file with all the config!
(If you have any doubts, first copy your entire table to another sheet of your workbook - Only sheet1 is taken into account by solidworks, the others can be used as backups).
Close Excel.
Rebuild all your configurations.
Edit the properties of a configuration (Any configuration):
In the tab: Configuration-specific
Manually add the " Variable " property names to be used in the part family. Assign them arbitrary values at the moment.
N001_CODE_ARTICLE
N001_PROVENANCE
…
Relaunch the edition of your part family.
You should get the following Pop-up:
choose " $PROPRIETE@N001_ARTICLE_CODE " and the other desired properties from the list again.
To be safe, always check the box " Show unselected objects again".
In Excel, the column $PROPRIETE@N001_CODE_ARTICLE should appear again.
Copy your values to the new columns.
Delete old columns (N001_Code_Article...)
To summarize:
Your Properties must exist in at least one configuration (Configuration Specific) before you can use them at the part family level.
Kind regards.
NB: I am on Solidworks 2022 I cannot send you the result in SLDPRT+EXCEL...
Thank you very much
It's perfect
