Why can I not get my assembly BOM to update with the custom properties changed at the part level? I change the description of a given part and it does not update on the BOM.
Are there configurations involved? If so, maybe there's a mismatch somewhere?
No configuration involved. I have even tried saving as a new part number. I deleted the BOM and re-inserted and the old part number still shows up.
Open the part file and check the property settings as shown in the attached file.
I've tried with no success. I have just started to have this problem since we upgraded to SW2018. Could this possibly be a bug in the software or maybe there is a check box somewhere that I need to check? This is occurring in multiple assembly drawings so it leads me to believe there is a setting somewhere that isn't right. Never had this issue with SW2017.
I'm having exactly this problem and it started after moving to 2018.
Some things I've noticed:
- Seems to only happen on parts that are being used by multiple assemblies (as if the other assemblies are locking out a change)
- If you go into the part and make a new configuration you can get it to update.
I'm having the same problem and see the same relations you are. Whenever I change a description I just make it a habit to delete the description column and recreate it.
I hope Solidworks addresses this soon.
Not sure if you have an answer yet but try this.
1. Go into the part file and select the configurations tab.
2. Right click on the configuration you're using and select properties.
3. You should see "Use in bill of materials". If that box is checked, whatever is typed in the field above is will show in your BOM.
4. Select the green check mark to accept the changes.
Hope this helps anyone out there that needs it.
Holy freakin jesus thank you. This was the issue. My company uses PDM, and I for the life of me could not figure out why our description custom property was getting overridden. I changed it in the data card, in the part, could not find out what was going on. I had to uncheck "use in bill of materials" then the custom property took effect.
Could you attach a simply ass/part/drawing I want to make some test on it....
Maybe you have a "Configuration Specific Property" set?
Dwight Livingston wrote: Maybe you have a "Configuration Specific Property" set?
Dwight Livingston wrote:
The Drawing has a different configuration. Keep all custom property information at the part or assembly level for an easier way to control the information. Having different information in the drawing file is asking for update issues..
Open part`s custom properties and close them after. Open the drawing and click on Update button.
use the solidworks bom and you should be able to update the part from the bill of material..
or did we loose that function.
I had the same issue and it took me a while to figure it out but this worked for me:
Click on the Custom Properties tab and at the bottom there is a button that says "More Properties". There you will get 3 tabs, "Summary", "Custom", and "Configuration Specific". In my case I deleted every line in the "Configuration Specific" tab. The "Custom" tab had all the properties I needed.
Hope this helps.
It's an old post but thought it could help to future users to post why my description cell in the drawing BOM wasn't updating. My parts have custom properties that I set myself with the Property Tab Builder. The cell "Title" (circled in green) was meant to be my "Description" (just called it "Title" at that time for whatever stupid reason). However, in the Custom Control Attributes (Circled in red), I had another attribute set. So I changed it to "Description" as shown in the screenshot and saved the file. My Description automatically showed up in the BOM right after that. Hope it helps!
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