Refer attached jpg
Is it possible to control the "Part number displayed when used in a bill of materials:" using a Custom property?
Sorry if this has been asked many times before - I did a search but can't seem to find an answer.
No option to do that. Don't know if a macro can fix that i.e. macro will get the value of the property and add/modify the Bill of Materials Options - "Part number displayed when used in BOM".
See attached file for an example SW2009.
Thanks for your efforts here.
I should have stated I was aware you can change this via a design table, you can also change it by inserting a BOM into the part and double-clicking the partnumber field. But you can't drive it directly via a custom property.
The client I’ve been contracting to for the last month use this function in SolidWorks to store their part numbers. They also store the same information in a configuration specific custom property, which is just plain nuts in my opinion. However I’m stuck with it and have to enter this information twice, which is frustrating and prone to error, but I guess I’ll have to live with it.
It's some what impractable to have a design table in a part that only has one configuration.
Sometime ago 8+ years I remember bumping into this same problem, at that point I simply decided not to use this function at all and just have a configuration specific custom property called partnumber or IDnumber and use that to define the part or assembly number.
Another SW mystery. I never had need to use this in a single configuration manner as you describe.
Very odd that it has to be defined within a DT to fill this slot.
I can enter it as a CP, but then it becomes $PRP@$PARTNUMBER. In the DT I can set $PARTNUMBER = $PRP@$PARTNUMBER and have the CP drive the Confgiuration Name.
Thanks for pointing this out.
accessing that particular piece of information has been on my wish list ever since I started using Solidworks (98plus).
What is your reason, or your clients, for wanting to store the information as a custom property?
For me, I found that I using standard Solidworks functionality that variable (PARTNUMBER) cant be accessed, it is only available in the BOM.
I needed to access the partnumber in a note on the drawing (client standard notes) but I also wanted to be able to see the partnumber in the tree.
I could have named the configuration the part number but at the time the partnumber was not allocated. So I've ended up with the partnumber entered twice which as you say is 'nuts'.
I've tried to use the property tab builder to link the note but I don't see away of doing it.
My only recourse was to submit an ER at each release.
I ran into the same exact problem, and I found a simple workaround without any APIs. In Configuration Properties, select “User Specified Name”, and type $PRP:”PartNo” (it should match whatever name you are using for your part number custom property – “Part Number, “PartNumber”, “Number”, “PartNo”, etc.). This will link your Custom Property to the BOM’s “PART NUMBER”, which is a property of a DIFFERENT type that we don’t have access to.
Obviously, if you have multiple configurations and a Design Table, just use the $PARTNUMBER column. You can make it equal to the $PRP@PartNo column in the Design Table. This way you’ll be able to link to your part numbers in drawings and title blocks as $PRPSHEET:”PartNo”. Because apparently there is no way to link to $PARTNUMBER in drawings.
If this worked and saved you a week of silly data entry work, LIKE it and send me a box of cookies.
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