I'm trying to get the part thickness to display in the BOM of an assembly. If I add the thickness in the properties of a part it will display in the BOM. Why do I have to add the thickness property to the part when it is known by the part? I understand having to add the material to the part since it is not known. But thickness is known in a sheet metal part.
If I understand correctly, this procedure is similar to what I was doing. It is a manual process for each part. Doesn't it appear that this (the thickness) should be automatically inserted since it is a known value? Material type is an unknown variable and needs to be manually entered. The sheet metal thickness is known from the Base Flange/Tab. The sheet metal thickness should be automatially passed to the assembly, just like part name and qty.
I hadn't considered sheet metal thickness as being essential BOM information on par with Quantity and part number. I mean from a simple standpoint of compiling the BOM, you can't get a meaningful list without being able to group components under a common identifier, so there has to be some piece of data in the part file to use for that. But I can have two parts with the same sheet thickness and they'll still be separate items in the BOM. For my part, when I'm doing a BOM for an assembly, I'm not really concerned with whether a part is sheet metal or molded plastic. I just want them to go together correctly and for the assembler to use the one's I've specified. I'm not looking to do part nesting or stock ordering or take-offs from an assembly BOM.
It sounds like what you're describing is more of a cut-list than a BOM. You might look into that functionality.
In any case, you can submit an enhancment request through the customer portal.
you can also add it to either the part template, or your property tab. either takes little more work than adding it to a single part file, and will add it to either all new parts (part template) or to any part you edit (property tab).
Thank you.
Sorry for starting over in this old topic.
I can add the values manual to each part this works. (also for template)
But for all my old drawings i want to use the property tab builder.
Wich value has to be in 'Value': "Thickness@????????????????.SLDPRT" obviously doesn't work.
Thanks in advance!
You need to setup a Property Tab Builder file and pick the one you want if you have multiple files as shown below...
And you need to have the custom property $PRPSHEET:"Thickness@????????????????.SLDPRT" in your drawing template
I thinks you don't understand me right...
I have allready a custom property tab builder active.
I got alot of old .sldprt files without the thicness value.
So i wan't to add with help of the custom property tab builder add the custom property 'thickness value'.
I wan't to add the value of the custom property to my BOM.
To add the custom property to the part files use Task Scheduler and pick an entire folder - type in the custom property you want to add to the parts. Then all the parts in the folder will have the custom property "Thickness" added then use that same custom property and add it to a New column in your BOM, don't forget to do a save as for your BOM template..
You can pre-select all sheetmetal parts in the assembly and then copy & paste the following into the relevant field on your property tab builder.
Code: "Thickness@part.SLDPRT"
This will resolve for each part file as long as the part is a sheetmetal. I can see from your snap shot that you have several property tab template files. The problem is that if your pre selected parts don't have the same property tab file name then you can't use this approach since you get the following issue (see image below). Don't ask me what they were thinking when they implemented this limitation. Then you will have to resort to Task manager or batch macros (can be found in this forum).
Thanks Elmar! It seems to work, because when i Apply the tab builder then it will display the value of thickness. (zie red marked area 2nd picture.
Only in my BOM it doesn't read out the value it only displays: " "
(in my tab builder is set the property for all configurations)
You know why this is?
+
You need to save all files. Do a full rebuild of the assembly and save it. Also, you need to select the property that relates to "Plaatdikte"
in your BOM and it will show up unless you have another configuration specific property of the same name that is empty. Solidworks will always choose config props over custom props.
Not sure what did it but it is working now!
Only with none sheet metal parts i get: "Thickness@part.SLDPRT" as text in my BOM Because the value don't change.
Can it display empty on the BOM?
Not going to work. The part needs to have a thickness defined under global values which is the case for all sheetmetals.
It will show the syntax as evaluated result if it can't find "thickness". Go to "advanced select" and filter out sheetmetal parts only.
That's one way to make sure you only select sheetmetal parts.
James, I'm aassuming you either want to include the material thickness in the part description or you want to have a seperate thickness property for a column in your BOM. This is pretty straight-forward. Once you've created your base-flange, Solidworks adds a thickenss global variable to the part which you can use to link to your custom properties. You don't have to physically select the thickness dimension to do this.
That generates the code shown in the screen capture.
To include the thickness in your description, with the property window open, pick in your description where you want the measurement to appear, double-click the base-flange feature in your tree to display the dimensions and then click on the thickness dimension. It's usually blue with a red link symbol.
Here's what the result looks like:
You can add that code to the custom properties of a template and it will auto-populate.
Now, just a note, you can have multiple sheet metal bodies within a part and the thickness property also applies to thin features, so in that respect, it's not always cut and dry what the thickness is.