Weldment part number in SolidWorks

When I have commercial parts that become components of a welded structure (like weld nuts, welded hinges, or even thread inserts) I insert them using the INSERT PART function. That way those bodies show up on the Weldment Cut List, and you can edit their properties to say whatever you want. Click INSERT / PART. The command gives you options on component material and properties and allows you to use mates to locate it properly.

I treat the part as a part number, the part with the nutsert as an assy part number. It can be done using configurations also.

Chris, CSWP
SolidWorks
ctophers home

Jboggs, thanks.

ctopher, can you explain what do you mean by "the part with the nutsert as an assy part number"? So basically if you have the weldment part+nutsert, then you treat is as an assembly?

I would cut the hole in the weldment, but not add the nutsert in the weldment part. I would make an assembly and bring in the weldment and the nutsert.

You can add properties to the weldment that would allow you to add a part number to the weldment groups. But the weldment would be seen as one complete part and that a way when you put it into an assembly you have but one part number. I have attached an image of the process I would follow.

Hope this helps,

Scott Baugh, CSWP
Mechanical Engineer
Ciholas

"If it's not broke, Don't fix it!"

Click to expand...

faq731-376

Yes, part with nutsert = assy

Chris, CSWP
SolidWorks
ctophers home

Hi, HungryDinosaur:

It depends on complexity of the part. If it is a simple part, I would model it as a part containing two separate parts.

Best regards,

Alex

Thanks Jassco, ctopher and Scott.

OP you asked one question and you got a few answers to different questions. One is how to assign a part number. Two is how to model such a case in CAD.

The part-numbering question really hinges on how your org handles things and at what level of scope you and/or your company works. For me, for example, I design weldments and then a separate company makes the weldment. So, to me, the whole weldment including any permanent attachment like a weld nut, PEM/clinching nut, etc. I consider it and number it as if it's a single part with no subcomponents. I can do this because I never need to buy the sub-pieces individually, so why give them a part number? I can call it out in the drawing and that's all I need to do. I do not assign the weldment a bill of materials.
On the other hand, let's say you're the fab shop in this scenario and you're making the weldment. The fab shop cares about each piece even though the thing going out the door is just a part to me, it's an assembly to them, and they need to buy or make each piece and keep track of it through the fab process. So in that case it would be proper for them to consider and part-number the weldment more like an assembly. This would also be true if you fab the weldment in-house. In both these cases your organization has a need to keep track of the individual pieces that make up the weldment so it would/should get a bill of materials.

In terms of modeling, I've done the "Insert Part" route and I do not like it. Insert Part creates separate bodies for each instance of the inserted component which reduces the efficiency measures in Solidworks such as lightweight/large assembly mode. Positions of bodies inserted into parts are limited to using Move/Copy which is conditionally useful but very far from having pull assembly-mate capability. Finally, I often create a pseudo-BOM in my drawing where I want to call out the nutserts or whatever, and modeling everything into a sldprt file forces you into using a Cut List which is still a lot less flexible than a Solidworks BOM although it's much better than it used to be.

I would model the weldment as a sldprt to use the weldment modeling tools, then I would put that into an sldasm so that I could add the purchased components and use Mates and patterns like any other assembly. I would set the sldasm to Hide all subcomponents via right-click on configuration>>Properties menu which will cause Solidworks to treat the sldasm like a sldprt on higher-level BOMs. Best of all worlds.