I've modelled a multibody sheet metal part an I now need to get a drawing with a cut list. how do I do this? there is no option to insert a cut list from insert tables.
Insert Weldment cut list.
I use the BOM for this. The welding cut list is for space frames made from angle or tube. The sheet metal pieces are not just standard parts.
Unfortunately I did this component as a multi body part and I dont think the BOM would work.
Have been faffing about making parts and assemblies to get what I want on the drawing and I don't think I'll use multi body parts again.
Creating separate parts seems so moch easier and more logical, the parts are created as they would be in real life one at a time and assembled as they would be in real life and the assembly gives a check of wether there are any discrepancies. And then you just create a BOM and it's done.
Deepak is correct. Insert a weldment cutlist. I do this exact thing everyday. I set up a table with custom columns of dim x, dim y and thickness as well. Then in the cutlist, I select the part add a custom property for each of these and select the dimension that shows the correct value.
Then I have cutlist for my multibody part. If you need an individual view of one of the components, use --insert---view---relative to model.
How do you send information to your sheet metal fabricator?
I insist on sending drawings. These have the tolerances I want achieved. Our fabricators routinely ask for the complete SolidWorks model, so that they can flatten it and work out their flat layouts. This is fine by me. Multi-bodies might pose a problem here.
I remember seeing posts here about showing cut list items in an indented BOM. I've never done it so I can't elaborate and I don't have time to look into it right now. It might be worth researching for your project, or someone else might be able to help.
I designed a welded steel tube structure, where I broke it down into flat bits that could be assembled on a table. Your indented BOM would have made sense on those drawings. I forget how I actually did it. I was working on a drafting board at the time.
In recent years I've always designed using multi-body parts, it's a great way to get everything to play nicely together. Once I'm ready to detail the model, ie, add fasteners, material specs etc, I save each part into a seperate file, create an assembly(sub assembly) of the part with the fasteners, then a main assembly. Insert all the sub-assemblies dirrectly in so that they re-align with the origin. No mating required. This creates a fully detailed assembly where every part is driven for the original multi-body part. The BOM, and subsequent part and assembly drawings are pretty straight forward from there.
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