For those of you who make multi-body sheet metal parts, convince me that this isn’t the sh****est method ever. Why do you do it? What advantages does it give you? What barriers does it remove?
And on the other side, does it cause any problems?
I ask because I’ve always avoided this method, I never saw an advantage other than avoiding assemblies, and “just because you can” sort of thing. It would be cool to learn something, and be proven wrong, though. Enough people do it that I must be missing something.
We do many weldments that combine structural steel members with multiple sheetmetal bodies. It’s cumbersome trying to pull out details and flat patterns for each sheetmetal body.
To get flat patterns of each sheetmetal part, we have to create a config and delete/keep bodies to isolate that part.
This definitely isn’t the only way, or might not even be the best way to handle these weldments, but it’s the best way for us.
Because they added multibody to sheetmetal, you can now copy/mirror bodies. I haven’t ended with a multibody sheetmetal part, but I have had multiple bodies that I brought together later into one.
This is the way I would envision using MB sm if I used it at all.
I get it with Weldments, but I think I would make the sm as it’s own part and insert it into the Weldment. I don’t really do this kind of work, so I haven’t had to work through all the details. I was curious how you all do it.
I am using MB sheet metal approach , and even worse i am using save bodies to make assembly all the time (it just work for me , although i know other have issues and bugs with that)
I am using a lot of weldments , but even without it , i still prefer MB with sheet metal only.
It is easier for me to model it , i never found working with assemblies(with in context modeling) productive for me.
My workflow is to model everything as MB , save bodies (with make assembly option checked) , and than make separate drawings (until recently i converted all SM parts to SM again , but dpihlaja showed method with insert part and delete/keep bodies and it works even better )
I dont have problem with SM bodies and MB approach , and i prefer it because (for me) it is easier to make changes , rather than using assemblies in context modeling.
I use SW Weldments and if a weldment happens to be made from Sheet metal or has sheet metal…it’s still a weldment. Why someone would use multi-body parts for sheet metal that’s not a weldment I have no idea.
Advantages are all the advantages that you get with Weldments. Yes you avoid assemblies, which means a single part. I think the advantages of weldments for sheet metal are not as great as they are for plate weldments. But a guy has to have standards so if you’re going to use SW weldments for plates you should probably stick to SW weldments for everything.
I’ve not run into any significant issues. At one time properties didn’t carry over but that was fixed in SP5 2018
Not following this. If you’re using SW Weldments there aren’t “Different parts in there” it’s the same as a single part. So however you’d shift thru the features for a part you’d do the same in a weldment.
I suppose you could try to do it manually with folders, but you wouldn’t be able to always keep features for the same body together. You can expand the bodies folder and see features though.
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It’s imho the best way to deal with parts that are as one and are only split due to i.e. sheet sizes.
Example from my old workplace:
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The body sheets have holes in them (in this case only two, but sometimes they had bolt holes to mount a liner across the hole length) and due to different sheet sizes we started making configurations of one part - that quickly got out of hand and severely impacted performance. Additionally making correct configurations (sheet a,b,c,d,e,f,g,h for 120" sheet size or 96" sheet size or 240" sheet size or…) was really bad to do too. The performance-configuration horror was real.
Now mating across different sheet sizes is an additional horror if you don’t have a full-size part that is not split (we did it with an envelope which was another configuration).
Introducing multi-body sheet metal parts and the performance pain was gone. Changing parts becomes a breeze and you save yourself mating too. Reference geometry is easier to handle etc.
2019 severely increased the usability (bounding box).
I simply go thru the model and use the RMB Context menu option of “Export to DXF/DWG” on each sheetmetal & Boss Extrude Face I want to Laser-Cut.
This “manual” method can be a little arduous sometimes, dependent upon how many bodies are to be exported as dxf flat-patterns, but it also has the distinct benefit of ensuring there are no errors in the flattened output. (and this does happen sometimes, where SW doesn’t really pick up that a particular body won’t flatten, untill you try.. Only then it throws up an error.)
I would not like to manage that many configurations in one part file, if I had a couple/few dozen flat-patterns to export.
Configurations can be painful when editing a part.. Or perhaps I still have much to learn.. (This is likely the case tho, methinks.)
This is exactly the method I’d avoid. You can’t reuse any parts (without splitting them out), you can’t use library parts (without inserting them), configurations won’t work they way they are intended, drawings are harder, file management is impossible, mistakes are much easier to create, errors are harder to troubleshoot, motion is shot. You’re just avoiding an assembly, but limiting everything else and causing so much more work. You don’t like your nose, so cut it off and bleed to death.
For sheet metal, I can see using multibodies for really simple (one or two bend parts), within a weldment, but not for other stuff. It’s not any more work to use one part per file. Solid Edge actually uses an assembly for weldments (and individual parts for configurations). I think the main reason is just that it’s so much more stable, and you can keep individual file sizes lower. Plus, assemblies and individual parts are just a better way to organize and segment data. Segmenting data makes it easier to reuse, find later, make changes, make drawings, troubleshoot, and I’m convinced it keeps the software from crashing as much. It’s like using a swiss army knife to build a house - it can do some of the work, but it sucks at most of it.
When I have written best practices for companies, replacing normal assemblies with multibody parts is definitely on the “avoid it” list.
I’m convinced that the reason for so many crashes and other discontent with SW is that people are forcing the software to work the way they want it to work, rather than just learning the way it actually does work. There are times to step out of line, but I see this as an unforced error.
I was just asking because pretty much everything you can do in a regular part you can do in a multi-bodied part so I wasn’t sure what the person was doing to “Organize” a regular part that he couldn’t do with multi-bodied parts.
If we have a weldment that is really large we will drop things in folders, re-name features etc etc. We do the same thing with parts or assemblies.
I really don’t know how everyone else is doing this but we have templates for everything we do if it’s going to flame, lasered or water jetted. To get a flat pattern for a sheetmetal part in a weldment all you need to do is create a view, select body and plop it on the drawing. If you need a DXF of it you just export the drawing.
We avoid them as much as possible but there are instances where I believe that it’s much easier to have it as a multi-body part then as an assembly with individual parts. Of course, that way of thinking might come from the fact that I started off that way before learning about the master sketch method, but I still think that way for instances.
We use multibodies when we make the beams for our trailers, because they need to follow a specific shape. The same feat could be accomplished with an assembly, but it would most likely be more hassle. Depending on the length of the beams, we might need to add or remove joints for the beam and when that does happen, it is much easier to do it from a multi-body then it is to do it from an assembly. I added a picture to perhaps clarify what I was refering to “beam joints”
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(it just work for me , although i know other have issues and bugs with that)
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