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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.

CarrieIves wrote: ↑Tue Aug 24, 2021 6:21 pm 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.

Thanks for the input.

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.

Lapuo wrote: ↑Wed Aug 25, 2021 9:02 am

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.

Just out of curiosity, how do you sort through the featuremanager with all of the features for different parts in there?

IndianaDave wrote: ↑Tue Aug 24, 2021 4:57 pm art, we have to create a config and delete/keep bodies to isolate that part.

If you're using SW weldments the configurations are created for you and the flat patterns are there. See the attached.

matt wrote: ↑Tue Aug 24, 2021 2:54 pm 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.

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

matt wrote: ↑Wed Aug 25, 2021 10:39 am Just out of curiosity, how do you sort through the featuremanager with all of the features for different parts in there?

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.

matt wrote: ↑Wed Aug 25, 2021 10:39 am Just out of curiosity, how do you sort through the featuremanager with all of the features for different parts in there?

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.

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: 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).

matt wrote: ↑Wed Aug 25, 2021 10:39 am Just out of curiosity, how do you sort through the featuremanager with all of the features for different parts in there?

Folders , comments , renaming features etc..

matt wrote: ↑Wed Aug 25, 2021 10:39 am Just out of curiosity, how do you sort through the featuremanager with all of the features for different parts in there?

It might not be the best way, but this is how I do it (this isn't a sheet metal part, but it is a multibody master part):

matt wrote: ↑Tue Aug 24, 2021 2:54 pm 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.

I'll just drop this here.. https://www.cadforum.net/viewtopic.php?p=4068#p4068
A post from a different thread pertaining to weldments, but it mostly covers my opinion on this too..

IndianaDave wrote: ↑Tue Aug 24, 2021 4:57 pm It's cumbersome trying to pull out details and flat patterns for each sheetmetal body.

I will agree with this to an extent.

IndianaDave wrote: ↑Tue Aug 24, 2021 4:57 pm To get flat patterns of each sheetmetal part, we have to create a config and delete/keep bodies to isolate that part.

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.)

dpihlaja wrote: ↑Thu Aug 26, 2021 7:19 am It might not be the best way, but this is how I do it (this isn't a sheet metal part, but it is a multibody master part):
image.png

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.

Lapuo wrote: ↑Thu Aug 26, 2021 1:38 am Folders , comments , renaming features etc..

You can do the same thing with the a multi-bodied part.

dpihlaja wrote: ↑Thu Aug 26, 2021 7:19 am It might not be the best way, but this is how I do it (this isn't a sheet metal part, but it is a multibody master part):
image.png

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.

Damo wrote: ↑Tue Aug 31, 2021 12:50 am 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.)

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.

matt wrote: ↑Tue Aug 24, 2021 2:54 pm 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 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"

I'm answering this from the standpoint of using multi-bodied parts for weldments. I'm not sure why you would use it for parts that are essentially assemblies.

matt wrote: ↑Tue Aug 31, 2021 9:11 am This is exactly the method I'd avoid. You can't reuse any parts (without splitting them out),

If you have parts that you want to "Re-Use" or use often you can make templates of them and insert them.

matt wrote: ↑Tue Aug 31, 2021 9:11 am you can't use library parts (without inserting them),

How are you getting library parts into assemblies etc without inserting them? Maybe I'm not understanding this one.

matt wrote: ↑Tue Aug 31, 2021 9:11 am configurations won't work they way they are intended,

Don't understand this one either. Configurations in weldments work the same way they do everywhere else.

matt wrote: ↑Tue Aug 31, 2021 9:11 am drawings are harder,

Not sure why. What is harder about making drawings from a multi bodied part versus an assembly or anything else?

matt wrote: ↑Tue Aug 31, 2021 9:11 am file management is impossible,

Don't understand this at all. You have one part.

matt wrote: ↑Tue Aug 31, 2021 9:11 am mistakes are much easier to create, errors are harder to troubleshoot

Again, not sure why that would be. Everything is in one file. Errors are easily seen and rectified.

matt wrote: ↑Tue Aug 31, 2021 9:11 am 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.

While you could do motion using multiple configurations, I'm really not sure why someone would use multi-body for an assembly....I mean it's an assembly not a multi-bodoed part.

matt wrote: ↑Tue Aug 31, 2021 9:11 am 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.

I don't really agree with this statement. You have a single part that is treated as a single part. Modeling it as a single part is easier from start to finish from modeling thru ERP thru manufacturing.

When I create a weldment all the properties are propagated via the weldment insertion. That keeps me from having to fill in nearly any custom properties which I would have to do individually for each part. I don't have to mate them. If I want to I can create multiple parts from a single sketch. This is extremely helpful for weldments that have many individual parts that run thru an entire cross section. See the pic below. One sketch, two extrudes and I have an entire base, done. All the parts have many of the custom properties we use automatically populated.

All the changes for the entire cross section are contained inside a single sketch. Change the sketch, everything else updates. No opening multiple parts, hunting down which mate locates the part etc.

matt wrote: ↑Tue Aug 31, 2021 9:11 am 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.

The vast majority of SW crashes I have happen in assemblies. In my opinion this is probably because of mates, rebuilds etc. Non of that exists in a multi-body part and I can honestly say I can't remember but a few occasions on some really funky weldments where I've had SW crash in a weldment.

As to replacing assemblies with multi-bodies, I agree, that doesn't make sense to me but if you're making a weldment using multi-bodied parts is, at least IMO, significantly superior to assemblies.

AlexLachance wrote: ↑Tue Aug 31, 2021 3:47 pm 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"

image.png

Yeah, I use multibodies for almost every project. Generally I make an overall shape that gets broken into multiple pieces, and it's very difficult to make nice shapes that are actually separate parts. And sometimes I use other parts for reference. But I never make multibodies just to avoid assemblies. Sometimes even things like captive screws, or pre-assembled purchased parts I'll do as multibodies.

This to me doesn't look like a weldment. It looks like an assembly of machined and purchased parts with features in folders.

MJuric wrote: ↑Tue Aug 31, 2021 3:51 pm
The vast majority of SW crashes I have happen in assemblies. In my opinion this is probably because of mates, rebuilds etc. Non of that exists in a multi-body part and I can honestly say I can't remember but a few occasions on some really funky weldments where I've had SW crash in a weldment.

As to replacing assemblies with multi-bodies, I agree, that doesn't make sense to me but if you're making a weldment using multi-bodied parts is, at least IMO, significantly superior to assemblies.

I feel I must agree with you on this one.
Most of the errors I get are from mates flipping, or suddenly thinking they are now over-defined, (where they were not previously, and most often I will simply delete them and recreate the same again and all is good..), or just plain breaking anyway. And sketch references losing there references across parts within assemblies. etc.. I can confidently work with some fairly large MB Parts (200-300 bodies) and run smoothly without crashing.

MJuric wrote: ↑Tue Aug 31, 2021 3:22 pm 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.

So, Export the DRW File as DXF..?! Scaled as 1 : 1 ..? That works..?
Many plates we cut would not fit on any size of paper for drawings sheet size..
Or am I missing something here..?

matt wrote: ↑Tue Aug 31, 2021 3:56 pm But I never make multibodies just to avoid assemblies.

This is sensible.. And neither would I. Assemblies definitely have their advantages..
And likewise, I would never create an assembly of single body parts just to avoid multibodies. Especially when multibody parts work soooo well.
And with a good cutlist template... Beautifully easy..

Your primary query being about sheetmetal multi-bodies applies too.. If I'm designing something that uses several, or many, folded plates all welded into one rigid form.. It'll be a mult-body part.. Everytime..

matt wrote: ↑Tue Aug 31, 2021 3:56 pm Yeah, I use multibodies for almost every project. Generally I make an overall shape that gets broken into multiple pieces, and it's very difficult to make nice shapes that are actually separate parts. And sometimes I use other parts for reference.

When you say, "that gets broken into multiple pieces" ... Do you mean "Save Bodies"..?
(I've seen someone do this and then take these saved bodies and "Convert to Sheetmetal" all over again..
That seemed odd to me, just to have separate bodies for individual drawings.)
There are many thing about this methodology I do not understand..

MJuric wrote: ↑Tue Aug 31, 2021 3:15 pm You can do the same thing with the a multi-bodied part.

That is what i said .... right??
I completely agree with your response to matt , and as i said i am far more efficient with multi-bodied parts than asssemblies.
My english sucks , so i believe i am getting misunderstood by others.

Damo wrote: ↑Wed Sep 01, 2021 2:10 am So, Export the DRW File as DXF..?! Scaled as 1 : 1 ..? That works..?
Many plates we cut would not fit on any size of paper for drawings sheet size..
Or am I missing something here..?

Yes, that works. I usually double check that the view is actually 1:1. Sometimes SW will change that when creating the view.

Are there limitations on the drawing sheet size? I guess if you are buying your sheet goods on a roll, this could be a problem. Otherwise I doubt you need a dxf larger than what SW can create. It had no problem with me setting my sheet size to 1000 in x 1000 in.

Damo wrote: ↑Wed Sep 01, 2021 2:10 am So, Export the DRW File as DXF..?! Scaled as 1 : 1 ..? That works..?
Many plates we cut would not fit on any size of paper for drawings sheet size..
Or am I missing something here..?

Yes, there is a setting in options, see below, that exports DXF's to a 1:1. You can then just import the geometry into whatever software you're using to cut the template. In some cases, depending on software, you may have to delete the border etc from the DXF or have it on a different layer you just turn off.

All depends on your process, equipment etc. All of our internal stuff is cut off the model so we don't do DXF. External stuff can be DXF, DWG, native whatever...

Damo wrote: ↑Wed Sep 01, 2021 2:24 am When you say, "that gets broken into multiple pieces" ... Do you mean "Save Bodies"..?
(I've seen someone do this and then take these saved bodies and "Convert to Sheetmetal" all over again..
That seemed odd to me, just to have separate bodies for individual drawings.)
There are many thing about this methodology I do not understand..

I'm not sure why anyone would "Save bodies", especially when you can create individual drawings from any multi-bodied part using the "Select body" option. I just think that many people doing this are unaware that you can do this with multi-bodied parts.

I have run into situations where a company has a software that cuts from the models and sometimes you have to break out the individual bodies for them. However, again, in many cases this is because people don't know how to use their nesting software.

I actually did this with our sister company. They were insisting they needed "One file One part" or their nesting software couldn't import the parts. I got a demo copy of their software, worked with the VAR and set up a filter for them that took a multi bodied part and imported all the flat patterns based on a particular configuration. This actually made it EASIER on them then having to import multiple different files.

Of course after doing all of this and showing them how to do it they stopped doing it because..."Well it's not what we used to do"....in other words it's something new that makes our job easier and would save everyone money....so we aren't doing it

MJuric wrote: ↑Wed Sep 01, 2021 8:55 am I'm not sure why anyone would "Save bodies", especially when you can create individual drawings from any multi-bodied part using the "Select body" option. I just think that many people doing this are unaware that you can do this with multi-bodied parts.

I have run into situations where a company has a software that cuts from the models and sometimes you have to break out the individual bodies for them. However, again, in many cases this is because people don't know how to use their nesting software.

I actually did this with our sister company. They were insisting they needed "One file One part" or their nesting software couldn't import the parts. I got a demo copy of their software, worked with the VAR and set up a filter for them that took a multi bodied part and imported all the flat patterns based on a particular configuration. This actually made it EASIER on them then having to import multiple different files.

Of course after doing all of this and showing them how to do it they stopped doing it because..."Well it's not what we used to do"....in other words it's something new that makes our job easier and would save everyone money....so we aren't doing it

There are numerous reasons why multibody parts aren't a good "end-in-themselves", and why a meat cleaver approach is needed to split them up:

-Cutlists have a very bad habit of resetting themselves and losing data. We have several part files that do this about every 2-3 weeks. Bringing linked values back means regenerating the cutlist which means losing all your custom properties. It. Is. A. Massive. PITA!

-SWX Detailed Cutlist BOMs are a torture chamber. (dissolve subassemblies and parts, combine identical components, attempt to reorder and sort bodies from different parts.....fails every time, beat head on desk)

-Title blocks don't work.

-Using different materials is doable, but fragile. It breaks if the body ID changes, which is DUMB.

-Revision management is difficult if not impossible (which body changed inside this part file anyway?)

-Part/document number schemes become convoluted with some numbers being in cutlist properties and some being in file properties.

-Alternate position views only display parts; there is no option for "Show Bodies".

matt wrote: ↑Tue Aug 31, 2021 4:10 pm

This to me doesn't look like a weldment. It looks like an assembly of machined and purchased parts with features in folders.

That is exactly what this is. It is my master part. Which is then split apart and re-assembled into an assembly.

If I ever need to modify anything, I just come into this part and modify it, then reopen the assembly and update it.

This is one of 7 master parts that I used for this project.

dpihlaja wrote: ↑Wed Sep 01, 2021 9:26 am That is exactly what this is. It is my master part. Which is then split apart and re-assembled into an assembly.

If I ever need to modify anything, I just come into this part and modify it, then reopen the assembly and update it.

This is one of 7 master parts that I used for this project.

Yeah, that's what I thought it was. Hope it works for you.

matt wrote: ↑Wed Sep 01, 2021 10:00 am Yeah, that's what I thought it was. Hope it works for you.

It did. The project is complete and the fixture is in the machine. Worked really well actually.
Granted, I spent some extra time splitting apart the master into the components to create the assembly. But I saved a lot of time making changes when/where I needed to and also saved time in the initial design stage.

But it works really well. I wouldn't do it on a small assembly, but a large one, definitely.

MJuric wrote: ↑Tue Aug 31, 2021 3:51 pm I'm answering this from the standpoint of using multi-bodied parts for weldments. I'm not sure why you would use it for parts that are essentially assemblies.

That's what the picture shows, right? an assembly being modeled as a part.

If you have parts that you want to "Re-Use" or use often you can make templates of them and insert them.

Why break in the back door when the front door is open?

How are you getting library parts into assemblies etc without inserting them? Maybe I'm not understanding this one.

You can't insert Toolbox library parts/hole wizard with all those advantages into a back door multibody assembly wannabe. You can't even do multiple instances of a single part in another part, they're all just separate bodies.

Don't understand this one either. Configurations in weldments work the same way they do everywhere else.

Yes, but you can't have a configured part inside another configured part unless the configured part is modeled as a separate part. Or you could but it would be an undecipherable rats nest.

Not sure why. What is harder about making drawings from a multi bodied part versus an assembly or anything else?

Additional steps for each body you do it for, can't access the drawing directly from the part, no association between the part number and the drawing, no provision for handling multiple instances of a single part, etc.

Don't understand this at all. You have one part.

you can't rev one part, you have to rev the whole mess, you can't reuse one part in another assembly without bringing links with it, there's just a slew of things you can't do

Again, not sure why that would be. Everything is in one file. Errors are easily seen and rectified.

if you've built features on features a failure of one part can cascade into all the parts. You must know stuff like this?

While you could do motion using multiple configurations, I'm really not sure why someone would use multi-body for an assembly....I mean it's an assembly not a multi-bodoed part.

???? Your whole argument is in favor of doing assemblies as multibodied parts.

I don't really agree with this statement. You have a single part that is treated as a single part. Modeling it as a single part is easier from start to finish from modeling thru ERP thru manufacturing.

Maybe you're leaving out a key piece of information here. You've got a set of parts being treated as a single part.

If this is just a purchased subassembly, then I could see making it this way, but I'd skip the multibodies and just make it a single body. If this is a concept that you haven't any idea how it's being manufactured then I could see modeling it this way until you figure it out, then this might be a usable workaround. But if these are parts your company designs and manufactures, then you're forcing it all through the back door when there's a big wide opening right up front. Simply avoiding an assembly doesn't give you any benefits. All I can think is that there is some key detail I didn't get, because it's just a string of bad ideas trying to force SW to be NX or Acad or something else. Your responsibility for the documentation goes beyond a printed piece of paper. The techniques you show are ok as a workaround when there is some extenuating circumstance, certainly not a go-to method for real production data where there are no barriers to using the software the way it's designed to be used. Unforced error. Personally I don't care what you do, but I really don't want some impressionable person to come here and say "Matt's site says you can save a lot of fuss by making assemblies as multibody parts". You can obviously do what you choose, but from a best practice point of view, from a training point of view, from a tech support point of view, from a demo point of view, this is a bad idea. It's only not a bad idea as a workaround for some issue other than "I don't like the way it was designed to work". Remember there are other people who are going to have to use this data after you.

I'm not against multibody modeling, I use it all the time. I'm not against master models, I use those all the time, but for me multibodies are almost always part of a method to get to a single body, or to carry a complex shape across several parts, or a mold die, or one of the established methods like weldments.

I started this thread specifically because I was curious and wanted to talk about sheet metal multibodies. It turns out that I'd still model the sheet metal separately and insert it into the weldment as a part, especially if it has a separate part number, as long as it isn't just made on the spot.

mike miller wrote: ↑Wed Sep 01, 2021 9:12 am There are numerous reasons why multibody parts aren't a good "end-in-themselves", and why a meat cleaver approach is needed to split them up:

-Cutlists have a very bad habit of resetting themselves and losing data. We have several part files that do this about every 2-3 weeks. Bringing linked values back means regenerating the cutlist which means losing all your custom properties. It. Is. A. Massive. PITA!

-SWX Detailed Cutlist BOMs are a torture chamber. (dissolve subassemblies and parts, combine identical components, attempt to reorder and sort bodies from different parts.....fails every time, beat head on desk)

-Title blocks don't work.

-Using different materials is doable, but fragile. It breaks if the body ID changes, which is DUMB.

-Revision management is difficult if not impossible (which body changed inside this part file anyway?)

-Part/document number schemes become convoluted with some numbers being in cutlist properties and some being in file properties.

-Alternate position views only display parts; there is no option for "Show Bodies".

As I've said a few times now I'm not sure why someone would use a multi-bodied part to do something that is more like an assembly. I don't use multi-bodied parts like that. I use multi-bodied parts for purchased parts that are single part numbers even though they are assemblies and may have motion and weldments.

I've used different materials in weldments and have never had a problem with it changing it back.

I do alternate position views all the time by using move body and configs. This is how I do all my purchased parts like Cylinders, ball screws etc etc.

Part numbering is easy and automatic for us as we use the file part name combined with the cut list number.

Again, sounds like some of what you're having problems with is due to trying to using multi-bodied parts as assemblies rather than multi-bodied parts. I never have issues with any of the things you mentioned but I also never dissolve multi-bodied parts and try to combine similar components. We use multi-bodied parts for weldments and on a weldment cut list you don't try to combine all the parts from multiple weldments into one. The cutlist is for that weldment. Combining similar parts is done at the ERP level not the cutlist for the weldment. If for some reason I had a part I used often inside of a weldment I would make it a library item and insert it. Then at the ERP level combine it. We do this every day with items like weld nuts etc.

I guess in this issue I agree with matt. Don't try and make the software do something it wasn't designed to do and you avoid a lot of problems. If the way you use multi-bodied parts doesn't match how SW had designed them to be used....don't do that.

I use them day in and day out and they tend to give me less of a hard time than most of the other things I use in SW.

matt wrote: ↑Wed Sep 01, 2021 11:13 am
I'm not against multibody modeling, I use it all the time. I'm not against master models, I use those all the time, but for me multibodies are almost always part of a method to get to a single body, or to carry a complex shape across several parts, or a mold die, or one of the established methods like weldments.

I started this thread specifically because I was curious and wanted to talk about sheet metal multibodies. It turns out that I'd still model the sheet metal separately and insert it into the weldment as a part, especially if it has a separate part number, as long as it isn't just made on the spot.

I think we are talking past each other here. As I have stated I do not know why someone would use multi-bodied parts rather than an assembly. We use them for weldments and purchased parts. We use them for purchased parts even if they are assembly because that assembly is a single part to us.

My response is to your "Sheet metal multibodies". If it's a weldment I use multi-body even if it's sheet metal. If it's not, I use an assembly.

Again we do this all the time. Enclosures are sheet metal assemblies because the parts are bolted or fastened together in some way other than welding. In this case each sheet metal part is processed seperatly and then "Assembled"....because it's an assembly.

If we have a structure that is going to be welded together then it's a multi-bodied weldment regardless of whether it's sheet metal etc. In that case the parts are "Pre-bent" and welded and that weldment is the part. All the individual pieces of that weldment are not "Parts" but merely raw material for that weldment. The pieces are no more "Parts" for us than a bar of 6" round CRS stock.

This however also means you have to process weldments like weldments and assemblies like assemblies. Our weldments have a cut list on that weldment, that individual part. Process weldments in this manner and you don't have any of the issues anyone in this thread is talking about. Try to process a weldment like an assembly and you will have all these issues.

MJuric wrote: ↑Wed Sep 01, 2021 11:45 am I think we are talking past each other here. As I have stated I do not know why someone would use multi-bodied parts rather than an assembly. We use them for weldments and purchased parts. We use them for purchased parts even if they are assembly because that assembly is a single part to us.
....

If we have a structure that is going to be welded together then it's a multi-bodied weldment regardless of whether it's sheet metal etc. In that case the parts are "Pre-bent" and welded and that weldment is the part. All the individual pieces of that weldment are not "Parts" but merely raw material for that weldment. The pieces are no more "Parts" for us than a bar of 6" round CRS stock.

Well then I'm confused about why we're arguing. Purchased assemblies, yeah, I'd do that as a single part.

The only exception I'd add to what you say about sheet metal in a weldment would be if you had a complex sheet metal part that is welded onto a frame. Like an enclosure with a lot of bends and other features. If it's just a couple of small bends on a bracket, then yeah, just make it multibody.

matt wrote: ↑Wed Sep 01, 2021 1:14 pm Well then I'm confused about why we're arguing. Purchased assemblies, yeah, I'd do that as a single part.

The only exception I'd add to what you say about sheet metal in a weldment would be if you had a complex sheet metal part that is welded onto a frame. Like an enclosure with a lot of bends and other features. If it's just a couple of small bends on a bracket, then yeah, just make it multibody.

That's what I'm arguing. I don't care about complexity I care about whether it's a weldment or not. If it's not a weldment, don't use multibody. If it is a weldment, use multi-body, lots of complex sheet metal parts or not.

I don't find one or the other "Harder" or "Easier" to do except how you process it down the line and specific tools available. I'm working on the cabinet below as a weldment. It's essentially two electrical cabinets that create a roll around cart. Door flanges, mounting blocks, top plate etc. Various parts have pre-machining, pre-bending etc etc. The entire thing then has machining as a weldment. All done as a weldment...because it's a weldment.

When I bold on the doors, add the power disconnect, interlocks etc...then it's an assembly

MJuric wrote: ↑Wed Sep 01, 2021 1:30 pm That's what I'm arguing. I don't care about complexity I care about whether it's a weldment or not. If it's not a weldment, don't use multibody. If it is a weldment, use multi-body, lots of complex sheet metal parts or not.

I don't find one or the other "Harder" or "Easier" to do except how you process it down the line and specific tools available. I'm working on the cabinet below as a weldment. It's essentially two electrical cabinets that create a roll around cart. Door flanges, mounting blocks, top plate etc. Various parts have pre-machining, pre-bending etc etc. The entire thing then has machining as a weldment. All done as a weldment...because it's a weldment.

When I bold on the doors, add the power disconnect, interlocks etc...then it's an assembly

image.png

What do you do with purchased hinges when one side is welded to the frame?

I'm mostly concerned about preventing problems down the road by making sure people are using the intended process. I do process consulting, training, troubleshooting, and sometimes just settling arguments. You have to have a modeling process that everybody can use. If you're the only one, you still have to provide for people who are going to get the data after you. You really don't want them calling you names.

If the parts to your cabinet are bent before it is assembled, meaning you pick parts from a stack of finished parts to weld them, then I would model as individual parts. If the same guy bends them and welds them all at one station, then I'd do it as a multibody. If the individual parts have part numbers - separate parts.

I stress this "process" part of things because it is important in SolidWorks. They also want to make everything easy, which means people get drawn into bad processes "because they can" sometimes. With synchronous, process doesn't matter at all. The only thing that matters is the end result. This is why synchronous is such an amazing relief, especially in assemblies. Edge does force you down the correct process more often than works does, so there is less to worry about in that respect. But you can probably force things off the rails if you really wanted to.

MJuric wrote: ↑Wed Sep 01, 2021 1:30 pm That's what I'm arguing. I don't care about complexity I care about whether it's a weldment or not. If it's not a weldment, don't use multibody. If it is a weldment, use multi-body, lots of complex sheet metal parts or not.

I don't find one or the other "Harder" or "Easier" to do except how you process it down the line and specific tools available. I'm working on the cabinet below as a weldment. It's essentially two electrical cabinets that create a roll around cart. Door flanges, mounting blocks, top plate etc. Various parts have pre-machining, pre-bending etc etc. The entire thing then has machining as a weldment. All done as a weldment...because it's a weldment.

When I bold on the doors, add the power disconnect, interlocks etc...then it's an assembly

image.png

That's an interesting drawing. How did you get that shoe watermark onto the page?

matt wrote: ↑Wed Sep 01, 2021 2:08 pm What do you do with purchased hinges when one side is welded to the frame?

For the most part when we do this we mount the hinge to the door and weld the hinge to the mating part so at least in our case this is an assembly process not part of the weldment. Typically mounting one half of the hinge to one side and then mounting the other half to the other side doesn't work out great.

If I were to make it part of the door weldment I can see two or three different ways to do this.
a) Split the hinge and have half with the weldment and half with the door
b) Put the entire hinge with the door and control motion with configs in the weldment.

Both of the above have at least a couple ways to break down the parts and part numbers as well.

I don't believe any of this is set in stone and in every case you have to find out what works best not only for the model, but for all the down stream processes, paper work etc etc.

matt wrote: ↑Wed Sep 01, 2021 2:08 pm I'm mostly concerned about preventing problems down the road by making sure people are using the intended process. I do process consulting, training, troubleshooting, and sometimes just settling arguments. You have to have a modeling process that everybody can use. If you're the only one, you still have to provide for people who are going to get the data after you. You really don't want them calling you names.

If the parts to your cabinet are bent before it is assembled, meaning you pick parts from a stack of finished parts to weld them, then I would model as individual parts. If the same guy bends them and welds them all at one station, then I'd do it as a multibody. If the individual parts have part numbers - separate parts.

Again I think this depends on use, process etc. For us if it's a weldment, it's a weldment. Doesn't matter what the process is to get the parts for those weldments. In fact many of our pieces for our weldments have multiple processes done to them prior to welding. Pre-Bend, Pre-machine happen to nearly all our parts. Those parts "Part numbers" are tied to the weldment. So if the weldment is ABCDEF then piece one is ABCDEF-01, part two is ABCDEF-02. For parts "RE-Used", like weld nuts, latches, pins etc they are inserted parts into the weldment.

mike miller wrote: ↑Wed Sep 01, 2021 2:13 pm That's an interesting drawing. How did you get that shoe watermark onto the page?

I downloaded those backgrounds a few years back. I have that one, a coffee stain, blood stain and burnt weld mark. Someone had them in a single zip file somewhere.

That's the only one I use because all the other ones have "Black spots" that if text or features end up behind you can't see them.

SPerman wrote: ↑Wed Sep 01, 2021 7:20 am Yes, that works. I usually double check that the view is actually 1:1. Sometimes SW will change that when creating the view.

Are there limitations on the drawing sheet size? I guess if you are buying your sheet goods on a roll, this could be a problem. Otherwise I doubt you need a dxf larger than what SW can create. It had no problem with me setting my sheet size to 1000 in x 1000 in.

image.png

Indeed 25m.sq. is MUCH bigger than any plate I would need cut. But 6mx3m (240"x120") is possible, tho rare.
It never occured to me to consider that paper size could be adjusted to be so large. Tho, I would question why ..?.. (Tentatively of course, my ignorance can be overwhelming sometimes..).. I guess if I was printing to a plotter or truly huge paper, but I mostly use A3. (11"x17")

MJuric wrote: ↑Wed Sep 01, 2021 8:44 am Yes, there is a setting in options, see below, that exports DXF's to a 1:1. You can then just import the geometry into whatever software you're using to cut the template. In some cases, depending on software, you may have to delete the border etc from the DXF or have it on a different layer you just turn off.

All depends on your process, equipment etc. All of our internal stuff is cut off the model so we don't do DXF. External stuff can be DXF, DWG, native whatever...

image.png

Then again, we do not laser-cut in-house, its all done by outsource suppliers who request DXF Files..
I've only used DRW files purely for the purpose of creating drawings. It also never occured to me to export a DXF from there.

And guys, are there benefits to this I'm missing out on..? clearly I do not understand.

I may learn something new..

Hi Matt,

What is your issue with multibody Sheet Metal? I think it is a brilliant way to design sheet metal parts in context to each other without top-down assembly method.

-Mark

Damo wrote: ↑Wed Sep 01, 2021 9:02 pm Then again, we do not laser-cut in-house, its all done by outsource suppliers who request DXF Files..
I've only used DRW files purely for the purpose of creating drawings. It also never occured to me to export a DXF from there.

And guys, are there benefits to this I'm missing out on..? clearly I do not understand.

I may learn something new..

To me, when speaking of weldments, using SW weldments is just significantly more efficient, effective and easier.

To me three are several advantages to working in weldments.
1) One sketch can do multiple pieces and controls, sizes, locations etc
2) No mates
3) All parts are naturally "In context" and update based on changes with any other part. Granted you can do this in an assembly but for the most part it causes issues and problems. In Inventor this is how I designed pretty much all my assemblies but had a whole lot of problems doing it in SW.
4) One file. Just like a weldment where you end up with a single welded together part one file represents one part but can contain all the information for all the pieces.
5) All the drawings come from that one file

The same advantages as above also apply to any assembly that you want to use as an assembly but want to represent as a single part, Cylinders, Ball Screws and other purchased actuators are a good example. That cylinder you tend to order as a single part so it's represented as a single part. Motions are show with configurations of that multi-bodied part. The single file approach tends to, at least in my experience, keep things cleaner. You no longer have to "find all the parts" or do a pack and go of an assembly to send a weldment to someone, one part.

There are a few other tools that are somewhat helpful when working with weldments that aren't available otherwise but none of them are really noteworthy.

first thing, i don't want people to change their workflow, stay with it if you are happy of it !

i understand what Matt wanted to start with this question.

but as you can see Matt, you can't clearly talk about that with anybody.

the knowledge of SW differ a lot from people, based on their job,
their formation, their desire to go deeper in understanding the software, have a minimum of informatical-logical-mind, etc...

some only see the top of the iceberg (but it's enough for their needs), but think they are master.
Matt, yes with some too advanded-complexe sheet, SW can turn buggy, i saw that, and the wise choise is the change the workflow for that kind of part, do it by using ASM.

i understand you matt, but you will not be able to talk about that and have a mature discussion here.

there are a lot of thing here or on others posts that can be counter-argue so easily.
example of bad things i saw :
PRT can have mates, PRT-Excel a way more powerful than Toolbox,
the opposite good-use of 3D-filters of SW, activating blockrebuilt on all library parts, etc...

Yes some people are using the software in the opposite-way, counter-way that some features are supposed to be used.

we can also saw some baby-questions like : don't understand thread-cosmetic behavior, don't understand parent-child for dims, bla bla bla...

Matt you can't talk to people who don't fully understand some kind of features (example Ext-Ref), have a deeper dialog about that.
again, some only know 20-30% of a feature, but think they know it entirely, and they are master in that domain.

i can say again what i said in the old-forum,
there is also the famous "hybride ASM-PRT" method, that can be really powerfull in some case, but that require to know deeply how bom and configs work...

and again, i don't want people to change their workflow, stay with it if you are happy of it !

also Matt, keep in mind that some people here, doesn't know the "working 3 modes" and ASM can have....
it says a lot...

it's also like the battle between the "Flatenners people" and normal people.
don't lose your energy in making them to open their eyes,
let them stay in their bubble-sphere vision.

Merovingien wrote: ↑Thu Sep 02, 2021 9:24 am
...................i understand you matt, but you will not be able to talk about that and have a mature discussion here...........

Uh, if not here....where else? Some of the brightest and best SWX users I know are members here (and no, I'm not one of them).

As far as new users asking "easy" questions, that's a crucial part of keeping this place active. Otherwise there's just a bunch of gurus sitting around and comparing the lengths of their beards. Please, let's not be so narcissistic that we drive them away ..... lest we end up being even more "America-centered".