multibody sheet metal

SOLIDWORKS SW General
41

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.

42

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

43

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.

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.

44

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.

45

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")

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.. :smiley:

46

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

47

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.

48

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.
Capture3.png
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 !

49

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.

50

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”. :open_mouth:

51

It’s sloppy, and from a file management point of view you lose track of parts that are done that way. Plus, if the parts are complex, you’ve got to be careful about feature order. Plus, multibody parts force history to dictate what’s on the screen. You want all of your features for each part together, maybe in folders, but if you do that, you can only have a one-directional view of the parts together, because in the other direction, one part is rolled back.

It’s sloppy and inelegant, and poorly organized.

If there are so many problems with assemblies, why don’t they fix assemblies rather than backdooring assemblies through parts? Especially in a history-based tool, it’s just a bad idea all the way around.

52

I’m glad you understand. Thanks for saying that. I think that a mature discussion is exactly what’s happening. I state my case, and people hopefully understand it. I’m not the police, so they keep doing what they want. I hope what I say at least makes people think. And I’m totally cool with people fixing bad practice workflows, by the way. :smiley:

Plus, I think I’ve at least offered some situations where it’s not such a bad idea, like really simple sheet metal, or one person responsible for their own stuff. (Ad hoc hack and whack modeling)

I have to admit that I too have a certain perspective. For sheet metal, I rarely do that in my every day work, but in consulting work I deal with it all the time, and with companies that have very different means of getting things done. I’m usually brought in to do best practice consulting, specialized training, process improvement, file management implementation, and so on. So I’m trying to get companies set up with the best possible process. If you’re just one person, and you’re responsible for your own stuff, I’d still recommend better practice, but it’s less of a disaster. The more people you have and the wider the range of skill levels you have, the more of a problem something like this becomes.

My perspective is modeling practice that creates the least number of problems when you look at the whole scenario. That almost always means there’s a hierarchy of practice, and there’s a definite orthodoxy. You should understand how it all works - the correct way and the backdoor workarounds, because there are times when you need those workarounds. My point of view is that workarounds should not become your primary techniques.

I wrote one time about the “Rings of Fire” or something like that. It was a set of concentric circles moving from stuff that is pretty safe to stuff that is less safe. Most of my modeling work is in the WARNING SEVERE INSTABILITY range, with surfaces and trims, and whatnot.

And since I’m kind of on the Solid Edge kick lately, this is less of a problem in synchronous because of the lack of the history problem. Why would you introduce history-based limitations between parts? You have to have the features of one part before or after the features of another part - mixing them together would be another level of disaster. Do you really have the discipline in an already undisciplined method to keep the features separate?

Synchronous assemblies would allow you to match features in the parts - going either direction or both directions (A=>B or B=>A)- without incurring in-context or circular references. You can actually also do that in Solidworks, but for some reason people keep forgetting it.

This is just like the mania that surrounds zero-thickness errors. You’ve got a whole class of people who claim they NEED to design with zero thickness conditions in their models. But they don’t really need it, obviously. Same exact deal. People claim there’s some problem with assemblies, and they keep trying to make parts into assemblies. But there are so many things you give up when you do that. I can’t say I understand it, but people accept a lot of limitations just to feel like they’re getting away with something.

I’ve said it all multiple times now, so for those who feel the need, it’s no skin off my nose what they choose to do, really.

53

Easy matt . It all depends on usage right? I’ve picked up that all some people need is the quickest and easiest and dirtiest way to get a digital representation of the physical objects they need. They will likely never need the model(s) again, likely never revised or reuse the same part numbers or even assign part numbers to them. Once the product is out the door they could move all the CAD files to tape backups and burn the tapes. Frankly, if that was the environment I worked in I would use all the snazzy whiz-bang methods marketing likes to show off and any attempt to reuse or maintain those models would be vanity, but who cares, just remake them. But I’m stuck in a world where files are copied to make similar part, revised, and reused all over the place for 20+ years. So stability and reusability is the priority. Even if it takes twice as long to model the first time it will save days of labor in the life of that part and all the others that spawn from it.

My $0.02

54

There’s maybe something some folks don’t get about me. I’m not one of these absolutists we see so much today who totally buy into one thing regardless how extreme they have to get. To me, there’s always a continuum. Yes, I believe replacing assemblies with multibody parts is a bad idea, but sometimes its a level 1 bad idea and sometimes its a level 10 bad idea. If you’re doing this on your own, 3d doodles, and you’re a SW wizard, then who gives a shit? But if you’re directing a department of people to do it, and you’ve got some who have a tenuous grasp on the software, and some wizards in the same group, you really need a more disciplined approach.

55

Some people are unwilling to accept that there isn’t a “One size fits all” answer and are simply convinced that the way they do it is the ONLY way and the RIGHT way.

When you have convinced yourself that your position is the only right way all other ways must, by default, appear wrong and the people doing them “Stupid”, “Unintelligent”, “Misguided”, “Wrong” etc.

People with this mentality feel that having such discussions are a waste of time because since they are completely unwilling to even contemplate other peoples positions they assume so is everyone else.

Thus it’s not just “Here” that ends up being a waste of time for discussions but anywhere where the discussion is not agreeable to their current position.

56

Hold on a minute. Weren’t you advocating the Ten Cadmandments just a few months ago? HOW DARE YOU BE A MORAL RELATIVIST WITH NO ABSOLUTES!?

:laughing: **

57

Sometimes killing someone else is murder, and sometimes it’s righteously slaying an evildoer with the jawbone of a jackass, right? Although it strikes me I might be dangerously mixing my religious metaphors here. I love the whole “jawbone of a jackass” bit. That can be used in so many ways.

58

Hey MJuric , i am curious , how do you handle sheet metal part with weld bolts?

59

I used “Insert part”. You have options to insert cut list properties, custom properties etc. If you set the inserted part up correctly that information is carried over to the cut list.

60

matt, losing track of parts is my main hold back with MB SM. This also applies to weldment end caps, bolt plates, SM brackets, etc. However, I would love to find a working method for this.

I used “Insert part”. You have options to insert cut list properties, custom properties etc. If you set the inserted part up correctly that information is carried over to the cut list.



“Multibodied parts” are almost always going to be weldments in my case. So I create a weldment and put bent sheet metal parts in that weldment. From there I create configurations that are of the above but only have the individual sheet metal parts. That way I can create drawings of individual sheet metal parts that are used in the weldment. That is how the below part was created which is a mixture of bent sheet metal and plates.

MJuric, in your quotes above I understand what you’re doing. But I don’t think there’s a way to pull quantities of those inserted parts in a master parts list (BOM) of an entire project.

For example, one workflow I often use is every individual part has it’s own part number and drawing. One bracket can be used in many levels of weldments or assemblies. In the top level asm I insert a “Parts only” BOM and save that as Excel file. This along with all the part drawings (pdf, dxf) is great for outsourcing to laser cutters, gives them all the total quantities of all parts they need.

When I get to a multibody tubing/angle/pipe scenario, I love to use the weldment feature. BUT plates or sheet metal that are laser cut and used in multiple weldments (end caps, bolt plates, gussets) I need to identify and show up as separate parts in the top level BOM. My workaround is model all the profiles (tubing/angle/pipe) in a weldment part, then insert into an assembly (technically acting as a ‘weldment’ still, as in parts that are welded together) in which I add any plate and sheet metal parts. Downside to this is you have about double the drawings for all weldments. First is the weldment part with the weldment cut list, and then that same weldment with a few plates added.

Haven’t full tested this but I’m also trying an indented, with detailed cut list, BOM on the assembly drawing that contains the weldment part and the extra plates. I think this just includes the weldment cut list which should allow me to eliminate the first drawing of the weldment part. BUT… that weldment part had a part number that will be in the master parts list that people will look for and, not find it. See, it’s not great.

Is there a more efficient way to do this?