CAD Forum

mbiasotti wrote: ↑Wed Sep 01, 2021 10:29 pm 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

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.

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.

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.

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.

matt wrote: ↑Thu Sep 02, 2021 10:11 am 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.

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

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 $#!+? 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.

mike miller wrote: ↑Thu Sep 02, 2021 9:35 am 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".

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.

matt wrote: ↑Thu Sep 02, 2021 11:03 am 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 $#!+? 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.

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!?

mike miller wrote: ↑Thu Sep 02, 2021 1:57 pm 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!?

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.

MJuric wrote: ↑Thu Sep 02, 2021 8:46 am 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.

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

Lapuo wrote: ↑Fri Sep 03, 2021 4:12 am Hey @MJuric , i am curious , how do you handle sheet metal part with weld bolts?

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.

matt wrote: ↑Thu Sep 02, 2021 10:11 am It's sloppy, and from a file management point of view you lose track of parts that are done that way.

@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?

Ivan wrote: ↑Tue Sep 21, 2021 5:56 pm @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.





@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.

As I've mentioned before there is a line, at least in my opinion, where something is a "Weldment" in which you should use SW weldments, and where something becomes am assembly, where you should use an assembly.

Where that line is is going to depend on many things that I don't think can easily be figured out on a forum like this.

That being said however there is nothing preventing the usage of a bracket in a weldment, even as a separate level and recalling the individual parts. You can do that using sub weldments. I do not believe you can get qty's, properties etc for sub weldments any deeper than a single level however. I drop some picks of what I'm talking about below.

So if you have bracket 123456 and that bracket was also used in a sub weldment you could create a weldment that contained bracket 123456 and a sub weldment that used bracket 123456 and when you dropped in the cut list you would show a qty (2) of bracket 123456.

As I said I'm pretty sure this will not do three levels though. So if you had a sub weldment that had a sub weldment that had bracket 123456 I do not think it would show in a cut list of the top level weldment.

I personally do not mess with sub weldments very often so I'm not 100% sure what their limitations are.

Oh, oh, another thing why weldments can be AMAZING.

This is one feature (wrap) within a weldment followed up by a split command. It's a pain to build with a SSP. Plus:
Using surfaces is incredibly painful with an SSP. I mean surfaces never break reference when you work in an assembly, right?

Honestly, From the outside looking in.... I couldn't figure out what you guys were arguing about...
Seems each comment changed what I thought you were saying...
Some of it might be language / translation issues.
Some of it might be using the term "Assemblies" when referring to to assembling parts into a welded part.
Some of it might be referring to weldments that aren't technically weldments, in Solidworks context.

Matt doesn't clarify if he's talking about multiple sheetmetal parts that are welded together, or bolted together, or (yikes) formed to be one part.

While there are many ways to skin a cat... I have seen some really tedious and dangerous ways of doing things suggested in this thread.

IndianaDave wrote: ↑Wed Sep 22, 2021 1:10 pm Honestly, From the outside looking in.... I couldn't figure out what you guys were arguing about...
Seems each comment changed what I thought you were saying...
Some of it might be language / translation issues.
Some of it might be using the term "Assemblies" when referring to to assembling parts into a welded part.
Some of it might be referring to weldments that aren't technically weldments, in Solidworks context.

Matt doesn't clarify if he's talking about multiple sheetmetal parts that are welded together, or bolted together, or (yikes) formed to be one part.

While there are many ways to skin a cat... I have seen some really tedious and dangerous ways of doing things suggested in this thread.

The terms are all SolidWorks terms, not necessarily common engineering or manufacturing terms. SW Multibody stuff can be used in a lot of ways. It can also be misused in a lot of ways. SW weldments throw a kink into things because it is inherently a multibody workflow, and a few releases back SW sheet metal enabled multibody models.

There are a lot of different ways of working. Some of the software methods don't fit some of the manufacturing/design flow very well. Some of the proposed techniques are very "hack and whack" and prevent you from doing much formal data management. It's hard to condemn any particular technique wholesale. If you've got one guy in a shop cutting plate and bending sheet and welding it all onto structural shapes, the formal process doesn't matter as much. If you have a large company that makes parts, puts them on the shelf, or has someone else make them, and then they weld the parts together, yeah, you've got to do something more formal and deliberate.

Pics may clarify my point...

(inline images, what a great concept!)

This gets me what I need. It just feels a bit redundant have 2 similar drawings of what is essentially 1 weldment in the shop.

I've also seen people model each separate pc of tubing as it's own part and then mate everything together in an assembly. That's just silly to me, why waste a great weldment feature. And have a massive stack of drawings. But... as has been mentioned better than I can, there are reasons for different methods.

mike miller wrote: ↑Wed Sep 01, 2021 7:14 am

dumpster.gif (50.03 KiB) Viewed 3502 times

I guess he doesn't know that it is dangerous to throw cigarette butts in garbage containers.

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.

It's not my preferred method.
I need to prepare production drawing and DXF drawing for each part separately. This process is very tedious for multi-body parts (for me).
But sometimes clients want Render, I need to turn quickly, creating a multibody drawing by sticking to the general dimensions is a quick way to render. (no production and technical drawing)
In short, dangerous for production but fast for visual work.

matt wrote: ↑Thu Sep 02, 2021 11:03 am 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 $#!+? 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.

Agreed Matt, but what you speak of are working methods, procedures, and proper training, or at least that's how we "treat" them here.

We have a document to explain how we use the skeleton method, depending on the type of product we are working on, because yes, the workflow can differ from one product to another.

We've created a bunch of procedures to follow along with the training we give to new users coming in. It serves as a reference for everyone and anyone who has to work on something they don't generally work on.

For example, I don't draw flatbed trailers very often, so I'd have to sort of remember how they are built. The procedure we created explains all of this, so I can explain something to someone and then refer them to the document at hand so that they can look it up later on.

We have documents to:
-Explain our internal part codification
-Explain how to create a project or a product.
-Explain how to use CustomTools with the set-up we have.
-Explain how to efficiently correct someone's project.
-Explain how to use the skeleton sketch method depending on which type of product we are working in.
-Explain how to use our ERP
-Explain how to create our electrical/pneumatic/hydraulic drawings in SolidWorks
-Understand how to use the collision detection tool efficiently.
-List all the known bugs on the current version we work on, along with the work-arounds we have found.
-Etc...

As I've previously said, we avoid multibody parts as much as we can but the cases we do use them are very specific and also make it a lot easier for us to build these multibody parts. We could most likely split it into single parts and build an assembly but there wouldn't be any gain on our end, so we stick with what we have.


Edit: It does make for quite a tedious training for one to work with us though.

AlexLachance wrote: ↑Thu Sep 23, 2021 10:29 am We have documents to:
-Explain our internal part codification
-Explain how to create a project or a product.
-Explain how to use CustomTools with the set-up we have.
-Explain how to efficiently correct someone's project.
-Explain how to use the skeleton sketch method depending on which type of product we are working in.
-Explain how to use our ERP
-Explain how to create our electrical/pneumatic/hydraulic drawings in SolidWorks
-Understand how to use the collision detection tool efficiently.
-List all the known bugs on the current version we work on, along with the work-arounds we have found.
-Etc...

Your methods are really nice. In the company I work for, there is no established discipline yet, generally things progress with the experience of people.
often the boss does not accept ideas that are not his own, he thinks that he should find all the innovations himself. and after a while he tells us some of the ideas offered to him as if they were his own.

Ömür Tokman wrote: ↑Fri Sep 24, 2021 2:01 am Your methods are really nice. In the company I work for, there is no established discipline yet, generally things progress with the experience of people.
often the boss does not accept ideas that are not his own, he thinks that he should find all the innovations himself. and after a while he tells us some of the ideas offered to him as if they were his own.

Those are not my methods, merely the company's knowledge/experience kept written down somewhere. I am indeed lucky to have open minded bosses, but things are not so different. Things progress with the experience of people around here too!

Ömür Tokman wrote: ↑Fri Sep 24, 2021 2:01 am and after a while he tells us some of the ideas offered to him as if they were his own.

Are you working for my Wife?

My clients make finish architectural metals. Every situation is completely different. So my design process usually has the "figuring it out" phase, and then the "fabrication ready" phase. Multibody is very helpful in the "figuring it out" phase... To be fair our sheet metal projects are usually quite simple, just a bends and a few other details.

This is a pretty neat post. Just wanted to share an sheet-metal export macro I wrote for anyone interested. It includes the option to export all bodies as separate dxf/dwg files. Can be downloaded here: http://www.sashaskolnik.com/downloadables.html

Honesty here, I haven't read the entire thread so I may be repeating something someone else has said.

I hated multi body sheet metal as an independent before I started working for a steel vendor. since then I have found that my clients don't usually provide verified cut files, which means I have redraw their parts and usually they have between 20 and 75 parts that are almost the same but different with 3 or 4 part types. I'll make the 3-4 types as multi body and control all the variations with a design table. the largest benefit i see from it is in the drawing environment where I can copy a drawing and change the configuration to me next part.
the 2nd largest benefit is being able to RAPIDLY processing change requests and updating all the drawings. for example today a customer want ed to change the thickness of their 40+ part package package. make a change, hit CTRL-Q like 5 times and save as PDF and I had it back to him in 5 mins instead of 6 hours