Weldment parts vs assemblies of welded parts

[gerard]

Hey there,

I'm officially an "old fart" having been around SolidWorks since '95.

One of the newer "developments" of SolidWorks is the ability to do weldments as a part.

I've gone through the tutorials and such, but I don't see the benefit.

I was taught from early days to put one part per page/drawing. I prefer per drawing, but I seem to be in the minority.

In working with fab shops, both in house and contractor, the ability to give separate parts on separate sheets to tradesmen was very useful. Otherwise some poor schlub gets to make copies on the copier...

I've gotten a bunch of models from one of our industry partners with weldments as parts.

My first inclination is to bust them all up into assemblies and detail all the piece parts and then detail the weldment.

Saying all that, I do this very infrequently nowadays, so I may definitely be "behind the times".

Once I'm done, I'm gonna hand this off to yet another party. If I break this up into assemblies, will this be a Whisky Tango Foxtrot moment?

What's the consensus part weldments or weldment assemblies.

Alex, I'm particularly interested in your thoughts.

cheers

g

[AlexLachance]

Well, there's a lot of variables to be taken into concideration into this and all roads lead to Rome, so in this instance it generally depends more on company policies and preferences then proficience I would say.

We use weldments in specific situations, and we also have work-arounds to work around the limits 'imposed' by using this method.

I guess the first questions you'd have to ask yourself would be:
Would it be easier for me to manage one drawing with multiple sheets then multiple drawings with one sheet?
What would be the benefits and drawbacks?
If you have an ERP, how would you get your ERP to do the distinction between a multibody part and a single-body part?
Do you need to generate PDF/DXF? If so, how will you proceed? How are you going to generate each drawings/DXF seperateley even though they are in the same SolidWorks file? More importantly, how will you merge pages that need to be merged together?(the 'assembly pages' for instance)

I don't think anyone who uses SolidWorks would have trouble with whichever approach is used, as long as they are instructed accordingly. Whichever decision is taken will have it's lot of 'work-arounds' to deal with the lot of exceptions that it generates.

[Frederick_Law]

Another feature DS didn't plan it out.
The main problem is Weldment PartList doesn't work well with assembly BOM.

Try it and see what work for you and what not.

[gerard]

Well, there's a lot of variables to be taken into concideration into this and all roads lead to Rome, so in this instance it generally depends more on company policies and preferences then proficience I would say.

We use weldments in specific situations, and we also have work-arounds to work around the limits 'imposed' by using this method.

I guess the first questions you'd have to ask yourself would be:
Would it be easier for me to manage one drawing with multiple sheets then multiple drawings with one sheet?
What would be the benefits and drawbacks?

If you have an ERP, how would you get your ERP to do the distinction between a multibody part and a single-body part?
Do you need to generate PDF/DXF? If so, how will you proceed? How are you going to generate each drawings/DXF seperateley even though they are in the same SolidWorks file? More importantly, how will you merge pages that need to be merged together?(the 'assembly pages' for instance)

I don't think anyone who uses SolidWorks would have trouble with whichever approach is used, as long as they are instructed accordingly. Whichever decision is taken will have it's lot of 'work-arounds' to deal with the lot of exceptions that it generates.

Good feedback. We don't have an ERP. I'm effectively acting as a consultant on this. The end "user" doesn't have an ERP either. It's a fairly odd arrangement that I'm not at liberty to discuss. This is a one off thing, so at the end of the day it could go one way or the other.

Another feature DS didn't plan it out.
The main problem is Weldment PartList doesn't work well with assembly BOM.

Try it and see what work for you and what not.

Therein lies the rub. I'm struggling with that as well.

Appreciate the feedback from you guys.

I'm going to go the assembly route.

thanks!

g

[TTevolve]

I am also and older user (since 2003) who is now working at a place where we do in fact make welded components. Using weldments in solidowrks makes a lot of sense when you actually have a part that is made up of pieces welded together. I just did a ladder that is made up of Sch40 pipe, doing it as a weldment allows you to cope the pipes and have the software generate the cut list for you, which can be a big help.

But you will run into issues if your using PDM/ERP and need to have individual components that have part numbers. In our case this ladder is a single part number for the entire thing, and we use the raw tube part numbers and length to cost it/make it, so we don't have an issue with this specific part. But if you have mounting plates, or other components that have to have separate part numbers/drawings to make them, then you are better off doing an assembly.

This is very similar to how/when you use multi-body parts vs. assemblies

[mp3-250]

It depends and vary from company to company depending on requirements.
If you need a part number for each "cut" you can make an assembly, if you do not need it you could try the multibody approach in weldments. the tool itself can automate a lot of cut operation and keep the weldments profiles cuts coherent driving them only with a simple 3D sketch.

this "old" welment functionality is not bad in theory, (I do not use the new welding system or whatever it is called so I cannot comment about it), but for our company the SW weldments has been a sour ride.

Bug ridden and regression killed the whole thing hard at least 3 times during the past 2 years.
Like materials assigned to single bodies popping up from god's only knows where after a part rebuild.
Or SW translating a legacy variable name instead of its label making our legacy data to output NOTHING inside the BOM description. (SPR escaled from low to critical)
I recently happened to discover that the balloon number lock inside the BOM is working in a quite exotic way and that there is no way to know if the bom order was manually altered by dragging the bom rows or the bom is still synchronized with the cutlists item in the 3D...I also made a post about it: I locked a bom, put the part on revision and all the added bodies got the same balloon number with different entries. like 1,2,3,4,5,5,5 you have to delete the bom to fix it, and workaround somehow to skip a row number if required. (for us is a must when a body is deleted from the 3d and its bom's row disappear after a drawing revision)

Just to give you an idea we have up to 80-100 parts in a weldment bom spanning like four A1 sheets 2d drawing.

[AlexLachance]

Good feedback. We don't have an ERP. I'm effectively acting as a consultant on this. The end "user" doesn't have an ERP either. It's a fairly odd arrangement that I'm not at liberty to discuss. This is a one off thing, so at the end of the day it could go one way or the other.



Therein lies the rub. I'm struggling with that as well.

Appreciate the feedback from you guys.

I'm going to go the assembly route.

thanks!

g

You can accomplish pretty much the same thing as a weldment in an assembly using the skeleton method, and it allows the possibility to use parts in multiple assemblies, rather then having the bodies bound to a part.

It's a bit more complex then that, but if you understand the skeleton method, you should get the jist of what I'm saying.

You will run into issues if your using PDM/ERP and need to have individual components that have part numbers. In our case this ladder is a single part number for the entire thing, and we use the raw tube part numbers and length to cost it/make it, so we don't have an issue with this specific part. But if you have mounting plates, or other components that have to have separate part numbers/drawings to make them, then you are better off doing an assembly.

I developped an internal codification for our "brute parts". What I call brute parts, are parts cut with dimensions and nothing else. We didn't want to have brute-parts integrated into our ERP, but as we continually evolve, it is a good thing that I built this codification because it allowed to ensure to not create duplicates, and it also gave the possibility to have these "brute parts" created as items rather then consumed as material if the need ever arose, which it did.

[Frederick_Law]

Once you got the weldment, you can save all the bodies out as parts.
Another painful thing to learn.
Like all SW commands, you need to finish it in one shot. Good luck when you have 200 bodies to save.

[Frederick_Law]

You can accomplish pretty much the same thing as a weldment in an assembly using the skeleton method, and it allows the possibility to use parts in multiple assemblies, rather then having the bodies bound to a part.

It's a bit more complex then that, but if you understand the skeleton method, you should get the jist of what I'm saying.

You'll need to do miter manually.
Not bad since the auto one go crazy when you modify the weldment anyway

[TTevolve]

I developped an internal codification for our "brute parts". What I call brute parts, are parts cut with dimensions and nothing else. We didn't want to have brute-parts integrated into our ERP, but as we continually evolve, it is a good thing that I built this codification because it allowed to ensure to not create duplicates, and it also gave the possibility to have these "brute parts" created as items rather then consumed as material if the need ever arose, which it did.

Yea, we do the same kind of thing. Our costing on welded assembly items is on the entire assembly, not on the individual pieces that make up the assembly, we do this to capture welding times in the costs. So we can get away with just having a cut list on a drawing for them to go by. A lot of things that you do in SW is usually determined by other outside factors, such as ERP and costing.

My experience with weldments is limited, I only took the weldments fundamentals class earlier this year, while it looks neat I can do most of the same stuff using an assembly, and I wouldn't do it with something super complicated with all the issues other are having.

[Arthur NY]

Weldments being in a Part file goes back to at least SW 2005-ish (I'm old and my memory fails me all the time.....). Pretty much once they added the possibility to use multi-bodies in a Part file this functionality became possible.

Also @Frederick_Law As long as you choose the option to for "indented' and "Detailed cut list" then your BOM should show everything. Also, and this is VERY vital once completed doing all of the weldments that you need you have to make sure to go to the "Cut List" at the top of the FMT and choose to "Update Automatically". This should be on by default but isn't and can throw things off especially when it comes to a BOM.

As a whole the overall modeling approach when using weldments isn't all that different than using Multibodies. While not a 1:1 there are some very similar methods and approaches that can be used. As @Frederick_Law pointed out you can use the "Save Bodies" feature to push out all of the individuals bodies to their own Part files which additional details can be added that will not be reflected in the master Part file. There isn't a huge downside to having one drawing with multiple sheets to it unless you start going past like 50 then you might want to start a new drawing.

[Arthur NY]

Speaking of which, I had to shake off the cobb webs of even using the Structure System side of Weldments as I've been so use to the "old way".

Much like the difference between using the Loft or Boundary Feature. Initially they seem quite similar but there a times when one can be leveraged better in certain situations where the other might fail.

There are definitely some nice additions to this system that add in ways that the old Weldment feature never had.

[Glenn Schroeder]

Hello,

I was off work yesterday and didn't check in here, so I'm late to the party, but I use weldments often, and have since 2009. Similar to @TTevolve above, if it gets welded together it's a single Part file, and I never break them down into individual Parts after the initial modeling.

When detailing them in a Drawing the "Select Bodies..." button is a big help. I believe it was introduced in SW2010.

As far as I know, in a situation like yours the only possible drawback is the inability to call out cut list properties in the title block. I don't do that anyway, so it's not an issue. As I think someone mentioned above, they have made improvements in referencing cut list properties in BOM's. If they'd do the same with referencing them in notes that don't belong to a specific drawing view that issue would be completely eliminated.

[Frederick_Law]

I tried structure system, it was worse. Another half baked feature.
It's easy to throw things together. Good luck get organize and get what you want.

[AlexLachance]

Hello,

I was off work yesterday and didn't check in here, so I'm late to the party, but I use weldments often, and have since 2009. Similar to @TTevolve above, if it gets welded together it's a single Part file, and I never break them down into individual Parts after the initial modeling.

When detailing them in a Drawing the "Select Bodies..." button is a big help. I believe it was introduced in SW2010.

As far as I know, in a situation like yours the only possible drawback is the inability to call out cut list properties in the title block. I don't do that anyway, so it's not an issue. As I think someone mentioned above, they have made improvements in referencing cut list properties in BOM's. If they'd do the same with referencing them in notes that don't belong to a specific drawing view that issue would be completely eliminated.


image.png

I use a work around. I create annotations that are bound to the view that displays the body and those annotations call out the properties of the body.

1. Body description
2. Body operation (Plasma cutting)
3. Body Weight
4. Body number validation.

The part-number shown in the title block is a combination of the drawing name and the sheet name.
Drawing name is POUT-M302
Body name is WEBS04
Combination name for ERP is POUT-M302-WEBS04

[TTevolve]

The "Update Automatically" has got me a few times now. Create a drawing of the weldment, add the cut list table and all the boxes are blank. No idea why this wouldn't be on by default.

[Arthur NY]

The "Update Automatically" has got me a few times now. Create a drawing of the weldment, add the cut list table and all the boxes are blank. No idea why this wouldn't be on by default.

I've brought this up NUMEROUS times to ppl over at SW HQ and there's this look in their eyes like deer and then they shake their heads Yes, as if they understand what I'm saying, and then clearly it falls out of their brains through their ears and just go back to some mindless dribble......

[gerard]

This has been a great convo. I've busted apart about a dozen of these things and I'm nearly done.

Will read this more carefully once the alligators are no longer nipping at my nether regions.

thanks

g