Weldments, am I the only one not using them?

SOLIDWORKS SW General
1

It seems that everyone who is designing welded assemblies uses “weldments”; some with great passion over modeling pc parts and assembly. We do not use weldments where I work yet majority of the metal pc parts we make end up being welded to. I’ve read the SW Help pages about weldments, again, and they confirmed what I had thought. However, if you all don’t mind confirming or rejecting my conclusions regarding this so we are not missing out on a tool that has quite a following. Note, this list is for Solidworks, but is nearly identical to our check into weldments in Solid Edge.

  • A Solidworks “weldment” is a single part file with multiple bodies that represent individual parts.
  • component reuse is difficult. Ie. If weldment 1 has parts A, B, C and weldment 2 has parts B, C, D; when part C is revised the changes will need to be done in both weldment files?
    **edit: I did a poor job explaining this, weldments 1 and 2 would be part files, parts A B C and D are not files, just bodies in the weldment .sldprt files 1 and 2.
  • exception I can think of is if the bodies B and C in weldment 2 are inserted from weldment 1 and kept linked then they should update. This sounds like a reference nightmare.
  • Solidworks weldments work well when the pc parts do not have part numbers, are not inventoried but are ordered per job.
  • Solidworks weldments do not work so well when all parts have part numbers, are inventoried and ordered based on collective demand from all the where used.
  • weldments work great for assembling sections (angles, tubes, I, C, etc.)
  • weldments do not offer much value when most of the parts are formed sheet metal or machined bodies and there is only one or two extruded sections
  • weldment is not required to show weld beads in model (MBDish so weld data starts in 3D and not just on the drawing), we can add weld beads in assemblies.
  • it is possible to model nearly any weldment in a single part file as a weldment or as an assembly using pc parts; which method is best depends on many factors outside the capabilities of the software and the easiest/fastest way to get a model may not be the easiest/fastest method long term.


    Thank you!
2

That’s a lot. I think you understand it pretty well. I use it routinely, and would try to understand your use case to help with specific advice.

Any weldment can be a external (non virtual) file and thus you could use Part C in both contexts, and revise it independently once. To do this, I would not define anything of it in context, but rather handle it explicitly. You can make one piece as one part, but then you’d have to trim it manually because I do not think that you can weldment trim something that is not in the same part. Sorry, I didn’t try that out now. To trim, you could have associative Blocks which perform the trim cut profile, which does not exactly follow the profile of the trim body. I can make images to explain this if it is unclear.

There is no rule that you place all weldment bodies in one Part, although that is the easiest and most efficient way in my case. I sometimes segregate each profile into separate parts so that I can impose a total length property to SUM in Excel for purchasing lengths, and in other cases place all weldments necessary for a fabrication in one to three parts.

Here’s a useful example to me. I have a skid base made of C channel, where I wish to show hidden edges in a drawing to dimension the bolt down holes (not visible otherwise) or show the cross member profiles in the side views. However, I place my pipe supports and/or LCP stand in a separate Part so that I can hide hidden edges on most of it, but show hidden edges on what I want. I do this because I cannot show hidden edges per body, but only show/hide per body. I can show hidden edges per component.

Weldments have strengths in trimming tools, end treatments, and cut lists, but you don’t have to take advantage of these. You can complicate things as much as you’d like.

AFAIK, there is no (simple) tool to create a multibody weldment and then explode it into its single body pieces as parts, but it can be done.

3

My typical modeling project is usually plastics related. But I still do some weldments from time to time, and even to do somethings that maybe aren’t considered weldments. I’ve made lumber projects (picnic table) and an outdoor shed using weldments, mainly because the lumber shapes are similar to the metal shapes, and you want to get similar information, like a cut list.

4

I keep weldment with structure only. ie tube, I-beam.
I put it in an assembly and add other components.
It get complicate if any structure need pre-machining. Holes, cutout. Not end trimming.
Which will be done at the end of design. Hopefully the frame won’t change much.

5

Working on a deck design at home now using it, great for that At work…not used due to parts reuse mostly and our products don’t really have a need.

6

Weldments (as I understand the term) can be, but don’t have to be, multi-body Parts. If single body, there’s no reason why they can’t be used in multiple unrelated Assemblies.

To me there are a couple of huge advantages to using weldments. The first is that it eliminates the need to draw the profile every time you want to create a piece of W-section, square tubing, channel, etc. I use a lot of structural steel at my job, and this has saved me countless hours.

The second is the ability to add custom properties to the .sldlfp file used to create the various bodies, which will carry over to the weldment Parts as cut list properties. While I don’t do it, Material can also be assigned in the .sldlfp files.

7

The number one thing to remember with weldments: watch your parent/kid relationships! IOW, try to use a stable feature that you know won’t change much as the “base” for all the others. This helps to avoid burning down the village.

A few more things to remember:

  • cutlist props are configurable. You can use them to specify part numbers to some extent.


  • If you need to have a single body downstream, you can always use the four bi-polar magicians (Insert Part, Insert into New Part, Split, Save Bodies).


  • If you have a simple weldment part, you can achieve “single bodies” by using configurations and Delete Bodies. Remember that file props can also be configured for this scenario.

It takes a bit of finesse, but it does work well.

8

I used to use weldments a lot..
We do woodwork so it seemed a good fit, but there were so many problems that I have ditched them pretty much entirely.

They are great when you have complex male and female joints as obviously there are no external refs to deal with but..

Getting a cutlist of the entire job (which may be multiple assemblies of weldments) is a challenge.
Applying appearances that have a direction (wood) is impossibly tedious.
You can choose for cutlists to update automatically but then they will combine things you don’t want and not combine things you do.
It is sometimes difficult to reuse your work in other projects

For me the increased investment in creating an assembly is worth it… but of course the benefits depends on the work you do.

9

I’ve not done this and it kind of goes against the reason for using weldments but you can insert parts into weldments. If you have particular parts that are “Stock items” that may at some time in the future might change you can create a part and insert that part into the weldment. That part would be treated in the cut list the same as it would be treated in a BOM for a typical assembly. If you change the inserted part it changes in the weldment and all weldments it is in.

I think assemblies work better for this but as stated above you can insert parts into weldments and they act essentially the same as they would in an assembly. You would have to have the properties in the individual part you are inserting, part name, size etc. This is definitely a clunkier approach than the typical weldment use but it works.



Not sure what you mean by this. You can create sheet metal parts as part of a weldment in the same manner you would an extrusion. The only downfall is that the properties from the weldment feature does not propagate to the created feature the same way it does with extrusions.

Also not sure what you mean by “Machined bodies”. You can create as many configurations as you want showing the individual parts in as many stages as you want and you can do essentially the same thing with those bodies as you can a part in an assy.

So for instance we often have weldments with plates and sheet metal that have pre-machining/Pre bend then machined as weldment and then modifications at assy. I can do this with three different configurations and have drawings for each state plus flat patterns for the sheet metal.


This is true essentially for anything. If your weldments are of “Stock parts” that you have changes to the individual parts often maybe weldments isn’t the way to go. That being said I’d be curious how that works. So if you make 10 weldments 5 with part ABCD and 5 with Parts BCDE. You weld them all up, machine them etc etc. Now a month later you decide that “C” needs to be a different shape, do you go back to the original 10 and cut them apart and recut the original plate?

I guess I’m wonder under what conditions you would actually disassemble a weldment and rework the individual parts rather than just throw it away and make a new one. If you’re always making a new one then why would you ever need to make a change to an existing one?

10

sorry for the long post, I’m trying to be careful how much of the quoted text I cull out.

I felt the same way that inserting external parts into a weldment kinda defeats the purpose of a weldment.

I don’t understand what is clunkier about having part properties in part files used in assemblies vs assigning properties (somehow) to bodies?/parts in a weldment file. Maybe because we’re using PDM? I cannot see how one file can have more than one set of properties. Well, data card variables can be configuration specific, but I don’t think that’s what we’re talking about here.

I think I’m long past my understanding of how the individual parts in a weldment file can each get a dxf for manufacturing and how each have their own set of properties. I thought weldments were to make solid extrusions of sections along a profile with automatic trim/miter/cope and end caps if needed. What I’m trying to say is if there are no extrusions/rolled sections in the weldment then is there much point to using weldment?

I just meant all the parts that might be welded that is not formed sheet metal or rolled section, so forgings, ductile iron, machined components, weld nuts, etc.

Oh my my. So those would each be different stocked part numbers for us, each with it’s own drawing. We do very little post weld machining and none in assembly. Well, they’re not supposed to but there is occasionally metal shavings created in assembly work stations.

It is exactly as you state, weldments are stocked and made from stocked parts and they all are open to revisions through out their lifespans.

Nope, those are out the door. We have part numbers that we have been making for nearly 3 decades, some are at rev 2 some at rev 20. Some of those parts’ where used are long obsoleted some of the where used were released into production last year. Revisions are forward looking, with phase in/out dates, shipped products all have serial number tags.

Only in custom shop working on prototype or onesie-twosie orders.
We don’t make a change to the existing physical parts, we change the part design and then inventory control/scheduling and manufacturing choreograph the phase in of the new revs. Some changes demand scrapping of existing inventory of the pc parts or weldments if there are any; example, if there was a problem identified or customer demands ASAP change (then they pay for that). Most of them are running changes.

11

I use weldments, but not multi-body weldments. I use them because you can load the template with information, such as a number that references our ERP number for an iron angle, for example.

It’s also got the simplicity of driving all it’s dimensions, either from the template, or the weldment it created from a sketch.

We do create multi-body parts but those rarely have weldments.

12

Regarding inserting a Part file into a weldment, the only time I do that is in the few occasions I’ve had where nuts are welded onto a structure. I do it in those cases so they’ll show in the cut list.

13

our “weldments” (physical object) do not contain any raw stock, everything that goes into a weldment has a part number and is inventoried/stocked. Maybe this is where the gap is?

14

Most likely. Keep in mind what works for us might not work for the next. Our inventory is rather large and keeps track as far as skeletons produced by our plasma…

Plus, there’s the fact that there’s been 3 different people that tried to manage it, each their own way. I guided them the best I could, but the decision was up to them, so I held on to what I could and let them change what didn’t really affect us in the technical department. The inventory is still kind of a mess because of that.

15

In the interest of not making a mess I’m going to try a different approach.

It sounds to me like you have a situation where you have a bunch of individual pieces in stock that will eventually become part of a weldment. Each one of those parts have their own part number.

Those parts that are in stock may at some time in the future be revised/Changed. This would result in the entire weldment being revised. However already existing weldments are not brought up to this revision level.

You have additional parts, castings etc that are part of these weldments, also with their own part numbers.

If the above is correct I really don’t see anything that couldn’t be done in weldments. If 90% of your weldments are “Premade” stock items that are two complex for weldment profiles then I would agree that weldments may not be the way to go. If 25% of weldments are these premade complex items and then you hang extrusions, sheet metal etc off of it, then I would say there is probably benefit to using weldments.

Parts like castings, and other misc “Complex bodies” can be inserted into weldments. “Stocked” plates can be turned into weldment profiles or extruded in the weldment.

Thru configurations, drawings etc you can have individual drawings of any part/body of the weldment in any state you want. If a purchased/Pre-fabbed part has multiple configurations you can only create a drawing of one configuration in the weldment and that would be the configuration used when the part is inserted. Again, why you would need to show multiple configurations of an inserted part is beyond me as you can only insert the part in a single state.

Without actually looking at the application it’s really hard to say one way or the other.

16

Whether there is benefit to weldments will still depend on what the pieces are. If the pieces are plates, extrusions etc I think there is still significant benefit. If the pieces are complex bodies then there is little to no, possible a drawback, in using weldments. Placing objects, cut lists etc in weldments is not as smooth and or as robust as a standard BOM in some cases.

If you think about it, for example, lets say you are making a weldment of a bunch of castings, there is very little short of some weld bead that you’re using the advantage of weldments for. In return you’re trading off a slightly more difficult placement method, slightly more difficult method to deal with properties, BOMS etc.

The strengths of weldments likes in extrusions, machining of weldments, plates etc etc. If I’m making a base I get to create a single part and just extrude stuff. For something like a base where there is a structure with several members of similar length, instead of having several parts, I just draw sketch with the different shapes and extrude…done. Add this to the fact you have one part when you’re all done rather than 100 bits and pieces and for those cases it’s massively beneficial.

17

I use weldments rarely…just the nature of our business.
But when I do, it’s wonderful that it’s sketch-based and that I can easily switch members (got too heavy or too expensive or too complicated or too overdesigned).
Since weldments isn’t often used here, I see people that don’t use it (haven’t learned it) and draw up the assembly from scratch…painful, especially when I’m called in alter to work on it.

If inventory (or other) processes require a member component as an individual part, I would still use weldments to the extent possible to leverage the ease in definition (& subsequent changes) of any available profiles.
Create each weldment member as its own part file and if trimming is needed, then add the trimming members as you normally would to get the trim.
Then change the material of the trimming members to a near-zero mass material (so they don’t affect the overall mass calcs) and then hide them.
Each of these parts will have its own cutlist data.

Insert each of these member part files, along with the other files, into a final assembly (or subassembly) file.
Kinda like a regular assembly, but with a little bit of weldments mixed in when advantageous.

For more overall control, insert a part that has the master sketch first thing for each member part file and build off of the this (SSP-like).

Kevin

18

I don’t know how much help this info will be to you.. But I just luv the Weldments tool it is my clear favourite and most often used. And I much prefer the muti-body approach to weldment members too. It seems to me sooo much cleaner and more intuitive.
Not to mention simply easier. Even tho some of my weldment part-files can have 100’s of individual bodies.
We build Semi-Trailers and Transport equipment. So, much of what we do is welded frameworks and laser-cut plates (The Sheetmetal tool is my next favourite..)
(I’ve seen some disasterous assembly files sent to me to work with involving single bodies in separate parts all mated in assemblies all with individual drawing files for separate weldment tubes,I know it can be done reasonably successfully with SSP principles. But, I’ve not seen a good example of that yet, and the messy BOM that accompanies it with excel tables for quantities and I cannot fathom why anyone would put themselves thru that pain. Nor do I see the point in single tubes of welded steel requiring their own specific part number and drawing for assembly.)
I like that I can use weldment profiles (and also easily create my own to suit if needed) as well as multiple sheetmetal parts and machined parts all in a single file.
Individual bodies can easily be assigned different material properties too. ie. steel, aluminium, plastic, brass, rubber, glass, etc.
The weldment cut-list has all the necessary info to detail the weldment tubes for fabrication. And no fussy part numbers needed or extra drawings to track. This approach makes for much easier file management being only a single file and a single multi-sheet drawing file for fabrication.
(Tho, this does well suit our fabrication processes here and may not be ideal for others.)
The cutlist properties easily allow part number creation for sheetmetal or machined parts by code and correctly maintain all relevant quantities without any user input at all.
And part numbers automatically adjust to suit a different project when simply renaming the part (or Pack & Go the entire assembly and renaming all parts). All this information is easily reflected in a well thought out Cut-list template for ease of drawing creation.
Creating DXF Files for laser-cutting & pressing can be a little arduous but the benefits are many and some well thought out procedures and templates can greatly reduce the work needed. There are likely also Macros to assist this, but I do not use any.

“True” Mirrored Bodies work soooo much better in a “Part” file than assembly, and because I do a lot of “Top-Down Design” with most components using “InPlace Mates”, there is alway a plane tied to assy centre for mirroring bodies. And again, the quantities are ALWAYS correct.
The very best thing about it is no Mates to flip or fail with altering faces or changed beam sizes, etc. Tho, some forethought is required during part creation for future alteration or repurposing the component. But that is the Solidworks way anyway.
A well planned weldment part is truly a powerful thing of great beauty and so easy to modify for design changes too.
It is very satisfying to have dozens, or even hundreds, of bodies update correctly and have a detailed cutlist where all sizes, lengths, quantities and materials update correctly with literally no user input required. The cutlist can also even give you a “total length” of the combined lengths of any tubes of the same profile.

And, as it happens, I do repurpose weldment files often enough to know that I can save a lot of time by renaming and tweaking an existing part than by creating a new one, or tweaking an assembly. It is also a straightforward process to attach a copy of an existing drawing of the previous weldment to the newly renamed one and save a lot of drawing time too. Perhaps it is fortunate for me that much of what I do is a varition on what I’ve done previously. We often build bespoke units and any multiple builds are quite often in small quantites, from 2-10)

Combined with the other great tools that accompany the weldments environment like Trim, End-Cap, Gusset, and Boss Extrude and the other direct editing and “Insert Part into Part” options also available it makes Weldments a very useful and powerful tool for the creation of very large and easy to manage welded components indeed.
Note: Tho honestly, “Insert Part into Part” can be a little clunky and does not always achieve the desired end result, it is very functional for beginning a welded structure around an outsourced/purchased component.

I do not ever use the Split or Save Bodies commands.. I’ve not seen or experienced a need for it..

In summary, I would highly recommend you look into the possibility of making full use of this great tool..

I have not had much chance or need to get far into Structure Systems as yet.. Tho, I suppose that day will come. I am not looking forward to the weldments tool being discontinued.. Are the rumours true..?!?!

19

Damo I use a very similar approach. https://www.cadforum.net/viewtopic.php?f=33&t=74 is a macro I use for exporting DXFs. It exports all of the flat-patterns in a Multi-body part or assembly to a folder created by the macro. If you know a little bit about programming you can change the naming scheme of the DXFs. This is one of the most useful macros I currently have, thanks to artem.

20

Thank you Damo for the detailed response. It’s packed full of good bits of usage practices.

Thing is, most of what you explained pretty much underscores the reasons we haven’t used weldments in the past and likely won’t start. It would be neat to be able to use all those slick modeling methods; so I try to look into them every now and then.

When I worked at a food grade stainless steel fabrication shop each project was it’s own set of parts and they didn’t have part numbers, only the common purchased parts would have a part number and those were never revised. There weren’t really revisions, the customer would make changes all the time, but edits made after the prints hit the floor were considered “as builts” and did not get priority as that same tank would never be built again. I did very little CAD work there but just enough to really appreciate top down practices or modeling a whole tank in one part file.

On the other side of the spectrum is where I live now, every part has a part number and goes through production release process and is then stocked and inventory tracked. Majority of the pc parts are used in multiple weldments, each of those with their own part numbers, inventory, and where used. Any model that gets a part number and released to production will live on as long as there’s orders for it and be reused in new places and have it’s own revision tracking for unknown number of years. We just don’t have any “one and done” projects. We don’t even categorize parts by project or have any project number on PDM data card variable. We have projects, but the project has a limited lifespan, it’s considered complete once all the parts are in production and first runs are complete and the product is fully released into production. At that time the “project” is complete and archived but the new part files live on, being manufactured, reused and revised for ever. I cannot see how to do that if the parts don’t each have their own file.