weldments

[Tenkan]

In the past I worked primarily with parts or small assemblies but not weldments, now I work at a company that does a lot of weldment assemblies and so I’m struggling to learn the best flow for solidworks design.

Ideally what I think I want is to build the assembly model from the part models, but the problem is solidworks does not fill in the welds. In my case, we use extra large weld gaps/prep in my experience so that kinda compounds the problem that and I am not experienced with the weld features in solidworks, it doesn’t seem to be intuitive and they don’t even show up in the dwg. Also, assembly features seem to lack functionality in solidworks for post assembly processes… for example, cut-extrude is limited to blind, thru all, and mid plane. Anyways, what I have been doing is breaking the links to the parts and editing the part model at will to remove weld prep and add any final post weld machine cuts/features etc. to the assembly model.

What I need is to be able to create a final drawing of the assembly, but want the assembly to update when the parts are revised.

Is there a best method I am missing?


lightweight, cheap, strong... pick 2

 

[MikeHalloran]

I just want to see what's suggested; I went through the tutorials, but couldn't make weldments work for what I was trying to do.



Mike Halloran
Pembroke Pines, FL, USA

 

[Jboggs]

You're building a weldment from individual parts? You're basically creating an assembly file, not a part file. Wrong!

In my opinion weldments is one of the most powerful and useful of Solidworks tools. But it is not intuitive, and not user friendly. Take all the tutorials you can find on how to create weldments. One thing you will notice is that when you declare a part to be a weldment it automatically sets the "merge" option on any new features so that they are not merged with previous features. That means they are separate bodies. That single fact will haunt you every step of the way as you learn weldments. It is critical for most feature tools such as patterns, mirrors, etc. For example, to create a mirror part you must select "Bodies to be mirrored" instead of "Features to be mirrored." You will eventually learn to repsect the differences between merged "features" and non-merged "bodies".

It has some really neat weldment tools like Trim and Extend for coping cuts, and End Caps for hollow tubes. And yes you can add weldbeads, including their notations, if you need to. (Personally I rarely ever include weld beads or weld notes unless there is some specific reason or need to. Its a matter of choice.) SW handles weld beads as separate bodies that are NOT included in the cut list. So if there is some part you don't want in the cut list, just declare it to be a weld bead.

It even sets up the configurations so you can easily show the "As welded" and the "As machined" conditions separately. (Learn configurations inside and out if you haven't already.)

You can easily create fabrication views of individual parts using the Relative View tool. Again, consult the tutorials.

Probably the most difficult thing to learn is how SW creates the Weldment Cut List. But once you learn how the properties and configurations affect it, you'll never look back.

 

[CADFlyer]

SW is set up to create a weldment “assembly” at the part file, not as an assembly file. It sounds confusing, but it starts to makes sense as you go through the SolidWorks Weldments tutorial. If you create the models per the tutorial, it should solve a lot of your issues.

That being said, our company does not let us use the SolidWorks weldment functionality (long story), so we have to do it as you are describing, and it’s a PAIN. We have to create an assembly file & drawing for each extrusion piece just to add a machining operation (holes & cuts).

 

[davidinindy]

A couple shortcomings of Solidworks weldment functionality I've noted.
Gussets and endcaps don't fill out properly in the cutlist.
If you have common parts that are used often in weldments, there is no way to add them in, and have them stay linked to the original part, that I've figured out.
That being said, we use weldments every day, and it works great for what we build.

David
Check out my professional profile and connect with me on LinkedIn.

http://lnkd.in/fY7-QK

 

[Jboggs]

David,
As far as inserting standard parts into weldments, I do it all the time. I'll add a weld-on eye bolt I downloaded from McMaster Carr, or weld a nut over a hole for attaching something with a screw, or insert Helicoils or Keenserts for stronger threaded holes.

Running SW2012. Under the Insert pulldown menu, look for the "Part" command. You browse to select the part file you want and click in the graphics area. You can select what properties of the file you want to import. I usually only import solid bodies, planes. threads, and maybe sketches. The part is shown highlighted in yellow, and you'll see a Locate Part dialog under properties. Here you add mates just like in an assembly. (That's why I import its planes, for easier mating.) The part is added to the feature tree. Under that feature you'll see its bodies, planes, sketches, and an item called Body-Move/Copy, under which you will see the mates you added. You can go back and add or edit the mates any time. Its been pretty handy for me. The file is still a part file, not an assembly. I don't think it is dynamically linked to the source part, so changes there won't show up in the destination part.

 

[CorBlimeyLimey]

A part inserted into another part is linked to the original file. Changes made to the original will be reflected in the inserted part.
If you right-click the inserted part and select Edit In Context, the original file will be opened for editing.
Also, with the original part open, if you right-click the inserted part and select List External Refs, you are able to select a different configuration.

 

[ShaggyPE]

+1 to what Jboggs is saying.

It sounds like OP is doing a weldment the way we had to do it pre 2008.

-Dustin
Professional Engineer
Pretty good with SolidWorks

 

[Tenkan]

Thanks everyone for the tips, I'll bookmark this thread as I play around with Solidworks and give the tutorial a try. It sounds like no matter, the weld features in SW is not the most intuitive but it makes sense to utilize it if I can. A while back I played around with the tutorial but got frustrated, so its a slow work in progress here for me.



lightweight, cheap, strong... pick 2

 

[davidinindy]

I stand corrected. I always thought since there was no "open part" option when you right click the inserted part, that it lost its reference. Never really looked any deeper into it than that though.
We do this mainly with weldnuts, but sometimes standard brackets, etc. get inserted into weldments also.
Is there a trick to getting the cutlist to fill out for these inserted parts?
How about getting the gussets and endcaps to fill out in the cutlist also?

David
Check out my professional profile and connect with me on LinkedIn.

http://lnkd.in/fY7-QK

 

[Jboggs]

The only reason the cut lists automatically fill out for standard welded sections is that the weldment profile files it uses come with those properties defined. Gussets and end caps do not use predefined files, so there are no predefined properties. Same for inserted parts. You just have to fill the cut list properties out manually. (I know that's an ugly word and I apologize for using it but I just had to!) You do that in the model, right? You don't try to fill them out in the drawing, do you?