Weldments in Solid Edge

[eric316]

Hi,

We currently use SolidWorks and our products often consist of weldments upon which detailed FEA analysis must be run. SW has a weld bead feature that allows you to select adjacent surfaces of two parts in an assembly and it will automatically create a weld bead. Although this weld bead wizard has options for selecting just about every weld you can imagine, the only one that I could get to work is a simple fillet weld. This is fine for most of the stuff we do.

I know that Solid Edge also has a weldment feature and I have seen it demonstrated. From what I remember, instead of selecting two adjacent surfaces of two parts in an assembly you can just select the edge (line) formed where these two parts meet, correct? In SW, you can only create weld beads between two parts at a time. What is it like in SE? Can you select several edges and follow them around multiple parts to create a more complex, continuous weld bead? Can SE only do fillets to or can it do other types of welds?

Question number two. In order to create our detailed FEA's I often need to create these individual weld beads in SW and then create a "joined part" so that I now have a single, complex, lattice-like, weld bead. Then I suppress all the individual beads that I used to create this joined part. Then I check the assembly for interferences because the FEA cannot have interferences. Often times, I need to make oblique cuts in the corners of some of the plates to clear a fillet weld that is passing through the area. Check for interferences again, etc... As you can imagine, setting up these assemblies for FEA can be a very tedious process. However, it does result in a more accurate analysis of what's really going on.

Whew!!! So my question is...knowing how we prepare assemblies for FEA, can Solid Edge do it faster/easier??? Please say yes! If so, how??? Please be detailed. I would like to understand the weldment module of Solid Edge much better. I guess I'm just hoping there is something out there that can make my job a little easier.

 

[kjoiner]

Eric,

I'll try to provide some more information on the weldments, but someone else will need to provide the details on the FEA aspects.

On version 18, weldments can now be part of the assembly file. On previous versions, you created a separate weldment file and brought in the assembly. Now you just check a box in the assembly that says it's a weldment and SE recognizes the assembly as a weldment and also adds another tool bar that allows you to create different kinds of welds such as fillet welds, groove welds and skip welds. There are probably advantages and disadvantages to either method, but the new method keeps the file count down.

In Solid Edge, you select the faces you want to join and if there is a continuous path, SE will run a bead around the joint. That works for fillet welds and skip welds.

For groove welds, you pick a base face and a target face for the weld. You mention picking a line - for groove welds you can can pick lines that define the top and bottom of the weld bead for both the base and target faces. That is useful because one part may be offset from the other and by picking a start and stop point, SE will carry the bead up to that edge. You can also define how the bead is projected from the base face to the target face. That is useful where you could either leave the bead flat against the two parts or build up a fillet.

Solidworks and SE sound similar as far as picking only two parts at a time to weld. I've got a frame I'm experimenting with where I've got two tubes intersecting another tube. I'll try running a weld around all three parts at the same time and let you know the results. I can't say whether or not it will work, but your question makes me want to try it out.

Kyle

 

[kjoiner]

Eric,

I made a frame where three tubes are perpendicular to another tube. I made the "base tube" the base face and selected the outer face of the three tubes the targets and SE ran fillet welds around the all the joints. The key is that the base face is common to all three legs. Later I'll try multiple base faces.

Kyle

 

[fredericmenage]

Hi,

To add to Kyle's answer, you can also model more complex shapes in the assembly using the modelling commands protrusion, revolved protrusion and especially swept protrusion (along path) and then label one edge of that protrusion so that Solid Edge recognizes this "body" as a weld bead. You can even make that new weld a stitched one.

Otherwise, all the weld commands (including the method described above except swept protrusion) support more than two input surfaces for the same weld.

For FEA, which software do you use ? I would make sure that it is up-to-date with Solid Edge in the sense that it can recognize the weld beads as solids to run the analysis on them.

HTH,

Fred

 

[eric316]

Thanks for the input.

Kyle, are the three tubes that intersect the main tube close together such that the weld bead created is actually one weld bead or are there actually three seperate welds?

Fred, right now we're using Cosmos with SolidWorks. Modeling weld beads using the regular feature commands is what I have been doing too when I need something more than a simple fillet weld.

In SE, if you have seperate weld beads that touch or run into each other, can you create one single joined weld bead and suppress all the individual beads?

Thanks!

 

[fredericmenage]

Hi,

I don't think there is a way to merge weld beads that are joining. They will remain separate features.

For the technique I described, just to clarify, it's not just modelling a weld bead as a part. It's actually modelled as a weld bead thus being represented with the proper color and calculated (weight,...) with the proper material.

Fred

 

[eric316]

Hmmm, if the weld beads are seperate parts then they will most likely have interferences in the assembly. Of course one could make in-context cuts in each weld bead to get rid of these interferences but that sounds tedious. The FEA will not run with interferences.

 

[kjoiner]

Eric,

I should have clarified my shape. It looks like a capital "E". The legs are far enough apart to make them separate, but I did create the weld beads in one operation by selecting the vertical part of the "E" as the base face and the outer perimeter faces of each of the legs as the target faces. I could also make them in 3 operations. There are probably advantages and disadvantages to each method. The weld beads in Solid Edge are not separate parts but are actually considered what are now called "assembly features". They are in the same category as holes created in the assembly or as Frederic mentioned, other features such as various protrusions. In a similar fashion, the pieces of tubing are not separate parts either. In the frame module, you draw simple sketches of the tube paths, and then select profiles from a library. Solid Edge then takes the little chunks of tubing and stretches them to fit each path. In reference to your FEA process of removing the weld beads, although I have not tried it, you can probably use the "simplify" command on the assembly and suppress the weld beads.

Kyle

 

[eric316]

Thanks Kyle.
In SE, say if I want to make my own weld bead as a part by sketching/extruding/revolving/etc, rather than using the wizard, can I then join or merge multiple weld beads and form a single part file?

 

[kjoiner]

Eric,

Yes, I think you could do that. If you want to create an entirely separate part, you could create a new file and then use interpart linking methods such as including faces or edges etc. to create the paths for the weld beads. Then you could suppress them from the assembly or check for interferences between the beads and other parts. That's something I've never tried but it's basically like creating any other part. Going back to my comments about simplifying the assembly, its intended purpose is to show exterior faces when working with large assemblies with lots of internal parts that may be hidden most of the time and would drag down the system. As far as merging weld beads, they would be independent parts.