FEA Model

[StructuralFEA]

I have modeled a vehicle carrier using solids and shells in FEMAP. I refined the mesh for the shells twice, and the solution converged, i.e. became asymptotic. However, I find the last few elements near the interface between a round HSS, and a square HSS to be have very high stresses. How do I make sure that these stresses/numbers are correct? As you can see, I have already run a convergence analysis. I have also compared the minimum, average, and maximum nodal Von Mises stresses to see the percent difference. Despite convergence of the analysis, the difference between minimum and average stresses, or between average and maximum stresses, is sometimes as high as 28%. Are these stresses reliable?
Thanks.

 

[rb1957]

how skewed and distorted are the elements ?

another day in paradise, or is paradise one day closer ?

 

[StructuralFEA]

Thank you, rb1957!
LOL about the "another day in paradise"!

I have attached a file displaying the Tri6 elements I used in the latest run. Prior to that, I had used quad elements. Please let me know whether this is what you meant.
Thanks.

 

[rb1957]

that helps ... a detail view of how the side of the rectangular tube meshes with the cylinder. I suspect the cylinder has a regular mesh but the square tube has a distorted mesh, to suit the cylinder.

right on this interface, 2D elements are going to be very confused.

look like a 90deg corner ... no fillet ?

How, physically, are the two tubes joined ? continuous weld ??

another day in paradise, or is paradise one day closer ?

 

[rb1957]

looking more carefully at the intersection ... how are the two tubes joined, in the FEM ? the meshing doesn't seem to be consistent between the tubes ??

another day in paradise, or is paradise one day closer ?

 

[StructuralFEA]

Thanks. You mean that the nodes of the meshing on the tube do not coincide with those on the cylinder, right? The answer is yes, and I had the same comment to the FEMAP technical support. It is OK to do that, as the tube and the cylinder are attached with glue all around the interface. I researched the maximum gap distance in the model, which is generated due to using shells instead of solids, and used the maximum search distance for the glue.

 

[rb1957]

1) does the round tube penetrate the square one, or butt up to it ?

2) how uniform is the mesh over the glue interface ? I think this might affect how well the glue works.

3) is the glue rigid or finite stiffness ?

4) how well does this represent the real world ?

another day in paradise, or is paradise one day closer ?

 

[StructuralFEA]

1) The cylinder does not go through the tube.
2) The mesh seems to be smooth from the picture.
3) I used the Glue Contact, which is rigid.
4) It should be a good representative of the real world.

I have noticed that the stresses are higher near the "round" corners of the tube. I believe that this has something to do with it, as the stresses at the top and bottom of the cylinder do not have those stress concentrations. I ran some hand calculations by hand, as I have a strong background in buildings, and the results are very close to those at the top and bottom of the cylinder, but not close to those seen in the picture.

 

[rb1957]

1) 'k
2) what I meant was are the nodes (on the square tube) uniformly distributed over the contact area (is the round shape reflected in the square tube mesh ? I don't think so ...) or are the square tube nodes wherever they occur in the square tube mesh and you're joining a bunch of nodes in the square tube that just happen to fall within the area of the cylinder ?
3) I think it'd be better to use a finite stiffness glue (if you can).
4) the real world is rarely rigid ! I imagine that there is a weld between the two tubes ?

I imagine we're looking at a von Mises stress ?

another day in paradise, or is paradise one day closer ?

 

[StructuralFEA]

Thanks.

I had asked technical support that question and their answer was that if I used a glued contact then I wouldn't need to match the nodes/mesh at the interface. In fact, the mesh cannot be matched, as I modeled both the tube and the cylinder as shells. As a result, the interface is between a "curve", i.e. the cylinder perimeter, and the tube face/surface. Therefore, only the nodes can be matched to accommodate the interface between the two shells. I will ask them again and try that. It may improve the solution, which I had suspected before they gave me their answer.

Yes, they are welded, and yes we're looking at Von Mises Stresses.

 

[rb1957]

you can always tailor the mesh to suit the structure. you should be able to project the cylinder onto the square tube, mesh the square tube around this, mesh the interface region with the same pattern as the cylinder. the elements won't be regular (hence my original question "how distorted are the elements?"). this way you can join the two pieces directly, without glue.

This may not be the problem, von mises can be a difficult stress ... what's the loading ? how are the normal stresses ? (what you'd expect for the load?)

another day in paradise, or is paradise one day closer ?

 

[BadgerPE]

With my limited FEM background, I would tend to agree with rb1957 here. I don't know the specifics of the program, but I would think you need to have the nodes from your round pipe align with those from your square tube.

Sorry. I meant to add the following....I would create a second model such that your nodes for your round are shared with nodes from the tube. If you analyze the second model and get the results you are expecting, then maybe you can have the discussion with tech support for your software. It wouldn't be the first time a program designer had a bug in the system.

 

[StructuralFEA]

Thank you both.

I guess it was "another day in paradise"!

The PLM forum site had the same answer as the technical support for FEMAP, which is when "glue" is used, then there is no need to match the nodes and/or mesh at the interface.

After going through a lot of work, I finally discovered that there is a gap between the round HSSS (Hollow Structural Steel) and the square HSS. Please see the attached files. It turned out that this is the way they do it in the real world for car carriers. I know from my building design background that the gap would be filled with "full penetration weld". This explains the stress concentration around the gap, as the model I received does not have welds in it.

The only thing remaining here is that I ran the model both as all solids, and as mixed solids and shells. The former yielded lower stresses at that specific location. I am thinking that it may have something to do with the gap around the "round" corner when the round HSS and the square HSS are represented as shells. Or it could be attributed to stress "lockup" in the all-solids model.

 

[StructuralFEA]

Next attachment

 

[StructuralFEA]

Fourth attachment

 

[rb1957]

yes, gaps in the corners would be a problem. but I think your glue connection is doing the work of a weld, although maybe a little too constrained.

in your geometry model, I'd make the cylinder penetrate the square tube. I'd then break the cylinder surfaces at the tube surfaces. at a first stab at it, I'd model the thin walled tubes as 2D plate elements (it looks like you're using 3D TETs). several advantages to using 2D elements ...
1) the geometry is easier to work with,
2) you can allow the cylinder to penetrate the square tube, break it at the tube, then mesh all the surfaces at once (so they'll understand their intersections and apply the same node on both sides and so you won't need glue).

another day in paradise, or is paradise one day closer ?

 

[Ron]

Animate the model and see if it moves the way you expect.

 

[StructuralFEA]

rb1957, thank you.

Yes, however, I am not sure that the glue is taking care of the gap. The reason is that there is a stress concentration around that area. I have, in fact, used 2D elements for both the tube and the pipe. I had also run the model with all solids prior to that. The 2-D elements reduce the number of elements and nodes, which helps with solution time.

I used the "extend" command in FEMAP to allow the pipe to penetrate the tube. I used a nominal distance of 0.125 which is the element size I assigned. I am currently running it, but I kept the glue in order to compare with the previous results without the extension/penetration (while keeping all other factors the same).

Would you please clarify what you meant by "break it at the tube"?

Ron,

Thank you.

It does not seem that I can animate the model, as the solution is linear. Please let me know whether there is still a way of animating the model. I had already looked at the deformed shape which was in agreement with what was expected.

 

[rb1957]

you're using a geometry model (under the analysis model) defining the surfaces.

So starting with the square tube, and add the cylinder ... both as surfaces. extend the cylinder into (or thru) the square tube. then modify/break or geometry/curve-from surface/intersect should understand where the cylinder intersects the square tube, and will assign different surface numbers to the different surfaces. mesh the surfaces that are real (ie don't mesh the cylinder surfaces that are inside the square tube).

I'd've thought glue worked like a rigid element, joining two defined sets of nodes (and so it can handle the gap between them ... though it might be producing rubbish). but I could be wrong ...

another day in paradise, or is paradise one day closer ?

 

[StructuralFEA]

Thank you.

I succeeded in extending the pipe past the tube, and getting those "distorted or skewed" elements. I did not mesh the inside part as you suggested, however this caused issues. Please see the attached file. Thank you.