FEA Model
FEA Model
(OP)
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.
Thanks.






RE: FEA Model
another day in paradise, or is paradise one day closer ?
RE: FEA Model
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.
RE: FEA Model
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 ?
RE: FEA Model
another day in paradise, or is paradise one day closer ?
RE: FEA Model
RE: FEA Model
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 ?
RE: FEA Model
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.
RE: FEA Model
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 ?
RE: FEA Model
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.
RE: FEA Model
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 ?
RE: FEA Model
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.
RE: FEA Model
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.
RE: FEA Model
RE: FEA Model
RE: FEA Model
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 ?
RE: FEA Model
RE: FEA Model
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.
RE: FEA Model
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 ?
RE: FEA Model
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.
RE: FEA Model
I isolated the pipe and tube. I meshed it again, did not use glue, and it worked. Now, I will try it on the whole model.
Thanks.
RE: FEA Model
RE: FEA Model
how are you breaking the cylinder at the square tube ?
there is a geometry/solid/intersect command ...
another day in paradise, or is paradise one day closer ?
RE: FEA Model
RE: FEA Model
how can you mesh a surface with 3D elements ? (unless I didn't understand something).
another day in paradise, or is paradise one day closer ?
RE: FEA Model
FeMap doesn't like it when, after breaking the pipe at the tube (Please see attached file), I try to add the pipe to the tube (to make them one piece per your suggestion so that I don't have to use glue). It gives me the message "OK to allow this operation to result in a Non-Manifold Solid?" (Please see attached file). So, in essence, I am one step away from making it work. Ironically, when I use only the pipe and the tube (after doing a save as, and deleting all other parts of the model), FeMap accepts the Add operation without complaints! The command I used to add the pipe and the tube is: Geometry, Solid, Add, and then I picked the pipe and the tube. I realize that I used the "Solid", but this is because I could not find any "Add" command under midsurface. Maybe this is what's causing the complaint. Please advise. Thanks.
RE: FEA Model
RE: FEA Model
Thanks.
RE: FEA Model
RE: FEA Model
I think my meaning was lost in translation ... I didn't mean to make one geometry solid out of the two 3D volumes. I meant if you mesh both geometry volumes at the same time the mesher understands that you want a consistent mesh across the boundary ... I think.
another day in paradise, or is paradise one day closer ?
RE: FEA Model
I see. That makes sense. You are right in that the program DOES understand that you want to mesh both of them together and yields the skewed elements near the interface. However, when it comes to connections, if you don't use glue, and you have two separate parts, i.e. the pipe and the tube, do you have to do anything in terms of connections or does the program "understand" that the stresses are to be transferred from node to node without glue? I believe the latter is what you meant. Thanks.
RE: FEA Model
another day in paradise, or is paradise one day closer ?
RE: FEA Model
RE: FEA Model
RE: FEA Model
I finally got it to work! As you and I know, both FEMAP and NASTRAN can be pretty finicky! The results are similar to those I got by using glue, though a little better, i.e. lower stresses at the interface. Interpretation of such stresses is needed irrespective of the method used. Please see the attached figures for the comparison between the two methods.
Thank you for all your help. I have learned a lot throughout the process.
RE: FEA Model
Here is the file with the stresses based on glue.
RE: FEA Model
In the glue model, just above the box, there looks to be a discontinuity in the mesh (with a node feeling red on one side and ice cold blue on the other) ?
I suspect that the finer mesh is getting closer to the Kt problem.
another day in paradise, or is paradise one day closer ?
RE: FEA Model
Would you please explain what Kt stands for?
I ran the model with the "pipe surfaces broken at the tube" with the same mesh size as the "glue" model, i.e. both models have a shell element size=0.125. An apple-to-apple comparison of the two methods shows that there is no consistency or trend in predicting a pattern. For example, the glue method yields a lower overall model stress (179.883 ksi), whereas the "compatible-node" method yields the lower pipe stress at the tube (upper pipe at left tube, as seen)(164.651 ksi). Of course, additional inconsistencies can be seen when comparing the 0.125 elements with the 0.25 elements.