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.

 

[StructuralFEA]

rb1957,

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.

 

[StructuralFEA]

I don't know why, but FEMAP doesn't like the extended pipe past the tube and asks whether it is ok to add the solids as non manifold. Any idea why? Thanks.

 

[rb1957]

you're modelling the pipe as a 3D solid now ? (it worked previously as 2D plates, yes?)

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 ?

 

[StructuralFEA]

No. I'm still modeling the pipe as 2D. I am breaking the pipe/cylinder at the tube by using the command" Geometry, Curve-From Surface, Intersect. The I select the first as the pipe and the second as the tube. Thanks.

 

[rb1957]

ok, that sounds ok, breaking the cylinder at the square tube. then you mesh only the surface you want (outside of the square tube). what is FeMap complaining about ?

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 ?

 

[StructuralFEA]

Thanks.

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.

 

[StructuralFEA]

Second File:

 

[StructuralFEA]

I just saw that I could add the surfaces as: Geometry, Surfaces, Non Manifold Add. Is this a better way or the right way of adding the pipe and the tube?
Thanks.

 

[StructuralFEA]

OK. It turned out that adding surfaces to surfaces of solids is a non-manifold operation, as I just got the answer from technical support. It is ironic that the program just adds the surfaces without "complaining" when there are only two parts as mentioned above. Anyway, I am currently running it, and will let you know. Thanks.

 

[rb1957]

"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)."

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 ?

 

[StructuralFEA]

Thanks.

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.

 

[rb1957]

it'll mesh the two pieces with a consistent mesh. then do a "coincident node" check (under tools/check) and that should identify the coincident pairs are remove one, then the two pieces will be joined. I suggest saving the model before the coincident node removal in case you want to revert to this model (easily).

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

 

[StructuralFEA]

I've tried, and I've even started the model from scratch. Ultimately, NASTRAN gives error messages about "All plate elements must have the same face ID", and "User fatal message 4297" about quad elements. I believe that this is de to the complex geometry at that "round" corner of the tube where the tangent to the face changes as the "corner" curves away from the previous surface.

 

[StructuralFEA]

I am giving it one more try. I have just added the pipe to the tube (as non-manifold) while meshing as discussed before, and NASTRAN didn't complain. It's currently running. Let's see whether it solves all the way. Thanks.

 

[StructuralFEA]

rb1957 (Aerospace),

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.

 

[StructuralFEA]

rb1957 (Aerospace),

Here is the file with the stresses based on glue.

 

[rb1957]

I notice that the glue model has a finer mesh ?.

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 ?

 

[StructuralFEA]

Yes to the finer mesh, and to the stress discrepancy in the "glue" 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.