Question about elastic shell element

[luckypants]

Dear STKO Team：

1. I build the shear wall by ShellMITC4 with Elastic Membrane Plate Section. There is an error when I write input file. The following picture is the error message. Here is my 7-story model. How could I solve the problem?

2. Then, I find there are two commands to build the shear wall. One is Planar, and the other is Face 3/4. What is different between them?

Any advice and helps that you provide are highly appreciated.

Best Regards

[STKO Team]

That error is simply saying that you are trying to use a 4-node Element Property (ShellMITC4) with a triangular mesh.
Go in the mesh tab, click on mesh control, select faces/structured/quad/linear, then select all your faces and press assign -> done.

This will tell STKO to mesh all the selected faces with a structured mesh, with quadrilateral elements, and they should be 4-node elements because of the linear order of interpolation.

Then you may want to refine your mesh (for shells) because 1 element per wall is definetly too coarse.

[luckypants]

Dear STKO Team：

Thank you very much. I follow your steps to revise the model, and it works now.

But there is still the problem in my model. After I finish the modal analysis, the result is weird.

Does using 1 element per wall cause the error? How could I refine my mesh?

How could I solve the problem?

Any advice and helps that you provide are highly appreciated.

Best Regards

[STKO Team]

Does using 1 element per wall cause the error?

No, the error you have is due to the fact that your model is singular. Probably you modelled your walls as separated geometries, i.e. not attached to the beams. If that is the case, you need to either attach them to the beams using the "Merge" command, so that they will result into a single geometry (In this case they will be continuous in both displacement and rotations), or you can link walls and beams with equalDOFs if you want to connect them only in some DOFs

How could I refine my mesh?

Just go in the mesh tab, and change either the global mesh seed, or refine the mesh seed on some specific edges using the "Edge Seed" command.

If you attach your .SCD file here (zipped) we can have a look

[luckypants]

Dear STKO Team：

I see. Now, there is another problem I want to ask.

Will the result be weird if I don't refine my mesh for shells(I still use one element per wall)?

Could it influence the result of the analysis if I use a coarse mesh(one element per wall)?

Then, the following is my model. Could you help me to solve the error?

Thank you very much.

Best Regards

[STKO Team]

As I said in the previous post, it is singular because beams and walls are modelled with separated geometries. Keep in mind that if 2 geometries are separated (and not connected with any kind of kinematic constraint), also the FEM model will be separated, and in your case, the walls are not attached to the beams and so the system is singular since the walls are un-constrained.

I used the following steps to join walls and beams:

Senza nome.png (248.51 KiB) Viewed 4945 times

After the merge command, make sure all properties are still correctly assinged. In fact, the merge command will join, for example, the edge of the face, and the overlapping beam. Now, only one of them (the beam) has a property. But since the CAD boolean operation uses its own random order, it may happen that the resulting joined edge does not keep the old property assignement.

Note that I also refined the mesh of the wall. To do this, I first used the EdgeSeed command, then I selected all the edges of the walls, and I chose a mesh size = 0.5. Finally press Assign and Done. Finally mesh your model.

Senza nome2.png (45.54 KiB) Viewed 4945 times

Note: when you refine your model, it might be too large for a -fullGenLapack. So I removed that option in the eigen customCommand, because the default goes with the Arapack Solver which works for sparse matrices.

I also added the record command after the modal analysis otherwise the MPCO recorder will not record anything

Here is the modified file:

sevenstory.zip

(71.09 KiB) Downloaded 212 times

[luckypants]

Dear STKO Team：

I solve my problem. Thank you very much.

Then, there are two question I want to ask.

1. What do "scaleDrilling" and "updateBasis" mean? I don't see the explanation in OpenSees manual.

2. I did the modal analysis to compare the coarse mesh (one element per wall) with fine mesh (used the EdgeSeed command). The second picture is the result of using fine mesh, and the third picture is the result of using coarse mesh. I found the result was different. So, what the reason make this difference? Will the result be
inaccurate if we use the coarse mesh?

Any advice and helps that you provide are highly appreciated.

Best Regards

[STKO Team]

1. What do "scaleDrilling" and "updateBasis" mean? I don't see the explanation in OpenSees manual.

• updateBasis: It is not documented but it is in the standard OpenSees code. If you check it, it will use nonlinear geometric analysis (large displacement and rotation) for those shell elements.
• scaleDrilling: It is not in the standard OpenSees code. It is only available in the OpenSees version pre-compiled by prof. Tarque. It basically scales the artificial drilling DOF (in-plane rotation for shells) stiffness, because the default value of 1, makes the element over-stiff in membrane-domanited problems.

2. I did the modal analysis to compare the coarse mesh (one element per wall) with fine mesh (used the EdgeSeed command). The second picture is the result of using fine mesh, and the third picture is the result of using coarse mesh. I found the result was different. So, what the reason make this difference? Will the result be
inaccurate if we use the coarse mesh?

Of course the results are different. Keep in mind that FEM gives you an approximate solution (due to discretization errors). The finer is the mesh, the least discretization error you have, thus the results will be closer to the exact solution. There are few simple cases in which just 1 sigle element per structural member is enough for obtaining the exact solution. For example linear beams with constant cross sections in linear eleastic static analysis. For the shells, this is not the case. Moreover, even the elastic beam does not give you the exact solution in eigenvalue analysis. Immagine a fixed-fixed beam... both nodes have all 6 DOF fixed. If you discretize it with just 1 element, how many modes will you obtain?
Zero, because you don't have any free DOF with masses... But if you discretize it you will see a result.

[luckypants]

Dear STKO Team：

I see. Thank you very much.

Best Regards