LayeredShell for shear walls

[nelsonlopez5484]

Hello everyone,
I am trying to model a simple shearwall, using a SectionLayeredshell, but there is no convergence at all for a nonlinear analysis (push over and cyclic), I am following the next procedure for the creation of the layered:
1_materials.nD.PlaneStressUserMaterial
2_materials.nD.PlateFromPlaneStress
3_materials.uniaxial.Steel02
4_materiasl.nD.PlateRebar (Longitudinal and transverse)
5_sections.LayeredShell

Then, I used the Element properties 'shell.ASDSheelQ4', and construct the analysis steps for a vertical load (compression in the top of the shear wall), and then, a pushover. The analysis completes well for the vertical load, but once the push over is starting, the analysis gets stuck in the first iterations, and finally, it is aborted.

At this point, I tried to change the Element properties, using a 'ShellNLDKGQ,' and the same happens.

I do not know what I am doing wrong. Does any of you have any suggestions or has something similar happened to you?

Thanks in advance.

[marafini.f]

Dear Nelson Lopez,

something really weird happens to your model, look:

Cattura.PNG (104.79 KiB) Viewed 4117 times

I don't think you wanted to create that kind of boundary condition. I didn't get the use of the equalDOF you wanted to make. Usually, we create interactions where we want to assign specific internal boundary conditions between disjoint geometries, but you only have one geometry. If you want to make the top shell portion very rigid you can just assign an elastic rigid material. Try to review this and rerun your model.

Moreover, I would suggest you to do the following changes:
- create an out of plane boundary condition, you are doing a 2D problem with 3D elements
- use a linear timeSeries for the pushover
- increase the rigidity of your actuator shell

You may have reasons why you picked different options so please let's discuss it here further if you wish
Here it the model I modified and the curve obtained.

2.PNG (52.22 KiB) Viewed 4117 times

TEST_1.zip

(140.01 KiB) Downloaded 230 times

Enjoy your modelling.
Francesca

[nelsonlopez5484]

Dear Francesca,

I want to thank you for the fast reply and for taking your time and took a look to my model; now the model is running better than before, still with some convergence issues, now in the cyclic analysis, but, it is running!. I have already done your suggestions and the model is performing well.

Thank you very much!.

[marafini.f]

You are welcome!

[nelsonlopez5484]

Greetings, it is me again,
I have followed your recomendations, and the model has improved; but, still has convergence problems, and I do not Know the reason but I think that this issues are related with the rigid member (I have changed it into a triangle, following the tutorial of Dr Petracca), but the model still does not converge. I have tried to eliminate the rigid triangle and put the loads in the top edge of the wall (now as edges forces instead nodal), but the result is even worst.
My supervisor recommended me to use a truss model instead this LayeredShell, in order to discard if the problem is the element property, bu I cannot find the element that I need, which has a name in opensees that I cannot find in STKO, but I think, it is the figure 3 (Attached), and if it is, I could not find the components for concrete (I have created an uniaxial concrete material but it does not appear in the concrete list, in order to select it), for instance.
I have attached the model, and some figures with the names of the components for the truss model.
I will appreciate if you can help me.
Thanks in advance.

[marafini.f]

Dear Nelson,

I think the problems in your model are due to the PlaneStressUserMaterial. We had problems with this material before.
We made an attempt using DamageTC3D, there are a lot of resources on it on this forum too.
Here is a model with this material, we defined it just once to be faster.

TEST10.zip

(167.56 KiB) Downloaded 215 times

If you want to use the truss model it can be done. You need to define a ConcretewBeta uniaxial material, you cannot use other concrete materials for it.
If you want to follow this approach instead of the shell make an attempt and then send the model if you have problems.

Francesca

[nelsonlopez5484]

Dear Francesca, thank you very much for the quick response.

I had used the user material for concrete becase I have seen it in some papers, but anyway, it does not work for me, so I have changed the usermaterial for this material DamageTC3D, and now the model is converging well (thanks for that). Now, this is a complete twist in my research, and I have now to study this material but I could not find more information related with it, just the information in this forum which has been very helpful, and the webinars, but I still have doubts. In order tu use this material, I have to reproduce the Thomsem and Wallace experiment, which is shown in figure 1, but I could not find which parameteres could change the slope in the discharge branch. During some test that I have done, the slope for the discharge and recharge branches is the same (I have tested de c1, c2 and c3 parameters but these are only for smoothing the curves), also, I think that the pdf_t and pdf_c parameters could be the key, varying between plasticity and damage. Maybe the question is basic but I just want to know if I can reproduce the experiment with this material before starting.

Thanks in advance.

[STKO Team]

Here is a working version of your model.
To calibrate the post peak regime, you have to play with the fracture energies (Gt and Gc).

pdf_t and pdf_c are used to calibrate the amount of plasticity (0 = pure damage, 1 = pure plasticity). A good value can be 0.5 for both.

I also changed your analysis to make it more stable: instead of an applied force + a displacement-control, I applied an imposed displacement with a load control (it converges better, and it is equivalent in this case were you have only 1 horizontal force).

Finally, I would raccomend you to check the parameters of your steel material. The isotropic hardening ratio seems to high, and it looks like steel is not yielding enough

Test22.zip

(172.87 KiB) Downloaded 217 times

[nelsonlopez5484]

Greetings dear STKO team, thanks for your reply.
Thanks a lot for the model modifications.
I will try to calibrate the parameters Gt and Gc, and see what happens.
Thanks a lot.

[STKO Team]

You're welcome