The occurrence of concentrated strain problems at the boundary between infinite and finite elements in ABAQUS can be attributed to several factors. Here are a few possible reasons:

It's important to note that concentrated strain problems at the interface between finite and infinite elements can be complex and depend on the specific modeling setup and geometry of your structure. It is recommended to consult the ABAQUS documentation, conduct sensitivity analyses, and consider seeking assistance from experienced users or support forums to address these issues effectively.

Es común que esto ocurra, ya que las condiciones de borde tratan de simular la continuidad del medio; hay dos alternativas para ello, y es extender el modelo para evitar que las condiciones de borde generen alteración de los resultados en el área de estudio y la segunda es exponer que el modelo presenta esas alteraciones dadas las condiciones de bordes impuestas.

Saludos espero le haya servido la información.

Hi Amir,

I checked your input file and it seems that you are using MC material def. for your soil. So, my guess was that the strain concentration is caused by discontinuity in the material behavior. Your soil block is pulling the infinite region and since it is less deformable, you get the stress concentration and plasticity in the interface region. But I tried to run your input file and in fact, the plasticity already occurred during the static step.

So, there are 2 concerns here from my pov:

1. The way you create the model. First, there is no infinite elements in the bottom of the soil. I understand what you are trying to simulate but by modelling it this way, you have no representation of the static and dynamic behavior in the vertical direction.

2. The geostatic state is missing. As you know, the soil behavior is governed by its confining stress. And it is paramount in nonlinear soil simulation. In your static step, you apply the gravity loading to the soil but there is no predefined stress in the soil. This yields incorrect nonlinear behavior because the soil strength is underestimated. Any deformation beyond this point would be considered invalid. If you are unfamiliar with this, please check the abaqus manual regarding geostatic step.

So, for your model, I recommend to apply the infinite elements surrounding the main study area. You can imagine the interface to be like a half-ellipsoid. The interface here is the line between regular and infinite elements.

And then apply the correct geostatic step. I know it can be a challenge to implement a geostatic step on a model with irregular surface. How I usually solve it is by having a preliminary geostatic computation. In this preliminary model, I apply the geostatic computation while applying fixed boundary condition to all soil (finite) region and record the reaction forces. These reactions are then used as input in the true geostatic step in the main model to stabilize the result. I don't know whether you want to go this far, so I'll stop with the details.

Cheers and good luck with the model.