Initial stress abaqus- stress distribution around the well 1

[FEAppp]

thread799-322424
Hello,
I want to know how the stress distributes around a well.
So I created a 3D solid cube model (5m*5m*5m) and have a well (radius 0.1m) in the center.
I am confused how to apply the stress in the step.

First in the initial step, I don't want the model to deform. So I pinned the six sides of the cube. Also, in the initial step, I defined a predefined fields, stress for sigma11=-20e6, sigma22=-10e6, sigma33=-30e6 (compressive).

What should I do next? I technically defined all the BC in the initial step and no need for the further step, but it won't let me run.

Thanks a lot.

Best,
Wenjing

 

[FEA way]

It's necessary to define analysis step (after initial one) to run the simulation. In case of initial stresses you need general static step to establish equilibrium.

 

[FEAppp]

Hello FEA way, what do you mean by establish equilibrium?

My question is trying to understand how the stress will distribute when the well is present in the subsurface. In the subsurface, we have three in situ stresses, the vertical stress (sigma33) and two horizontal stresses (sigma11,sigma22). If the well is present, the stress will concentrate around the well (Kirsch's equation). And in the geotechnical engineering, we don't want the model to deform because we assume the ground is very large and infinite.

So in the initial step, I pined the six side of the cube and then defined the predefined stress field.
As for the analysis step, I want to know what I should put to establish equilibrium. Could you elaborate more?

Thanks a lot.

Wenjing

 

[FEA way]

In the first static step Abaqus checks for equilibrium and, if necessary, iterates to establish it. Initial time increment should be equal to total step time. This way Abaqus will try to find equilibrium in a single increment. If you performed soil analysis with pore fluid flow included, you would have to use geostatic step instead of static general one.

 

[FEAppp]

Hello FEA way,

Sorry I have another question. In the predefined stress field, the sigma11,22,33,12,3 or 23, do 1,2,3 correspond to the global coordinate x,y,z or correspond to the local coordinate?
Thanks a lot.

Wenjing

 

[FEA way]

Normally initial stress components are specified in global coordinate system. Unless user-defined orientations (keyword *Orientation) are used.

 

[FEAppp]

Hello FEA way,

Thanks, this makes more sense now.
In the system of equation, we have K*u=f (stiffness, displacement, force). So normally, we give essential Boundary conditions or natural boundary conditions.
So what does the predefined stress field correspond to?
In other words, why I only pinned the boundary (essential boundary conditions) and gave predefined stress field, the FEM can give a result.
Does predefined stress field somehow relate to the natural BC, or else?

Wenjing

 

[FEA way]

In FEM intial stresses are added directly to load vector. They are multiplied by the transpose of strain-displacement matrix B first.