Generally, geostatic step is used to establish in-situ stresses in soil profile concurrent with no deformation which is the case for most of the geotechnical problems.

You can use static general step under gravity loading but you will have some degree of deformation under this load.

Thank you for the reply guys, the reason I wanted to avoid the geostatic was because I was getting a small deformation at the end of that step. My mesh was slightly course which means the initial stresses calculated and the ones that were input were slightly different. I believe this is causing the deformation (the ratio of deformation to length of the boundary is of the order 10^-5). Now I am getting a deformation when I use static, general too but the amount is slightly smaller. I just thought this might have been due to the geostatic and wanted to see it would be replaceable. I guess now I need to refine the mesh and see what impact it has on the problem. 

I used body force in the geostatic analysis, the equilibrium can be reached. I changed to gravity but the equilibrium cannot be reached. I am using pore pressure/stress elements. Anyone knows the reason?

If you are using body force it means that you are working in excess pore pressure in opposition to gravity load that's based on total pore pressure. If you use total pore pressure (gravity loading) you have to enter initial conditions regarding distribution of pore pressure

Elaheh, first let me try to describe about specifying the initial stresses. The predefined stresses option allows you to define the stress state of any object at the initial time step. You can use it in one of two methods namely the initial stress option or the geostatic stress options. Using the initial stress you can specify the 3 principal and 3 shear stresses. For most common geotechnical problems we do not need to use this option and we stick to geostatic stresses. ABAQUS requires the specification of vertical stresses at 2 points which it would then use for calculating the stresses at all nodes in between them by linear interpolation. For example assume a column of soil 1m high below the ground level then the vertical stress at the top of the soil is 0 for vertical coordinate 0. The stress at vertical coordinate 1m is equal to - density x gravity x height (here 1m), here the sign convention for compressive stresses need to be negative.  The K0 value is specified using the lateral coefficient 1, if the horizontal stress is asymmetric then you specify the other value in lateral coefficient 2. As far as modeling your wellbore problem, I am not sure on the nature of the simulation. If you can give a few more details, we can look at solving it. I hope this helps!! 

From the discussions above, it seems that the geostatic analysis step is used to determine the in-situ stresses. In the case that the overburden stress and in-situ stress are given, geostatic analysis is not necessary. Please correct me if you have different opinion.

 Dear all,

Many thanks for your responses and guidance. I have a question and I would be very thankful if you could help me.

Does this procedure work only for creating in situ stress of horizontal layers?

I read a paper which mentioned that" where the ground surface, the subsoil layer or the ground water level is not horizontal, the k0 procedure will lead to the existence of unbalance force or non-equilibrium of initial forces within the soil body". 

Best regards,

"The elevations defining a geostatic stress state are the same"

I got this error message while running my caisson-clay model. Any help to find out the mistake and solve that?

Hi mohammad

when you are defining state of the soil, you should determine 2 different elavation and 2 different stress values corresponding to elavation. You define a same level of elavation.

Good luck

Hi,

I would like to share my experience here and hope it is somewhat helpful. One thing we need to pay attention in ABAQUS/CAE while setting the geostatic stress as the predefined field is that the direction of geostatic stress is set in z-direction as default. So if you build your soil model with y-direction as the vertical direction, you may first want to rotate the model under assembly module. I am not sure is this settings same in different versions of ABAQUS or not, so maybe first thing is to check the manual.

Good luck!

In Abaqus Axisymmetric Tunnel Modelling, if Predefined Geostatic stress field is applied, is there a need of “GEOSTATIC” as first step or it should be “STATIC GENERAL”?

The difference between this two step is the degree of freedom "pore pressure". The general static don't consider consolidation.

In normal tunnel excavation problem both "Geostatic" and "Static general" will have the same results.