Help with geostatic analysis

[Nightelf08]

Hi all,
I am quite new to Abaqus and I'm trying to find the effective stresses on a mass of soil with several layers. I have defined material properties including density, elasticity, Mohr-Coulomb failure and permeability for each layer. I have also applied a gravity force of -9.8 on the geostatic step to the entire system, and I have predefined the total stresses at the top and bottom of each layer. I have defined the groundwater table as a pore pressure boundary condition (with a value of 0), and have defined the initial void ratio of each layer in the predefined fields. For some reason this results in negative pore pressures above the ground water table and negative effective stress values (s22) that are quite larger than they should be. Any ideas on what I missed of if I should be approaching this problem in different steps?
Thank you all in advance!

 

[UWOVenky]

I consider that your model is 2d, that's why you are saying S22 otherwise for 3d model, it would have been S33. I see that you have so many parameters, so to troubleshoot just simplify the model by removing the groundwater table and initial void ratio and keep density, linear elastic and mohr-coulomb behaviour. Apply body force in downward direction( downward is negative and upward is positive). I could not my step with gravity and so I applied body force. Also apply *initial conditions, type=stress, geostatic. I guess you know this. This is my suggestion. Probably it may work. Then you can apply extra conditions if this step is successful.

 

[Nightelf08]

Yes, my model is 2D. What would I use for the body force? Just the same -9.8?

 

[UWOVenky]

body force is specified in force per unit volume. So I applied a body force equal to the value of density of the soil. For example, if density is 2556 Kg/m3, then convert this to N/m3 which comes 19000 N/m3. So just write 19000 in component 2 direction. I am assuming here that the vertical direction in which the depth varies is Y direction. One more important thing- I was keeping my upwards dir as negative but later I came to know that it is good to keep downward as negative dir, the way it is usually in Cartesian coordinate system.

 

[Nightelf08]

Hi again UWOVenky. I tried to simplify the model, and now it gives me an error so it doesn't run and it's not having a msg file so I can't see what is wrong. I am thinking of just scrapping the whole thing and starting fresh with a single layer of soil. Which parameters should I define? I just wanna make sure I am doing this right.
Thanks again!

 

[UWOVenky]

For a 2d model, choose plane strain elements. Define only elastic properties i.e. E and v. For boundary conditions, use roller (U1=0) for the sides and fixed for the bottom. Apply a body force as told before. Also use *Initial Conditions, Type= Stress, Geostatic by editing keywords file. Once you get this, then you can add the Mohr Coulomb Plasticity model and check again. You can share your .cae file if you want.

 

[Nightelf08]

Hi again UWOVenky,
So I decided to simplify it even more. I now made it an axisymmetric single layer of soil with no ground water table but the stresses are not negative at the top. I really don't know what I am doing wrong. I attached my file. Could you take a quick look at it? I don't know what else to do. Thank you again!

 

[UWOVenky]

Sorry I do not have 6.13 and so I cannot see your file. However I am attaching a Sample geostatic file. This is 6.10 version file but you can convert it to 6.13. The reverse is not possible. Here is the brief description about the file
Soil is saturated undrained overconsolidated clay. So note the value of E and v (0.49) I have used. Moreover, I have added Mohr Coulomb plasticity which is the case for my model, but you can do it without this also. I have applied a body force in downward direction and accordingly added *INITIAL CONDITIONS in the KEYWORDS. The direction is extremely important. In my case, upwards in + Z and downwards is - Z. The geostatic step is used with FIXED incrementation. But sometimes one does not get the desired results. In such case, you can use AUTOMATIC incrementation by going into STEP>INCREMENTATION and selecting Automatic option. This is called Geostatic step with Enhanced procedure. Refer section 6.8.2 in Abaqus Manual Part 2 about when and where you can use this.
When you are in visulization module, observe that S33 are pointing downwards (-ive S33) and U3 is also pointing downwards(-ive U3)with very low values 10^-9 m. This implies that the step is successful. I hope this helps you.

 

[Nightelf08]

Thank you UWOVenky, Your file helped a lot and I was able to get it to work with the body force approach! Thanks again!

 

[UWOVenky]

I am glad to know that. all the best.