On the Geostatic Step 1

[Cansand]

Does any one have some remarks on how can I establish equilibrium and get zero displacement out of Geostatic Step. I have avery simple plain strain (2D) model and
I applied the following initial stress that balances the gravity load of g=-10 m/s^2 operating in z direction throughout a zone that extends vertically from z=0 to z=100 m

I am estimating the intial vertical stress as follows. I have the zone density of 2066 kg/m^3 and therefore bulk unit weight is (2066 * g=-10) =-20060 N/m^3
the stress at depth of 100 is 100*-20060= -2006000 N/M^2

Therefore Initial Geostatic Stress is

*initial conditions, type=STRESS, geostatic
Ground, -2006000, 0, 0, 100, 0.38, 0
Where 0.38 is the coefficient of earth pressure .However I am getting ridicules displacement : in the order of 10 m
Any guidance about how should I establish Initial Geostatic Stress condition to obtain negligible displacement field out of Geostatic Step as what is supposed to be

 

[sendy]

hi,

i've just try it and it works with displ in order of 10^-20 for only equilibrium, and the vertical and horizontal stresses are exactly the value i inputted in initial condition option.
have you do the equilibrium after applying initial condition ?

As quoted from the manual (Abaqus Standard Manual/Prescribed Conditions/Initial conditions):

"The geostatic stress state specified initially should be in equilibrium with the applied loads (such as gravity) and boundary conditions. An initial *STEP should be included to allow ABAQUS to check for equilibrium after this interpolation has been done; see the discussion above on establishing equilibrium when an initial stress field is applied."

hope this help.

 

[Cansand]

I do not think that guessing the right initial stress that lead to zero displacement filed (equilibrate the applied gravity force) can be easily done.
The idea is that ABAQUS will equilibrate the stress field calculated from the applied gravity force considering elastic law
The thing is that one should keep playing with the initial applied Geostatic Stress and the Coefficient of earth pressure until matching reasonably (so that the resulted obtained displacement field is zero) the stress field induced by the gravity force.
This play could take many many hours. It is regretfully a hit and try-game with minimum judgment involved
Do you agree with me

 

[sendy]

hi,

I think there is "no guessing" in the sense that users input the geostatic initial condition and apply the gravity load in the first step. In this case the results read:

\sigma_v = \gamma*h, \sigma_h = K*\sigma_v, where h and K are distance of the calculated point from the surface and Coef earth pressure, respectively.

As I understand, that first step is for establishing equilibrium. Afterwards, the next load step may be applied.
So... I don't see any "playing" with Geostatic earth pressure and Coef earth pressure, except that the users should know the correct Coef earth pressure which may go to another issue (in my opinion).

regards.

 

[Cansand]

In fact (in plain strain) the exact geostatic stresses in the body is done through Calculating stress and displacement fields resulted from gravity (assuming elastic media) is done through elasticity relations ( not piece of cack )
Inserting initial stresses based on
\sigma_v = \gamma*h, \sigma_h = K*\sigma_v, where h and K are distance of the calculated point from the surface and Coef earth pressure, respectively.
is just a very approximate way for the existing stress field and hence displacement field.
One should play with these approximate field until it becomes very close to the above exact stress field (calculated based on FE elasticity)
I followed the same way you talked about and estimated K0 from the famous approximate relation K0=V/1-V where V is Poission ratio and I have Gamma =2066
but i still get high displacement 40 cm for the medium of 100 m depth.
By the way what do you mean by
have you do the equilibrium after applying initial condition? do you mean I used Geostatic Step. Yes I did please send me the input file where we got negilgent displacement

Thank you

 

[sendy]

hi,

following is the input that i got almost zero displacement at the equilibrium step. Here, users may use either *STATIC or *GEOSTATIC. In the input file I don't use your gamma value. Hope it won't influence the displacement in the equilibrium step too much.
I think here the coef earth pressure is a kind of approximation at the at rest condition; infact it is not constant through out the next loading behavior (well.. this is just what is in my opinion).

Hope this help abit.

regards.

**********HEAD*******************************
**
*HEADING
Vertical pressure on half space boundary
**
******NODE/NODE SETS DEFINITION**************
PREPRINT, Echo=Yes, MOdel=Yes, History=Yes
*********************************************
**
*NODE
101,0. ,0.
141,0.80,0.
2101,0. ,0.40
2141,0.80,0.40
*NGEN,NSET=NROW1
101,141,1
*NGEN,NSET=NROW21
2101,2141,1
*NFILL,NSET=NALL
NROW1,NROW21, 20, 100
*NSET,NSET=NRIGHT,GEN
141,2141,100
*NSET,NSET=NLEFT,GEN
101,2001,100
*NSET,NSET=NMID,GEN
121,2121,100
*NSET,NSET=NFOOT1,GEN
2101,2103,1
*NSET,NSET=NFOOT2,GEN
2102,2104,1
*NSET,NSET=NFOOT
NFOOT1,NFOOT2
*NSET,NSET=NTOPC
2101
*NSET,NSET=NTOP1,GEN
2101,2140,1
*NSET,NSET=NTOP2,GEN
2102,2141,1
*NSET,NSET=NHIST
2101,1804
**
******ELEMENT/ELEMENT SETS DEFINITION********
**
*ELEMENT,TYPE=CPE4
101, 101,102,202,201
*ELGEN,ELSET=EALL
101, 40,1,1, 20,100,100
**********************************************
******MATERIAL PROPERTY**********************
*SOLID SECTION,ELSET=EALL,MATERIAL=SOIL
***HOURGLASS STIFFNESS
** 0.005
*MATERIAL,NAME=SOIL
*ELASTIC, TYPE=ISO
**kPa
3.036E4,0.328
*DRUCKER PRAGER, SHEAR CRITERION=Linear
***\Friction angle,\K-value\,dilation angle,\temperature
40.9,1.0,10.,0.
*DRUCKER PRAGER HARDENING, TYPE=COMPRESSION
***\Yield.stress,\Corresponding.plastic.strain
120.,0
***USER MATERIAL, UNSYMM, CONSTANTS=4
**-101.2,-962.1,-877.3,1229.2
****-69.4,-673.1,-655.9,699.6
****-200.0,-1572.5,-1572.5,2583.3
**
***DEPVAR
** 15
*DENSITY
** ML^-3 = t/m^3
1.7
**
*************************
*ELSET,ELSET=ELEFT,GEN
101,2001,100
*ELSET,ELSET=ERIGHT,GEN
140,2040,100
*ELSET,ELSET=ETOP,GEN
2001,2040,1
*ELSET,ELSET=ELOAD,GEN
2001,2002,1
*ELSET,ELSET=EHIST
2001,1904,1503
*ELSET,ELSET=ELTEN,GEN
2004,2021,1
*************************
*EQUATION
2
NFOOT1,2,1.0,NFOOT2,2,-1.0
*************************
******BOUNDARY CONDITION*********************
*BOUNDARY
NROW1,1,2
NLEFT,1
NTOPC,1
NRIGHT,1
**
********INITIAL CONDITION**********************
*INITIAL CONDITIONS,TYPE=STRESS,GEOSTATIC
EALL,-6.8,0.,0.,0.4,0.5
***INITIAL CONDITIONS,TYPE=STRESS
** ETOP,-5.,0.,-5.,0.
***INITIAL CONDITION,TYPE=SOLUTION, USER
**
******STEP DEFINITION************************
******STEP 1 ********************************
*STEP, NLGEOM, INC=100, UNSYMM=YES
STEP 1
*STATIC
1.e-6,1.e-6,1.e-6,1.e-6
*DLOAD
** ETOP,P3,1.
** ETOP,P2,5.
** ETOP,P4,5.
EALL,GRAV,10.,0.,-1.,0.
*MONITOR,DOF=2,NODE=2101
**
*ELPRINT,ELSET=EALL,FREQ=50
SP1,SP2,SP3
*OUTPUT,FIELD,FREQ=5
*NODE OUTPUT,NSET=NALL
U,RF
*ELEMENT OUTPUT,ELSET=EALL
E,S,SP
*OUTPUT, HISTORY
*NODE OUTPUT,NSET=NHIST
U
*ELEMENT OUTPUT,ELSET=EHIST
E,S,SP
*END STEP