This section provides examples of typical initial-state problems, as follows:
The following example initial-stress problem shows how to define an initial-stress file and use the INISTATE,READ command to read the data into your analysis.
The following file contains the initial stresses to be read into Mechanical APDL. Each element has eight integration points in the domain of the element.
/CSYS,0
! ELEM ID ELEM INTG LAY/CELL SECT INTG SX SY SZ SXY SYZ SXZ
1 , 1, 1, 1, 100, 0, 0, 0, 0, 0
1 , 2, 1, 1, 100, 0, 0, 0, 0, 0
1 , 3, 1, 1, 100, 0, 0, 0, 0, 0
1 , 4, 1, 1, 100, 0, 0, 0, 0, 0
1 , 5, 1, 1, 100, 0, 0, 0, 0, 0
1 , 6, 1, 1, 100, 0, 0, 0, 0, 0
1 , 7, 1, 1, 100, 0, 0, 0, 0, 0
1 , 8, 1, 1, 100, 0, 0, 0, 0, 0
In the following input listing, initial-stress loading data is read in from a file. The data is read in during the first load step, and establishes a preliminary deflection corresponding to a tip loaded cantilever beam with a tip load of 100.
/prep7 /title, Example of Initial stress import into ANSYS et,1,182 ! Plane stress PLANE182 element mp,ex,1,1.0e9 mp,nuxy,1,0.3 ! ! Define the nodes ! n,1 n,2,2.0 n,3,4.0 n,4,6.0 n,5,8.0 n,6,10.0 n,7,,1.0 n,8,2.0,1.0 n,9,4.0,1.0 n,10,6.0,1.0 n,11,8.0,1.0 n,12,10.0,1.0 ! ! Define the 5 elements ! e,1,2,8,7 e,2,3,9,8 e,3,4,10,9 e,4,5,11,10 e,5,6,12,11 ! Constrain all dofs on all nodes at x=0 to be zero nsel,s,loc,x, d,all,all nall finish ! /solu ! Read in the initial stresses from istress.ist file ! as loading in the 1st load step. ! Input stresses correspond to the element integration ! point location. ! inistate,read,istress,ist ! List the initial stresses inistate,list outres,all,all solve finish ! /post1 set,last prnsol,u finish
The INISTATE,WRITE command specifies the coordinate system into which the data is to be written.
You can apply constant stresses to all selected elements by issuing a INISTATE,DEFI,ALL command. The INISTATE command can also delete stress from individual elements after the stress is applied. The INISTATE,LIST command lists the applied stresses. The following input listing shows how these commands are used.
solution ! ! Apply a constant state of the initial stresses. ! inistate,defi,all,,,,1322.34,2022.21,302.43,4040.32,5076.32,6021.456 ! ! Verify the applied stresses then delete those of element #1 ! inistate,list inistate,dele, 1 ! ! Set the boundary conditions and then solve ! inistate,list solve finish
This example initial strain problem is a simple uniaxial test. A displacement of 0.05 is applied to this single element. An additional 0.05 initial strain is applied. The calculated results include the effects of both initial strain field and the applied displacement.
delta = 0.05 ndiv=1 /prep7 ! Define the material mp,ex,1,20E3 mp,nuxy,1,0.3 mp,dens,1,7850 ! kg/m3 et,1,185 block,0,1,0,1,0,1 lesize,all,,,ndiv vmesh,all,all finish /solu nsel,s,loc,x d,all,ux nsel,s,loc,y d,all,uy nsel,s,loc,z d,all,uz inistate,set,dtyp,epel inistate,defi,,,,,0.05, nsel,s,loc,x,1 d,all,ux,delta allsel,all solve /post1 set,last presol,s presol,epto presol,epel finish
This initial plastic strain example is a simple 3-D problem where the cross section has three layers. An initial plastic strain and stress are applied to one of the layers. One end of the block (shaped like a beam) is fixed and the stresses are allowed to redistribute. The following input listing shows how to apply initial plastic strain to one layer within a cross section and check the redistributed stresses.
/prep7 et,1,185,,2,1 keyopt,1,8,1 ! store data for all layers (can be excessive) mp, ex, 11, 20.0e6 ! psi (lbf/in^2) mp, prxy, 11, 0.25 ! unitless mp, ex, 12, 20.0e6 ! psi (lbf/in^2) mp, prxy, 12, 0.25 ! unitless mp, ex, 13, 20.0e6 ! psi (lbf/in^2) mp, prxy, 13, 0.25 ! unitless ! MISO material model tb,plas,11,,3,miso tbpt,,0.0,1e3 tbpt,,0.6,1e3 ! BISO material model tb,biso,12,,1 tbdata,define,100,100000 ! Plastic material model tb,plas,13,,7,miso tbpt,,0.0000,30000 tbpt,,4.00e-3,32000 tbpt,,8.10e-3,33800 tbpt,,1.25e-2,35000 tbpt,,2.18e-2,36500 tbpt,,3.10e-2,38000 tbpt,,4.05e-2,39000 sectype,1,shell,,my3ply ! 3-ply laminate secdata, 0.30, 11, , 3 ! 1st layer THICK, MAT, ANG, Int. Pts. secdata, 0.30, 12, , 3 ! 2nd layer THICK, MAT, ANG, Int. Pts. secdata, 0.30, 13, , 3 ! 3rd layer THICK, MAT, ANG, Int. Pts. ! align esys with the global system block,0,1,0,0.1,0,0.1 type,1 secnum,1 esize,0.1 vmesh,1 finish /solu antype,static outres,all,all ! Uniaxial State Initial plastic Strain. inistate,set,mat,13 inistate,set,dtyp,eppl inistate,defi,all,all,all,all,0.1,,, inistate,set,dtyp,pleq inistate,defi,all,all,all,all,0.1,,, inistate,set,dtyp,stress inistate,define,all,all,all,all,1000 inistate,set,dtyp,, inistate,list,all nsel,s,loc,x,0 d,all,all,0.0 ! Fix one end nsel,all solve save finish /post1 set,last esel,s,elem,,1 /com ----------------------------------------------------------------------------- /com, Expected result: You should see newly redistributed stresses and strains in /com, all layers /com ----------------------------------------------------------------------------- layer,1 presol,s,comp presol,eppl,comp layer,2 presol,s,comp presol,eppl,comp layer,3 presol,s,comp presol,eppl,comp finish
This initial creep strain example demonstrates how you can use initial creep strain from one analysis, then continue the problem to perform a second step.
In Analysis 1, creep strains are calculated up to TIME = 100 in the first step, and then the analysis is continued up to TIME = 200 in the second step.
In Analysis 2, initial-state data generated at TIME = 100 is used as the starting point, and the creep analysis is performed only for TIME = 100 to TIME = 200.
The two analyses generate the same results, validating the use of initial creep strain.
!*************************************************************** ! Analysis 1: Multiple Steps *without* INISTATE !*************************************************************** ! Read the FE Model from the CDB File. FE Model has both Plasticity and Creep Material Models Defined. /prep7 CDREAD,ALL,geom,cdb ! Perform a two-step sample creep problem /SOLU RATE,OFF /OUT, scratch TOFFST,273, TIME,1E-6 AUTOTS,0 NSUBST,1 KBC,0 SOLVE ! Step 1: Generate initial-state information RESCONTROL,,2,10 RATE,ON,ON TIME,100 ! Reduced time for faster solution run time. AUTOTS,1 NSUBST,1000,1000,10 KBC,0 OUTRES,ALL,10, inistate,write,1,,,,-1,s inistate,write,1,,,,-1,eppl inistate,write,1,,,,-1,pleq inistate,write,1,,,,-1,epcr SOLVE inistate,write,0,,,,-1,s inistate,write,0,,,,-1,eppl inistate,write,0,,,,-1,pleq inistate,write,0,,,,-1,epcr ! Step 2: Perform Step 2 of the creep problem TIME,200 SOLVE FINISH ! Print out the results /POST26 /OUT /com ------------------------------------------------------------------------- /com | The deflections in y direction of nozzle top from continuous solution| /com ------------------------------------------------------------------------- /OUT,scratch NSOL,2,453,U,Y,Etype181 /OUT PRVAR,2 FINISH /post1 presol,epcr,comp finish ! Clear the database /clear !*************************************************************** ! Analysis 2: Multiple Steps *with* INISTATE !*************************************************************** ! Resume old cdb file /prep7 CDREAD,ALL,geom,cdb ! Step 1: Read in INISTATE data with creep strain from the IST ! file with rate off and solve /SOLU RATE,OFF /OUT, scratch TOFFST,273, TIME,100 AUTOTS,0 NSUBST,10,10,10 KBC,0 inistate,read,filename ist SOLVE ! Step 2: Continue and generate the same results as Analysis 1 RESCONTROL,,2,10 RATE,ON,ON TIME,200 AUTOTS,1 NSUBST,10,100,10 KBC,0 OUTRES,ALL,10, pred,off SOLVE FINISH /POST26 /OUT /com ------------------------------------------------------------------------- /com | The deflections in y direction of nozzle top from continuous solution| /com ------------------------------------------------------------------------- /OUT,scratch NSOL,2,453,U,Y,Etype181 /OUT PRVAR,2 FINISH /post1 presol,epcr,comp finish
This initial-state example shows how you can use initial-state data (as state variables) from one analysis, then continue the problem in a subsequent analysis.
To continue an isotropic hardening plasticity analysis, plastic strain,
accumulated equivalent plastic strain, and stress are needed. In this problem, the
accumulated equivalent plastic strain is saved from the
UserMat routine
as state variables, which are then used as initial-state data for the initial
accumulated equivalent plastic strain applied in the subsequent analysis.
Analysis 1: Adisplacement of ux = 0.3 is applied in load step 1, unloaded to ux = 0.2 in load step 2, and an additional displacement of ux = 0.2 is applied in load step 3. Initial-state data is generated at the end of load step 2. Plastic strain, stress and accumulated equivalent plastic strain are saved in the .ist file.
Analysis 2: The initial-state data generated previously is used as the starting point. An additional displacement of 0.2--the difference between the displacement in load step 3 and load step 2 in the prior analysis--is applied in load step 2 in this analysis.
The two analyses generate the same results, validating the use of initial state with state variables.
/filname,tutor-bag06s
/prep7
et,1,185
keyopt,1,3,1
! Define
tb,user,1,2,4
tbdata,1,19e5, 0.3, 1e4,2000, ! E, posn, sigy, H
tb,state,mat2,,10
tbdata,1,0.0,0.0,0.0,0.0,0.0,0.0 ! initialize state variables
tbdata,7,0.0 ! initialize state variables
type,1
real,1
mat,1
sectype,1,shell
secdata, 0.125, 1, 0.0,1
secdata, 0.125, 1, 30.0,1
secdata, 0.125, 1, 60.0,1
secdata, 0.125, 1, 90.0,1
block,0,1,0,1,0,1
esize,0.5
vmesh,all
nsel,s,loc,x,0
d,all,ux
nsel,s,loc,y,0
d,all,uy
nsel,s,loc,z,0
d,all,uz
allsel,all
cdwrite,comb,tutor-bag06s,cdb
finish
/solu
outres,all,all
time,0.5
eresx,no
nsel,s,loc,x,1
d,all,ux,0.03 ! First load step,displacement on x-axis
allsel,all
solve
time,1
nsel,s,loc,x,1
d,all,ux,0.02
allsel,all
! Save Plastic Strain, Elastic Strain and State Variables.
inis,write,1,,,,-2,s
inis,write,1,,,,-2,eppl
inis,write,1,,,,-2,svar
solve
inis,write,0,,,,-2,s
inis,write,0,,,,-2,eppl
inis,write,0,,,,-2,svar
time,2
nsel,s,loc,x,1 ! Second load step , displacement on x-axis
d,all,ux,0.04
allsel,all
solve
finish
/post1
/com
/com +**************************************************************
/com Results fron the analysis without INIS command
/com ***************************************************************
rsys,solu
set,2
esel,s,elem,,1
etable,epplx_2r,eppl,x
etable,epply_2r,eppl,y
etable,epplz_2r,eppl,z
set,last
etable,epplx_3r,eppl,x
etable,epply_3r,eppl,y
etable,epplz_3r,eppl,z
allsel,all
pretab,epplx_2r,epply_2r,epplz_2r,epplx_3r,epply_3r,epplz_3r
fini
/clear,nostart
/delet,tutor-bag06s,rst
/filname,tutor-bag06s
cdread,comb,tutor-bag06s,cdb
/com ***********************************************************************
/com Second case: analysis with INISTATE command
/com ***********************************************************************
/solu
outres,all,all
time,0.1
inis,read,tutor-bag06s,ist ! First load step, reading back initial strain datas
ddele,all,all
nsel,s,loc,x,0
d,all,ux
nsel,s,loc,y,0
d,all,uy
allsel,all
nsel,s,loc,x,1 ! First load step ,no displacement on x-axis
d,all,ux,0.0
allsel,all
inis,set,dtyp
inis,list,1
solve
time,2
nsel,s,loc,x,1 ! Second load step , displacement on x-axis
d,all,ux,0.02
allsel,all
solve
finish
/post1
/com
/com ***************************************************************
/com Results fron the analysis with the INIS command
/com ***************************************************************
rsys,solu
set,1
esel,s,elem,,1
etable,epplx_2r,eppl,x
etable,epply_2r,eppl,y
etable,epplz_2r,eppl,z
set,last
etable,epplx_3r,eppl,x
etable,epply_3r,eppl,y
etable,epplz_3r,eppl,z
allsel,all
pretab,epplx_2r,epply_2r,epplz_2r,epplx_3r,epply_3r,epplz_3r
fini
This example node-based initial-state problem describes how to generate a node-based initial-state file from another analysis and then apply that data to a modal analysis.
In step 1, a node-based initial-state file is generated. In step 2, the file is read in and a static solution is generated. In step 3, the modal analysis is done.
/prep7
!********** Define the material **********
mp,ex,1,210e9 ! Pa
mp,nuxy,1,.29 ! No units
mp,dens,1,7850 ! kg/m3
et,1,182
rectng,0,10,0,2,
esize,0.5
amesh,all
nsel,s,loc,x
d,all,ux
nsel,s,loc,y,0
d,all,uy
nsel,s,loc,x,10
d,all,ux,0.1
nall
finish
/solu
antype,static
time,1
nsubst,10,10,10
solve ! Solve for Sample Prestress Loads
fini
/post1
*get,mxnid,node,,num,max
nsel,s,node,,mxnid
prnsol,s,comp
nsel,all,all
*vget,nl,node,,nlist
*vget,sx,node,,s,x
*vget,sy,node,,s,y
*vget,sz,node,,s,z
*cfopen,tutor-bag07s-ist.dat ! Generate Ist File
*vwrite
('INIS,SET,NODE,1')
*vwrite,nl(1),sx(1),sy(1),sz(1)
('INIS,DEFI,',F4.0,' , , , , ',E,' , ',E,' , ',E,',0.0,0.0,0.0')
*cfclos
/solu
ddele,all,all
d,all,all
nall
antype,static
time,1
nsubst,10,10,10
/inp,tutor-bag07s-ist.dat ! Read in Node Based IST Data
esel,s,elem,,1,80,5
inis,list
allsel,all
rescontrol,linear,all,1
solve
finish
!********** Perform a perturbed modal analysis **********
/solu
antype,static,restart,,,perturb
perturb,modal,,,nokeep
solve,elform
nsel,s,loc,x
nsel,a,loc,x,10.0
d,all,ux
nsel,s,loc,y,0
d,all,uy
nall
modopt,lanb,5
mxpand,5
solve
fini
/post1
file,,rstp
set,list
fini
This example shows how to apply and use initial pore
pressure and void ratio on coupled pore-pressure-thermal
elements (CPTnnn).
/PREP7 ET,1,212 KEYO,1,3,1 R,1 !------------------------------------------------------------------------------- !---- MATERIAL PROPERTY DEFINITION ! SET MATERIAL DENSITY DENS,1,1.2 ! ! ELASTIC MATERIAL LAW KAPPA=0.054 ! NU0=0.35 ! NU0=(3*P0*(1+E0)/KAPPA-2*MU0)/(2*(3*P0*(1+E0)/KAPPA)-MU0) E0=0.34 ! VOID RATIO E0=N_F0_F/N_S0_S A0=20 ! INITIAL SIZE OF THE YIELD SURFACE AH_MIN=0.01*A0 EM=1440 K0=EM/(1-2*NU0) ! FOOTING PROBLEM: K0=EM/(1-2*NU0) PT_EL=K0*KAPPA/(1+E0) ! FOOTING PROBLEM: K0=EM/(1-2*NU0) !PARAMETER TO VON MISES PLASTICITY BETA_DRY=1.0 ! SHAPE OF THE YIELD SURFACE IN DRY PART [-] BETA_WET=1.0 ! SHAPE OF THE YIELD SURFACE IN WETTING PART [-] LAMBDA_F=0.37 ! PLASTIC SLOPE (STIFFNESS) [M^2/KN] >KAPPA (2-3 TIME OF KAPPA) KS=1.0 ! SHAPE OF THE YIELD SURFACE IN THE OCTAHEDRAL STRESS PLANE MC=1.4 ! SLOPE OF THE CSL IN THE HYDROSTATIC STRESS PLANE 6*SIN(PHI)/(3+SIN(PHI)->PHI: STRESS FRICTION ANGLE !TBDATA,8, KAPPA, NU0, E0, PT_EL TB,PELAS,1,,,POISSON TBDATA,1, KAPPA, PT_EL, NU0, E0 !---- POROUS MATERIAL DEFINITION FPX=8.62E-3 ONE=1.0 TB,PM,1,,,PERM TBDATA,1,FPX,FPX,FPX TB,PM,1,,,BIOT TBDATA,1,ONE ALLSEL !------------------------------------------------------------------------------- W=3 ! WIDTH RECTNG,0,6*W,0,-9*W TYPE,1 REAL,1 MAT,1 MSHAP,0,2D ESIZE,W/4 AMESH,1 NSEL,S,LOC,Y,-9*W D,ALL,UX,0 D,ALL,UY,0 ALLSEL NSEL,S,LOC,X,0 NSEL,A,LOC,X,6*W D,ALL,UX,0 ALLSEL NSEL,S,LOC,Y,0 D,ALL,UX,0 D,ALL,PRES,0 NSEL,R,LOC,X,0,W SF,ALL,PRES,1E3 ALLSEL FINI /SOLU ! SET AN INITIAL PORE PRESSURE OF P0 P0=69 INISTATE,SET,DTYP,PPRE INISTATE,DEFI,ALL,,,,P0 ! Override the void ratio defined in the TB,PELAS with 0.4 newvratio=0.4 INISTATE,SET,DTYP,VOID INISTATE,DEFI,ALL,,,,newvratio ANTYPE,STATIC NROPT,UNSYM!FULL NEQIT,30 TIME,1E3 NSUBST,100,1000,20 OUTRES,ALL,ALL KBC,1 SOLVE FINI /POST1 /OUT, ESEL,S,ELEM,,1 !Output Pore Pressure in element 1 PRES,PMSV PRES,EPTO /COM, EXPECTED RESULTS: EVOID=E0+VCE+(1+E0)=0.3453 FINISH
This example shows how to apply and use initial degree of saturation and relative
permeability on coupled pore-pressure-thermal
elements (CPTnnn).
For more information, see Porous Media in the Mechanical APDL Material Reference.
/prep7 et,1,213 keyopt,1,3,2 rectng,0,0.2,0,1 esize,0.2 amesh,1 MP,EX,1,22E6 ! YOUNG'S MODULUS 22MPa MP,NUXY,1,0.1 ! POISSON'S RATIO FPX=1.0e-6 ONE=1.0 TB,PM,1,,,PERM TBDATA,1,FPX TB,PM,1,,,BIOT ! BIOT COEFFICIENT TBDATA,1,ONE grav_val = 9.8 KS=38e20 !---BULK MODULUS OF SAND GS=18000 !---SPECIFIC WEIGHT OF SAND KF=2.0e9 !---BULK MODULUS OF WATER GF=9800 !---SPECIFIC WEIGHT OF WATER PORO=0.46 TB,PM,1,,,SP TBDATA,1,KS,GS TB,PM,1,,,FP TBDATA,1,KF,9800,PORO TB,PM,1,,,GRAV TBDATA,1,grav_val TB,PM,1,,,DSAT TBPT, DEFI,-29392.04436, 6.55E-01 TBPT, DEFI,-19496.6884 , 6.97E-01 TBPT, DEFI,-9684.84608 , 7.68E-01 TBPT, DEFI,-4019.864744, 8.55E-01 TBPT, DEFI,-2600.901772, 8.93E-01 TBPT, DEFI,-1960, 9.16E-01 TBPT, DEFI,-1303.344238, 9.47E-01 TBPT, DEFI,-379.9278504, 9.76E-01 TBPT, DEFI,0, 1 TB,PM,1,,,RPER TBPT,DEFI,-29399.14446, 1.49E-02 TBPT,DEFI,-19506.50996, 2.86E-02 TBPT,DEFI,-9792.20116, 0.105711 TBPT,DEFI,-4375.105336, 0.28040033 TBPT,DEFI,-2800.991802, 0.50408592 TBPT,DEFI,-2143.613388, 0.7166936 TBPT,DEFI,-1955.016308, 0.7875667 TBPT,DEFI,-1675.97297, 0.84350266 TBPT,DEFI,-1583.528982, 0.8546851 TBPT,DEFI,-1303.344238, 0.92554665 TBPT,DEFI,-841.695638, 0.9739965 TBPT,DEFI,0, 1 d,all,ux,0 nsel,s,loc,y,0 d,all,uy,0 allsel init_kr=0.92554665 init_sw=9.47E-01 inistate,set,dtyp,rper inistate,defi,all,,,,init_kr inistate,set,dtyp,dsat inistate,defi,all,,,,init_sw init_pres=-1303.344238 nsel,s,loc,y,0 d,all,pres,init_pres allsel nsel,s,loc,y,1 d,all,uy,0.01 allsel finish /solu ANTYPE,SOIL SSOPT,SFSW,0,-1,0,OFF,OFF ! NO FLUID WEIGHT SSOPT,CONSOLIDATION NROPT,UNSYM NSUBST,50,5000,25 KBC,0 ! LOADS CHANGED IN STEPS OUTRES,ALL,ALL tim1 = 50 TIME,tim1 SOLVE finish /post1 set,first *get, pp,node,node(0.2,0.4,0),pmsv,ppre /out, ppnode=pp finish /exit,nosave
This example shows how to apply and use initial pore pressure and void ratio as a function of location.
/PREP7 ET,1,212 KEYO,1,3,1 R,1 !------------------------------------------------------------------------------- !---- MATERIAL PROPERTY DEFINITION ! SET MATERIAL DENSITY DENS,1,1.2 ! ! ELASTIC MATERIAL LAW KAPPA=0.054 ! NU0=0.35 ! NU0=(3*P0*(1+E0)/KAPPA-2*MU0)/(2*(3*P0*(1+E0)/KAPPA)-MU0) E0=0.34 ! VOID RATIO E0=N_F0_F/N_S0_S A0=20 ! INITIAL SIZE OF THE YIELD SURFACE AH_MIN=0.01*A0 EM=1440 K0=EM/(1-2*NU0) ! FOOTING PROBLEM: K0=EM/(1-2*NU0) PT_EL=K0*KAPPA/(1+E0) ! FOOTING PROBLEM: K0=EM/(1-2*NU0) !PARAMETER TO VON MISES PLASTICITY BETA_DRY=1.0 ! SHAPE OF THE YIELD SURFACE IN DRY PART [-] BETA_WET=1.0 ! SHAPE OF THE YIELD SURFACE IN WETTING PART [-] LAMBDA_F=0.37 ! PLASTIC SLOPE (STIFFNESS) [M^2/KN] >KAPPA (2-3 TIME OF KAPPA) KS=1.0 ! SHAPE OF THE YIELD SURFACE IN THE OCTAHEDRAL STRESS PLANE MC=1.4 ! SLOPE OF THE CSL IN THE HYDROSTATIC STRESS PLANE 6*SIN(PHI)/(3+SIN(PHI)->PHI: STRESS FRICTION ANGLE !TBDATA,8, KAPPA, NU0, E0, PT_EL TB,PELAS,1,,,POISSON TBDATA,1, KAPPA, PT_EL, NU0, E0 !---- POROUS MATERIAL DEFINITION FPX=8.62E-3 ONE=1.0 TB,PM,1,,,PERM TBDATA,1,FPX,FPX,FPX TB,PM,1,,,BIOT TBDATA,1,ONE ALLSEL !------------------------------------------------------------------------------- W=3 ! WIDTH RECTNG,0,6*W,0,-9*W TYPE,1 REAL,1 MAT,1 MSHAP,0,2D ESIZE,W/4 AMESH,1 NSEL,S,LOC,Y,-9*W D,ALL,UX,0 D,ALL,UY,0 ALLSEL NSEL,S,LOC,X,0 NSEL,A,LOC,X,6*W D,ALL,UX,0 ALLSEL NSEL,S,LOC,Y,0 D,ALL,UX,0 D,ALL,PRES,0 NSEL,R,LOC,X,0,W SF,ALL,PRES,1E3 ALLSEL FINI /SOLU ! SET AN INITIAL PORE PRESSURE OF P0 AND INCREASES WITH DEPTH P0=69 SL=0.1 INIS,SET,DATA,FUNC INISTATE,SET,DTYP,PPRE INISTATE,DEFI,ALL,,,,LINY,P0,SL ! OVERRIDE THE VOID RATIO DEFINED IN THE TB,PELAS WITH 0.4 NEWVRATIO=0.4 INISTATE,SET,DTYP,VOID INISTATE,DEFI,ALL,,,,LINY,NEWVRATIO,0 ANTYPE,STATIC NROPT,UNSYM!FULL NEQIT,30 TIME,1E-2 NSUBST,100,1000,20 OUTRES,ALL,ALL KBC,1 SOLVE FINI /POST1 /OUT, ESEL,S,ELEM,,1 !OUTPUT PORE PRESSURE IN ELEMENT 1 PRES,PMSV PRES,EPTO /COM, EXPECTED RESULTS: EVOID=E0+VCE+(1+E0)=0.3453 FINISH