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 ANSYS. 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,miso,11,,3 tbpt,define,5e-5,1e3 tbpt,define,0.010,1e3 tbpt,define,0.600,1e3 ! 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 files 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