Although initial stress is element-based, the structure of the INISTATE command is element-type-independent.

For continuum or link elements, apply initial stress according to the specific element integration point.

For layered elements, apply initial stress based on the layer number, the layer integration point or the element integration point. Beams allow you to apply initial stress based on the cell number, the section integration point, and/or the element integration point.

For reinforced elements, you can assign different values of initial stress to different reinforcings within the same element.

For coupled-field elements CPT212, CPT213, CPT215, CPT216, and CPT217, the initial stresses to be applied are Biot’s effective stress. They are automatically written out when the output stress option is specified (INISTATE, WRITE, , , , , ,S).

Initial state with stress is supported for hyperelastic materials (TB,HYPER, TB,BB, TB,AHYPER, TB,CDM, TB,EXPE).

The following example input shows how initial stress can be applied in such cases:

Constant Initial Stress on the Whole Model
inistate,defi,,,,,100,200,300,400,500,600

Apply Constant Stress of SX=100 On Beam Element 1
inistate,defi,1,,,,100

Apply a Stress of SX=33.333 at Elem Integration Pt 3 within Element 2
inistate,defi,2,3,,,33.3333	

Apply Constant Stress Of SX=200 in Cell 2 For All Selected Beam Elements
inistate,defi,,,2,,200

Apply Constant Stress Of SX=200 For All Beams In A Model
And Wherever There Is Material=3
inistate,set,mat,3
inistate,defi,,,,,200

Apply a Stress of SX=100,SY=200,SXY=150 for Layers 1,3,5 and
SX=200,SY=0 for Layers 2,4,6 in a Layered Shell Element. Layer
1,3,5 have material 1 and Layer 2,4,6 have material 2.
inistate,defi,,,1,,100,200,150
inistate,defi,,,2,,200
inistate,defi,,,3,,100,200,150
inistate,defi,,,4,,200
inistate,defi,,,5,,100,200,150
inistate,defi,,,6,,200
		OR
inistate,set,mat,1
inistate,defi,,,,,100,200,150
inistate,set,mat,2
inistate,defi,,,,,200 

Apply a Stress of SX=33.333 at Reinf 1 for all elements
inistate,defi,,,1,,33.3333

Also see Example: Initial Stress (Using .ist File) and Example: Initial Stress (INISTATE Command).

After you apply initial stress, Mechanical APDL can convert it to initial strain and apply it (INISTATE,SET,STOE,1).

The initial-stress-to-strain option is available with elastic materials with these solid elements: PLANE182, PLANE183, SOLID185, SOLID186, SOLID187, SOLSH190, SOLID272, and SOLID273.

! Constant initial stress on the whole model
inistate,set,dtyp,s
inistate,defi,,,,,100,0,0,0,0

! Convert initial stress to initial strain
inis,set,stoe,1

Also see Example: Convert Initial Stress to Initial Strain (INISTATE Command).

The initial-stress application example can be extended for initial strain by simply changing the data type to EPEL, as shown.

Initial elastic strain cannot be combined with initial stress. Either, but not both, can be specified in the input.

! Constant Initial Strain on the Whole Model
inistate,set,dtyp,epel
inistate,defi,,,,,0.1,-0.01,-0.01
 
!Apply a Constant Strain of EPEL X=0.01 On Beam Element 1
inistate,set,dtyp,epel
inistate,defi,1,,,,0.01
 
!Apply a Strain of EPEL X=0.01 at Elem Integration Pt 3 within Element 2
inistate,set,dtyp,epel
inistate,defi,2,3,,,0.01
 
!Apply a Constant Strain Of EPEL X = 1E-6 in Cell 2 For All Selected Beam Elements
inistate,set,dtyp,epel
inistate,defi,,,2,,1E-6
 
!Apply a Constant Strain Of EPEL X=1E-3 For All Beams In A Model
!And Wherever There Is Material=3
inistate,set,dtyp,epel
inistate,set,mat,3
inistate,defi,,,,,1E-3
 
! Apply EPS X = 0.1, EPS Y = -0.02, EPS Z = -0.02, for Layers 1,3,5 and
! EPS X = 0.2, for Layers 2,4,6 
! Layer 1,3,5 have material 1 and Layer 2,4,6 have material 2.
inistate,set,mat,1
inistate,defi,,,,,0.1,-0.02,-0.02
inistate,set,mat,2
inistate,defi,,,,,0.2

Also see Example: Initial Strain.

The initial-stress application example can be extended for initial plastic strain by simply changing the data type to EPPL, as shown:

! Constant Initial Plastic Strain and Stress on the Whole Model
inistate,set,dtyp,eppl
inistate,defi,,,,,0.1
inistate,set,dtype,s
inistate,defi,,,,,1000
 
! Apply a Strain of EPEL X=0.01 at Elem Integration Pt 3 within Element 2.
! Here it is assumed that the initial stress is zero.
inistate,set,dtyp,eppl
inistate,defi,2,3,,,0.01

! Apply accumulated equivalent plastic strain.
inistate,set,dtyp,pleq
inistate,defi,2,3,,,0.02
 
! Apply EPS X = 0.1, EPS Y = -0.02, EPS Z = -0.02, for Layers 1,3,5 and
! EPS X = 0.2, for Layers 2,4,6 
! Layer 1,3,5 have material 1 and Layer 2,4,6 have material 2.
inistate,set,dtype,eppl
inistate,set,mat,1
inistate,defi,,,,,2.0
inistate,set,mat,2
inistate,defi,,,,,0.2

Also see Example: Initial Plastic Strain.

The initial-stress application example can be extended for initial creep strain by simply changing the data type to EPCR, as shown:

! Apply creep strain, plastic strain, accumulated equivalent plastic strain, stress on 
! all the selected elements
inistate,set,dtyp,epcr
inistate,defi,,,,,0.005
inistate,set,dtyp,eppl
inistate,defi,,,,,0.1
inistate,set,dtyp,epeq
inistate,defi,,,,,0.02
inistate,set,dtype,s
inistate,defi,,,,,1000

Also see Example: Initial Creep Strain.

To use the initial-state capability with state variables via the INISTATE command, simply change the data type to SVAR, as shown:

! Apply initial state – state variables.
! This fictitious svar example contains 7 components: 
!   The 1st component is accumulated equivalent plastic strain.
!   Components 2-7 are plastic strains values.
! at all the selected elements

inistate,set,dtyp,svar
inistate,defi,,,,,0.005,0.1,-0.02,0.02,0,0,0

The INISTATE command does not consider the coordinate systems of quantities stored within the state variables. It is therefore your responsibility to account for the transformations.

Also see Example: Initial Plastic Strain with State Variables .

As shown below, a node-based initial state can be applied to all nodes or to a selected subset of nodes. Layer numbers can also be specified.

! Enable Node-Based Initial State
inis,set,node,1
! Apply elastic strains at all nodes in layer 1 and 3
inistate,set,dtyp,epel
inistate,defi,all,,1,,0.005
inistate,defi,all,,3,,0.005
! Apply a different elastic strain at all nodes in layer 2
inistate,defi,all,,2,,0.010
! Apply zero elastic strain at node 10
inistate,defi,10,,all,,0.000
! Apply zero elastic strain at node selection
nsel,s,loc,x,0
inistate,defi,all,,all,,0.000

Also see Example: Node-Based Initial Strain.

Initial pore pressure and void ratio are available for coupled pore-pressure-thermal elements (CPTnnn). Apply initial pore pressure and void ratio on CPTnnn elements by changing the data type to PPRE and VOID, respectively.

! Apply to all the selected elements
porepr=69
inistate,set,dtyp,ppre
inistate,defi,,,,,porepr

! Apply to all the selected elements
vratio=0.4
inistate,set,dtyp,void
inistate,defi,,,,,vratio

Also see Example: Initial Pore Pressure and Void Ratio.

Initial degree of saturation and relative permeability are available for coupled pore-pressure-thermal elements (CPTnnn). Apply initial degree of saturation and relative permeability on CPTnnn elements by changing the data type to DSAT and RPER, respectively.

! Apply to all the selected elements
init_sw=0.9
inistate,set,dtyp,dsat
inistate,defi,all,,,,init_sw
init_kr=0.87
inistate,set,dtyp,rper
inistate,defi,all,,,,init_kr

Also see Example: Initial Degree of Saturation and Relative Permeability.

Function-based initial state is a method for applying data as a function of internal variables. Three options are available: a linear function in X coordinates (LINX), a linear function in Y coordinates (LINY), or a linear function in Z coordinates. The method is available for both node-based and element integration-point-based initial state.

The coordinates used to evaluate the value at a given location are based on initial coordinates in the load step. For user-defined field variables, the coordinates are the initial ones queried via the NLIST (or *GET) command. For a rezoning or linear perturbation model (or after issuing an UPGEOM command after a load step) where the coordinates change, the coordinates used in the subsequent load step are the updated coordinates (which become the initial coordinates for the current load step). As before, the coordinates used can be queried if necessary (NLIST or *GET). For other non-user-defined field variables (such as initial stress or strain), function-based initial state is evaluated only at the first substep in the first load step, and only the initial coordinates are used.

For higher-order elements, the initial-state values at the midside nodes are evaluated by averaging the coefficients of the function applied at the corner nodes. A single element must have the same function type at all nodes in the element.

Function-based initial state can also be applied if needed in a user-defined coordinate system. The coordinates needed to evaluate the initial-state data are transformed to the user-defined coordinate system before the evaluation process.

! Apply linearly varying pore pressure in the Y direction
p0=1e3
psl=1.3
inis,set,data,func
inis,set,dtyp,ppre
! Select a subset of elements
esel,s,elem,,1,100
local,11,0,0,0,0,0,0,30
! Change coordinate system if needed
inis,set,csys,11
inis,defi,all,,,,LINY,p0,ps1

Also see Example: Function-Based Initial State.

You can apply an initial backstress for the bilinear kinematic hardening (TB,PLASTIC,,,,BKIN) and Chaboche nonlinear kinematic hardening material models (TB,CHABOCHE). To do so, issue this command:

For plane stress, plane strain, 3D and stress axisymmetric problems, Mechanical APDL converts user-input initial-backstress variables to a deviatoric form and saves them in the material record data. For plane-stress problems, the program converts the deviatoric backstress form into a form specific to the plane-stress state.

To define initial backstress for the BKIN model, or for the CHABOCHE model with up to two subchains, the following general input format applies:

! Constant Initial Plastic Strain and Initial Back Stress on the Whole Model
inistate,set,dtyp,eppl
inistate,defi,,,,,-0.01,0.04,-0.01,0,0,0
inistate,set,dtype,bstr
inistate,defi,,,,,-400,800,-400,0,0,0 


! Apply the back stress values at Elem Integration Pt 3 within Element 2.
! Here it is assumed that the initial stress is zero.
inistate,set,dtyp,bstr
inistate,defi,2,3,,,-400,800,-400,0,0,0


! Apply the back stress for material 1 and material 2.
inistate,set,dtype,bstr
inistate,set,mat,1
inistate,defi,,,,,-400,800,-400,0,0,0
inistate,set,mat,2
inistate,defi,,,,,-300,600,-300,0,0,0


! Apply the back stress and plastic strain for two sub-chain CHAB material on the whole model.
inistate,set,dtyp,eppl
inistate,defi,,,,,-0.01,0.04,-0.01,0,0,0
inistate,set,dtype,bstr
inistate,defi,,,,,-400,800,-400,0,0,0,-300,600,-300,0,0,0


! Apply the back stress and plastic strain for five sub-chain CHAB material on the whole model.
inistate,read,’backstress’,’ist’,,


!in the backstress.ist file, defining:
/dtyp,eppl
All,all,all,all, -0.01,0.04,-0.01,0,0,0
/dtyp,bstr
All,all,all,all,-400,800,-400,0,0,0,-300,600,-300,0,0,0,-200,400,-200,0,0,0,-100,200,-100,0,0,0,-50,100,-50,0,0,0
/dtyp,epel
All,all,all,all,0.001,0.004,0.001,0,0,0

Also see Example: Initial Backstress.

For information about how initial backstress is applied for the supported material models, see Bilinear Kinematic Hardening and Nonlinear Kinematic Hardening in the Theory Reference.

A typical application for the initial-deformation gradient involves an acoustic or fluid-structure interaction (FSI) analysis where the correct stress and stiffness of a hyperelastic material in an updated deformed configuration is required.

Due to the nonlinear behavior of hyperelasticity-based finite-strain material models, such an initial state cannot be consistently defined directly via initial stresses. You can, however, use an initial-deformation gradient to indirectly define an initial-stress state for these material models:

 

4.2.12.1. Initial-Deformation Gradient: Theory Summary

The elastic behavior for the supported material models is already nonlinear. Stresses (such as the Cauchy stress ) are derived from a strain-energy potential , generally a function of the deformation gradient or strain-like quantities derived from it. (See Hyperelasticity in the Theory Reference.)

Generally, strain-energy potentials are defined in such a way that, for an undeformed state (where the deformation gradient is the identity matrix), the stresses are zero. Because of the nonlinear relationships, an initial-stress state cannot be defined directly as is the case for small-strain material models with linear elasticity. It is possible, however, to realize initial stresses in hyperelastic materials by modifying the deformation gradient. By introducing the initial-deformation gradient (INISTATE,SET,DTYP,EFG), the modified deformation gradient is defined as:

The initial-deformation gradient is independent of the element deformation. All element deformations are considered in the original deformation gradient . In the stress calculation, the strain-energy potential is evaluated using the modified deformation gradient:

Accordingly, the strain-energy potential in an undeformed state is evaluated at the initial-deformation gradient, generally resulting in a nonzero initial-stress state at zero deformation:

This approach enables existing strain-energy potentials to be used without modification.

! Apply initial-deformation gradient to all selected elements
! simple shear
gamma=1e-3
inistate,set,dtyp,defg
inistate,defi,all,,,,1.0,0.0,0.0,gamma,1.0,0.0,0.0,0.0,1.0

! Apply initial-deformation gradient to element 1
! pure shear
gamma=1e-3
inistate,set,dtyp,defg
inistate,defi,1,,,,1.0,gamma,0.0,gamma,1.0,0.0,0.0,0.0,1.0

! Apply initial-deformation gradient to all elements with material 1
! uniaxial extension of an incompressible material
Lambda=1.01
inistate,set,dtyp,defg
inistate,set,mat,1
inistate,defi,all,,,,lambda,0.0,0.0,0.0,1.0/sqrt(lambda),0.0,0.0,0.0,1.0/sqrt(lambda)

! Apply initial-deformation gradient to all selected nodes
! pure uniaxial extension (compressible material)
Lambda=1.01
inistate,set,dtyp,defg
inistate,set,node,1
inistate,defi,all,,,,lambda,0.0,0.0,0.0,1.0,0.0,0.0,0.0,1.0