INISTATE
INISTATE,
Action, Val1,
Val2, Val3,
Val4, Val5,
Val6, Val7,
Val8, Val9,
--
Defines initial-state data and parameters.
-
Action Specifies action for defining or manipulating initial-state data:
SET
—
Use
Action= SET to designate initial-state coordinate system, data type, and material type parameters. See "Command Specification forAction= SET".DEFINE
—
Use
Action= DEFINE to specify the actual state values, and the corresponding element, integration point, or layer information. See "Command Specifications forAction= DEFINE".Use
Action= DEFINE for function-based initial state. See "Command Specifications forAction= DEFINE (Function-Based Option)".WRITE
—
Use
Action= WRITE to write the initial-state values to a file when the SOLVE command is issued. See "Command Specifications forAction= WRITE".READ
—
Use
Action= READ to read the initial-state values from a file. See "Command Specifications forAction= READ".LIST
—
Use
Action= LIST to read out the initial-state data. See "Command Specifications forAction= LIST".DELETE
—
Use
Action= DELE to delete initial-state data from a selected set of elements. See "Command Specifications forAction= DELETE"-
Val1, Val2, ..., Val9 Input values based on the
Actiontype.
Notes
INISTATE is available for current-technology elements.
The command can also be used with MESH200 (via the mesh-independent method for defining reinforcing) to apply an initial state to all generated reinforcing elements automatically. For more information, see Applying an Initial State to Reinforcing Elements in the Structural Analysis Guide.
Initial-state support for a given element is indicated in the documentation for the element under Special Features.
Initial-strain input (INISTATE,SET,DTYPE,EPEL) enables the nonlinear solver option automatically even if no nonlinear materials are involved.
Initial-deformation-gradient input (INISTATE,SET,DTYPE,DEFG) must be provided in the global Cartesian coordinate system (CSYS,0). The initial-deformation gradient defined by INISTATE is the total deformation gradient which can include thermal, plastic, or viscous components.
Also see Initial-State Limitations in the Advanced Analysis Guide.
For more information about using the initial-state capability, see Initial State in the Advanced Analysis Guide.
Command Specification for Action = SET
INISTATE, SET, Val1, Val2
Val1 = |
Val2 = | |||||||||||||
|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|
| CSYS |
Coordinate system.
| |||||||||||||
| DTYP |
Data type.
| |||||||||||||
| MAT | Material type. Val2 is the material
ID. Specifying Val2 = 0 disables
material-based initial state and enables integration-point-based
initial-state data. | |||||||||||||
| NODE | Enable node-based initial
state. When Val2 = 1, all
subsequent INISTATE commands use the node-based
format. To disable node-based initial state, specify
Val2 = 0. | |||||||||||||
| DATA | Input method. By default, the data is discrete at either the node- or element-integration point. Function-based initial state can be activated via the FUNC option. | |||||||||||||
| STOE |
|
Command Specifications for Action = DEFINE
INISTATE, DEFINE, ELID,
EINT, KLAYER,
ParmInt, C01,
C02, C03,
C04, C05,
C06, C07,
C08, C09,
C10, C11,
C12, C13,
C14
-
ELID-- Element ID number when using element-based initial state. Defaults to current element selection.
Node number when using node-based initial state. Defaults to current node selection.
-
EINT-- Gauss integration point. Default = ALL or -1.
For node-based initial state (
Val2= NODE), element ID number (if specified). The INISTATE command is applied only to the specified element (unlike the default behavior, where the command is applied to all selected elements containing the specified node).Not valid for material-based initial-state data (
Val1= MAT) or node-based initial state (Val2= NODE).-
KLAYER-- Layer number (for layered solid/shell elements) or cell number for beam/pipe elements. Blank for other supported element types and material-based initial-state data. Default = ALL or -1.
-
ParmInt-- Section integration point within a layer, or cell-integration point for beams (typically four integration points). Default = ALL or -1. Not valid for material-based initial-state data (
Val1= MAT) or node-based initial state (Val2= NODE).Not valid for material-based initial-state data (
Val1= MAT).Not used for node-based initial state with elements that do not have a beam/pipe/shell section defined.
For node-based initial state with beams/pipes, values 1 through 4 can be used to specify the values at corner nodes within a cell.
For node-based initial state with layered sections, values can be specified at TOP, BOT, and MID, or left blank (ALL or -1).
-
C01, C02, C03, C04, C05, C06, C07, C08, C09, C10, C11, C12, C13, C14-- Components of the initial-state data.
Action= DEFINE limits the number of components to 14. To define more than 14 components, such as components for initial backstress (BSTR) or state variables (SVAR), use an inistate .ist file and INISTATE, READ.The number of components and their order depends on the type of data (DTYP) to be defined:
Stress (S), strain (EPEL), plastic strain (EPPL) or creep strain (EPCR):
Up to six components can be defined: C01, ..., C06=Cxx, Cyy, Czz, Cxy, Cyz, CxzBackstress (BSTR):
The bilinear kinematic hardening (TB,PLASTIC,,,,BKIN) and Chaboche nonlinear kinematic hardening (TB,CHABOCHE) material models are supported. Bilinear kinematic hardening defines all six values ( C01, ..., C06=Cxx,Cyy,Czz,Cxy,Cyz,Cxz), similar to initial stress or initial plastic strain.For the Chaboche model, you can define up to 12 values, so you can use this method for two subchains of the model. The input format is: C01, ..., C12=Cxx1,Cyy1,Czz1,Cxy1,Cyz1,Cxz1,Cxx2,Cyy2,Czz2,Cxy2,Cyz2,Cxz2If more than two subchains of the Chaboche model are required, the initial backstress definition is possible via Action= READ only. The .ist file supports up to five subchains of the Chaboche model. For five subchains of the Chaboche model, for example, the input format becomes:Cxx1,Cyy1,Czz1,Cxy1,Cyz1,Cxz1,…,Cxx5,Cyy5,Czz5,Cxy5,Cyz5,Cxz5For more information, see Applying Initial Backstress in the Advanced Analysis Guide. Also see Bilinear Kinematic Hardening and Nonlinear Kinematic Hardening in the Theory Reference. Accumulated equivalent plastic strain (PLEQ), plastic strain energy density (PLWK), pore pressure (PPRE), void ratio (VOID), relative density (RELD), user-defined fields (UF
nn):For scalar quantities, only one component, C01, is defined.State variables (SVAR):
The number of components depends on the number of user-defined state variables (TB,STATE). The components are defined as: C01, C02, C03, ...=SVAR1, SVAR2, SVAR3, ...Deformation gradient (DEFG):
Nine components must be defined: C01, ..., C09=F11, F21, F31, F12, F22, F32, F13, F23, F33The initial-deformation gradient is defined in the global Cartesian coordinate system (CSYS,0). The determinant of the initial-deformation gradient must be > 0. If an initial-deformation gradient is defined for 2D plane elements, Mechanical APDL applies the following corrections to the defined initial-deformation gradient: – Plane stress, axisymmetric, and generalized plane strain conditions: 
– Plane strain conditions: 
and 
Notes
You can issue the INISTATE command repeatedly to define multiple sets of initial-state values. initial-state data can be specified according to elements, layers or integration points.
When the initial-state parameters are being defined based on the material,
(INISTATE,SET,MAT,MATID),
ELID designates the element ID number and all
subsequent values are ignored.
For coupled-field elements, the stresses to input must be Biot’s effective stresses.
Command Specifications for Action = DEFINE (Function-Based
Option)
INISTATE, DEFINE, ELID, EINT, --, --, FuncName,
C1, C2, ..., C12
-
ELID-- Element ID number when using element-based initial state. Defaults to current element selection.
Node number when using node-based initial state. Defaults to current node selection.
-
EINT-- Gauss integration point (defaults to ALL). Not valid for material-based initial-state data (
Val1= MAT) or node-based initial state (Val2= NODE).- (Blank) --
Reserved for future use.
- (Blank) --
Reserved for future use.
-
FuncName-- LINX | LINY | LINZ. Apply initial-state data as a linear function of location based on the X axis (LINX), Y axis (LINY), or Z axis (LINZ) in the coordinate system specified via the INISTATE,SET,CSYS command. Default coordinate system: CSYS,0 (global Cartesian).
-
C1, C2, ..., C12-- For
FuncNamewith tensors, each component uses two values. SXX =C1+ X*C2, SYY =C3+ X*C4, and so on. Specify 12 values (for the six tensor components).For
FuncNamewith scalars, only two valuesC1andC2(VALUE=C1+ X*C2) are necessary to apply the initial state.
Notes
You can issue INISTATE repeatedly with the function-based option to define multiple sets of initial-state values. Initial-state data can be specified according to elements or integration points.
For coupled-field elements, the stresses to input must be Biot's effective stresses.
Command Specifications for Action = WRITE
INISTATE, WRITE, FLAG, , , , CSID, Dtype
-
FLAG-- Set this value to 1 to generate the initial-state file, or 0 to disable initial-state file generation.
-
CSID-- Determines the coordinate system for the initial state:
- 0 (default)
Write in global Cartesian coordinate system for solid elements.
- -1 (or MAT)
Write in material coordinate system
- -2 (or ELEM)
Write in element coordinate system for link, beam, and layered elements.
-
Dtype-- Sets the data type to be written in the .ist file:
- S
Output stresses.
- EPEL
Output elastic strain.
- EPPL
Output plastic strain.
- PLEQ
Output equivalent plastic strain.
- PLWK
Output plastic strain energy density.
- EPCR
Output creep strain.
- PPRE
Initial pore pressure.
- VOID
Initial void ratio.
- SVAR
State variables.
- BSTR
Initial backstress.
- DEFG
Deformation gradient.
Notes
Default CSID = 0 (global Cartesian
coordinate system) for solid elements, and -2 (element coordinate system) for
link, beam, and shell elements.
State variables are always written to the .ist
file in the material coordinate system (CSID =
-1).
Deformation gradient is always written to the .ist file
in the global Cartesian coordinate system (CSID =
0).
Only the three in-plane stresses for the top and bottom surfaces are written.
For coupled-field elements, the stresses written out are Biot’s effective stress values.
Initial pore pressure and void ratio are available for
the coupled pore-pressure elements (CPTnnn) only:
CPT212, CPT213,
CPT215, CPT216, and
CPT217.
Command Specifications for Action = READ
INISTATE, READ, Fname, Ext, Path,
MeshIndMethod
Reads initial-state data from a standalone initial-state (.ist) file of the specified name
(Fname) and filename extension
(Ext), located in the specified path
(Path). The initial-state file must be in a
comma-delimited ASCII file format, consisting of individual rows for each
stress/strain item, with each row consisting of columns separated by commas.
Use Action = READ to apply complex sets of
initial-state data to various elements, cells, layers, sections, and integration
points. This option is available for element-integration-point-based initial-state
data and node-based initial-state data.
Mapping to nodes may offer better performance when many substeps are involved; however, only location support is available. Mapping to element-integration points supports additional field variables TIME, FREQ and TEMP and generally uses less memory.
For other non-user-defined field variables (such as initial stress or strain), initial state is evaluated only at the first substep in the first load step.
-
MeshIndMethod-- Mesh-Independent method .ist read options:
0 or DEFA -- Standard (mesh-dependent) initial state .ist file (default). MAPN -- Map to nodes internally when applying the initial state. MAPI -- Map to element-integration points. DOBJ -- Do not use .ist data in the finite element solution. (Use this option if converting initial-stress data to a traction load.)
Command Specifications for Action = LIST
INISTATE, LIST, ELID
If using the standard method
for applying initial-state data,specify ELID = element ID
number to list initial-state data for elements. If ELID
is unspecified, all initial-state data for all selected
elements are listed.
If using the mesh-independent method, specify ELID = MIND to
list initial-state data.
Command Specifications for Action = DELETE
INISTATE, DELE, ELID
If using the standard method, specify
ELID = element ID number to delete initial-state data for
elements. If ELID is unspecified,
all initial-state data for all selected elements are
deleted.
If using the mesh-independent method, specify ELID = MIND to
delete initial-state data.