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
The INISTATE command is available for current-technology elements. Initial state supported for a given element is indicated in the documentation for the element under “Special Features.”
The command is not for use with kinematic hardening material properties (such as TB,BKIN) or the shape memory alloy material model (TB,SMA).
INISTATE with elastic strain alone is not supported for gasket materials (TB,GASK) and hyperelastic materials (TB,HYPER, TB,BB, TB,AHYPER, TB,CDM, TB,EXPE).
INISTATE with initial stress alone is not supported for gasket materials (TB,GASK).
INISTATE with plastic strain (which must include initial strain or stress, plastic strain, and accumulated plastic strain) does not support gasket materials (TB,GASK), rate-dependent plasticity (TB,RATE), and viscoplasticity (TB,PRONY, TB,SHIFT).
|
For detailed information about using the initial state capability, see Initial State in the Mechanical APDL 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 inistate can be activated via the FUNC option. |
Command Specifications for Action = DEFINE
INISTATE, DEFINE, ID, EINT, KLAYER, PARMINT, Cxx, Cyy, Czz,
Cxy, Cyz, Cxz
-
ID-- 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).
For node-based initial state (
Val2= NODE), element ID (if specified). The INISTATE command is applied only to the element ID (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.
-
ParmInt-- Section integration point within a layer, or cell-integration point for beams (typically four integration points). The default value is ALL. 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).
-
Cxx, Cyy, Czz, Cxy, Cyz, Cxz-- Stress (S), strain (EPEL), or plastic strain (EPPL) values.
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), the
ELID value designates the element 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, ID, EINT, --, --, FuncName, C1,
C2, ..., C12
-
ID-- 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+ 2*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.
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.
Notes
Default is 0 for solid elements and -2 for link, beam, and shell elements.
State variables are always written to the .ist file in the material coordinate system.
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
Read initial state data from a standalone initial-state 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. The
INISTATE,READ command is available for
element-integration-point-based initial-state data and node-based initial-state data
(described in Initial-State (.IST) File).
Notes
Use the READ option to apply complex sets of initial state data to various elements, cells, layers, sections and integration points. Fore more information, see Initial State in the Mechanical APDL Advanced Analysis Guide.