inistate

DataTables.inistate(action='', val1='', val2='', val3='', val4='', val5='', val6='', val7='', val8='', val9='', **kwargs)

Defines initial-state data and parameters.

Mechanical APDL Command: INISTATE

Parameters:

actionstr

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 for Action= SET.

• DEFINE - Use Action = DEFINE to specify the actual state values, and the corresponding element, integration point, or layer information. See Command Specifications for Action= DEFINE.

  Use Action = DEFINE for function-based initial state. See Command Specifications for Action= 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 for Action= WRITE.

• READ - Use Action = READ to read the initial-state values from a file. See Command Specifications for Action= READ.

• LIST - Use Action = LIST to read out the initial-state data. See Command Specifications for Action= LIST.

• DELETE - Use Action = DELE to delete initial-state data from a selected set of elements. See Command Specifications for Action= DELETE

val1str

Input values based on the Action type.

val2str

Input values based on the Action type.

val3str

Input values based on the Action type.

val4str

Input values based on the Action type.

val5str

Input values based on the Action type.

val6str

Input values based on the Action type.

val7str

Input values based on the Action type.

val8str

Input values based on the Action type.

val9str

Input values based on the Action type.

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

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.

The command does not support kinematic hardening material properties (such as tb ,PLAS,,,,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 viscoelasticity ( tb,PRONY, tb,SHIFT).

For more information about using the initial-state capability, see Initial State

Command Specifications

Command Specification for Action= SET

This command contains some tables and extra information which can be inspected in the original documentation pointed above.

Action = SET specifies and modifies the environment into which you will define the initial-state data (via a subsequent inistate,DEFINE command). Otherwise, subsequent inistate,DEFINE data is input as initial stress data in the global Cartesian coordinate system.

Command Specifications for Action= DEFINE

• 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).

• Cxx, Cyy, Czz, Cxy, Cyz, Cxz - Stress (S), strain (EPEL), or plastic strain (EPPL) values.

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)

• 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 FuncName with 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 FuncName with scalars, only two values C1 and C2 ( VALUE = C1 + X* C2 ) are necessary to apply the initial state.

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

• 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.

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 (CPT nnn ) only: CPT212, CPT213, CPT215, CPT216, and CPT217.

Command Specifications for Action= READ

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

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

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.