MultiPhysicsVault/.raw/AbaqusAnalysisUserGuide5/AbaqusAnalysisUserGuide5_007.md

<!-- source-page: 61 -->

# 34.2.1 INITIAL CONDITIONS IN Abaqus/Standard AND Abaqus/Explicit

Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE

# References

• “Prescribed conditions: overview,” Section 34.1.1   
• \*INITIAL CONDITIONS   
• “Using the predefined field editors,” Section 16.11 of the Abaqus/CAE User’s Guide, in the HTML version of this guide

# Overview

Initial conditions are specified for particular nodes or elements, as appropriate. The data can be provided directly; in an external input file; or, in some cases, by a user subroutine or by the results or output database file from a previous Abaqus analysis.

If initial conditions are not specified, all initial conditions are zero except relative density in the porous metal plasticity model (which will have the value 1.0).

# Specifying the type of initial condition being defined

Various types of initial conditions can be specified, depending on the analysis to be performed. Each type of initial condition is explained below, in alphabetical order.

# Defining initial acoustic static pressure

In Abaqus/Explicit you can define initial acoustic static pressure values at the acoustic nodes. These values should correspond to static equilibrium and cannot be changed during the analysis. You can specify the initial acoustic static pressure at two reference locations in the model, and Abaqus/Explicit interpolates these data linearly to the acoustic nodes in the specified node set. The linear interpolation is based upon the projected position of each node onto the line defined by the two reference nodes. If the value at only one reference location is given, the initial acoustic static pressure is assumed to be uniform. The initial acoustic static pressure is used only in the evaluation of the cavitation condition (see “Acoustic medium,” Section 26.3.1) when the acoustic medium is capable of undergoing cavitation.

Input File Usage: \*INITIAL CONDITIONS, TYPE=ACOUSTIC STATIC PRESSURE

Abaqus/CAE Usage: Initial acoustic static pressure is not supported in Abaqus/CAE.

# Defining initial normalized concentration

In Abaqus/Standard you can define initial normalized concentration values for use with diffusion elements in mass diffusion analysis (see “Mass diffusion analysis,” Section 6.9.1).

Input File Usage: \*INITIAL CONDITIONS, TYPE=CONCENTRATION

Abaqus/CAE Usage: Initial normalized concentration is not supported in Abaqus/CAE.

<!-- source-page: 62 -->

# Defining initially bonded contact surfaces

In Abaqus/Standard you can define initially bonded or partially bonded contact surfaces. This type of initial condition is intended for use with the crack propagation capability (see “Crack propagation analysis,” Section 11.4.3). The surfaces specified have to be different; this type of initial condition cannot be used with self-contact.

If the crack propagation capability is not activated, the bonded portion of the surfaces will not separate. In this case defining initially bonded contact surfaces would have the same effect as defining tied contact, which generates a permanent bond between two surfaces during the entire analysis (“Defining tied contact in Abaqus/Standard,” Section 36.3.7).

Input File Usage: \*INITIAL CONDITIONS, TYPE=CONTACT

Abaqus/CAE Usage: Initially bonded surfaces are not supported in Abaqus/CAE.

# Defining initial damage initiation

You can define initial values for the damage initiation measure for the ductile, shear, and the Müschenborn and Sonne forming limit diagram based damage initiation criteria (“Damage initiation for ductile metals,” Section 24.2.2). This capability is particularly useful in situations where a metal forming operation is carried out in one analysis, which is followed by a separate analysis that subjects the formed metal part to further deformation. The damage initiation measures at the end of the first analysis can be directly specified as initial conditions for the second analysis.

An alternate but approximate way of modeling initial conditions on damage initiation is by specifying the initial values of the equivalent plastic strain. Abaqus computes damage initiation measures based on the specified initial equivalent plastic strain, assuming a linear strain path between the initial (undeformed) state and the final (deformed) state. This approximation does not work well for deformation paths that deviate significantly from linearity in the strain space.

Input File Usage: Use the following option to specify the damage initiation measure for the ductile damage initiation criterion:

\*INITIAL CONDITIONS, TYPE=DAMAGE INITIATION, CRITERION=DUCTILE

Use the following option to specify the damage initiation measure for the shear damage initiation criterion:

\*INITIAL CONDITIONS, TYPE=DAMAGE INITIATION, CRITERION=SHEAR

Use the following option to specify the damage initiation measure for the Müschenborn and Sonne forming limit diagram based damage initiation criterion:

\*INITIAL CONDITIONS, TYPE=DAMAGE INITIATION, CRITERION=MSFLD

Abaqus/CAE Usage: Defining initial values for the damage initiation measures is not supported in Abaqus/CAE.

<!-- source-page: 63 -->

Defining initial damage initiation for rebars

Initial values for damage initiation can also be defined for rebars within elements for the ductile and shear damage initiation criteria (see “Defining rebar as an element property,” Section 2.2.4).

Input File Usage: \*INITIAL CONDITIONS, TYPE=DAMAGE INITIATION, REBAR

Abaqus/CAE Usage: Initial damage initiation for rebars is not supported in Abaqus/CAE.

Defining initial damage initiation that varies through the thickness of shell elements

Initial values of damage initiation can be defined at each section point through the thickness of shell elements for the ductile and shear damage initiation criteria.

Input File Usage: \*INITIAL CONDITIONS, TYPE=DAMAGE INITIATION, SECTION POINTS

Abaqus/CAE Usage: Defining initial damage initiation that varies through the thickness of shell elements is not supported in Abaqus/CAE.

# Define the initial location of an enriched feature

You can specify the initial location of an enriched feature, such as a crack, in an Abaqus/Standard analysis (see “Modeling discontinuities as an enriched feature using the extended finite element method,” Section 10.7.1). Two signed distance functions per node are generally required to describe the crack location, including the location of crack tips, in a cracked geometry. The first signed distance function describes the crack surface, while the second is used to construct an orthogonal surface such that the intersection of the two surfaces defines the crack front. The first signed distance function is assigned only to nodes of elements intersected by the crack, while the second is assigned only to nodes of elements containing the crack tips. No explicit representation of the crack is needed because the crack is entirely described by the nodal data.

Input File Usage: \*INITIAL CONDITIONS, TYPE=ENRICHMENT

Abaqus/CAE Usage: Interaction module: crack editor: Crack location: Specify: select region

# Defining initial values of predefined field variables

You can define initial values of predefined field variables. The values can be changed during an analysis (see “Predefined fields,” Section 34.6.1).

You must specify the field variable number being defined, n. Any number of field variables can be used; each must be numbered consecutively (1, 2, 3, etc.). Repeat the initial conditions definition, with a different field variable number, to define initial conditions for multiple field variables. The default is n=1.

The definition of initial field variable values must be compatible with the section definition and with adjacent elements, as explained in “Predefined fields,” Section 34.6.1.

Input File Usage: \*INITIAL CONDITIONS, TYPE=FIELD, VARIABLE=n

Abaqus/CAE Usage: Initial predefined field variables are not supported in Abaqus/CAE.

<!-- source-page: 64 -->

Initializing predefined field variables with nodal temperature records from a user-specified results file

You can define initial values of predefined field variables using nodal temperature records from a particular step and increment of a results file from a previous Abaqus analysis or from a results file you create (see “Predefined fields,” Section 34.6.1). The previous analysis is most commonly an Abaqus/Standard heat transfer analysis. The use of the .fil file extension is optional.

The part (.prt) file from the previous analysis is required to read the initial values of predefined field variables from the results file (“Defining an assembly,” Section 2.10.1). Both the previous model and the current model must be consistently defined in terms of an assembly of part instances.

Input File Usage: \*INITIAL CONDITIONS, TYPE=FIELD, VARIABLE=n, FILE=file, STEP=step, INC=inc

Abaqus/CAE Usage: Initial predefined field variables are not supported in Abaqus/CAE.

Defining initial predefined field variables using scalar nodal output from a user-specified output database file

You can define initial values of predefined field variables using scalar nodal output variables from a particular step and increment in the output database file of a previous Abaqus/Standard analysis. For a list of scalar nodal output variables that can be used to initialize a predefined field, see “Predefined fields,” Section 34.6.1.

The part (.prt) file from the previous analysis is required to read initial values from the output database file (see “Defining an assembly,” Section 2.10.1). Both the previous model and the current model must be defined consistently in terms of an assembly of part instances; node numbering must be the same, and part instance naming must be the same.

The file extension is optional; however, only the output database file can be used for this option.

Input File Usage: \*INITIAL CONDITIONS, TYPE=FIELD, VARIABLE=n, FILE=file, OUTPUT VARIABLE=scalar nodal output variable, STEP=step, INC=inc

Abaqus/CAE Usage: Initial predefined field variables are not supported in Abaqus/CAE.

Defining initial predefined field variables by interpolating scalar nodal output variables for dissimilar meshes from a user-specified output database file

When the mesh for one analysis is different from the mesh for the subsequent analysis, Abaqus can interpolate scalar nodal output variables (using the undeformed mesh of the original analysis) to predefined field variables that you choose. For a list of supported scalar nodal output variables that can be used to define predefined field variables, see “Predefined fields,” Section 34.6.1. This technique can also be used in cases where the meshes match but the node number or part instance naming differs between the analyses. Abaqus looks for the .odb extension automatically. The part (.prt) file from the previous analysis is required if that analysis model is defined in terms of an assembly of part instances (see “Defining an assembly,” Section 2.10.1).

Input File Usage: \*INITIAL CONDITIONS, TYPE=FIELD, VARIABLE=n, OUTPUT VARIABLE=scalar nodal output variable, INTERPOLATE, FILE=file, STEP=step, INC=inc

<!-- source-page: 65 -->

Abaqus/CAE Usage: Initial predefined field variables are not supported in Abaqus/CAE.

# Defining initial fluid pressure in fluid-filled structures

You can prescribe initial pressure for fluid-filled structures (see “Surface-based fluid cavities: overview,” Section 11.5.1).

Do not use this type of initial condition to define initial conditions in porous media in Abaqus/Standard; use initial pore fluid pressures instead (see below).

Input File Usage: \*INITIAL CONDITIONS, TYPE=FLUID PRESSURE

Abaqus/CAE Usage: Load module: Create Predefined Field: Step: Initial, choose Other for the Category and Fluid cavity pressure for the Types for Selected Step; select a fluid cavity interaction; Fluid cavity pressure: pressure

# Defining initial values of state variables for plastic hardening

You can prescribe initial equivalent plastic strain and, if relevant, the initial backstress tensor for elements that use one of the metal plasticity (“Inelastic behavior,” Section 23.1.1) or Drucker-Prager (“Extended Drucker-Prager models,” Section 23.3.1) material models. These initial quantities are intended for materials in a work hardened state; they can be defined directly or by user subroutine HARDINI. You can also prescribe initial values for the volumetric compacting plastic strain, , $- \varepsilon _ { \mathrm { v o l } } ^ { p l }$ \_pl for elements that use the crushable foam material model with volumetric hardening (“Crushable foam plasticity models,” Section 23.3.5).

You can also specify multiple backstresses for the nonlinear kinematic hardening model. Optionally, you can specify the kinematic shift tensor (backstress) using the full tensor format, regardless of the element type to which the initial conditions are applied.

Input File Usage: \*INITIAL CONDITIONS, TYPE=HARDENING, NUMBER BACKSTRESSES=n, FULL TENSOR

Abaqus/CAE Usage: Load module: Create Predefined Field: Step: Initial, choose Mechanical for the Category and Hardening for the Types for Selected Step; select region; Number of backstresses: n

# Defining hardening parameters for rebars

The hardening parameters can also be defined for rebars within elements. Rebars are discussed in “Defining rebar as an element property,” Section 2.2.4.

Input File Usage: \*INITIAL CONDITIONS, TYPE=HARDENING, REBAR

Abaqus/CAE Usage: Load module: Create Predefined Field: Step: Initial, choose Mechanical for the Category and Hardening for the Types for Selected Step; select region; Definition: Rebar

# Defining hardening parameters in user subroutine HARDINI

For complicated cases in Abaqus/Standard user subroutine HARDINI can be used to define the initial work hardening. In this case Abaqus/Standard will call the subroutine at the start of the analysis for

<!-- source-page: 66 -->

each material point in the model. You can then define the initial conditions at each point as a function of coordinates, element number, etc.

Input File Usage: \*INITIAL CONDITIONS, TYPE=HARDENING, USER

Abaqus/CAE Usage: Load module: Create Predefined Field: Step: Initial, choose Mechanical for the Category and Hardening for the Types for Selected Step; select region; Definition: User-defined

# Defining elements initially open for tangential fluid flow

You can specify the pore pressure cohesive elements that are initially open for tangential fluid flow (see “Defining the constitutive response of fluid within the cohesive element gap,” Section 32.5.7, and “Defining the constitutive response of fluid transitioning from Darcy flow to Poiseuille flow,” Section 32.5.8).

Input File Usage: \*INITIAL CONDITIONS, TYPE=INITIAL GAP

Abaqus/CAE Usage: Initial gap is not supported in Abaqus/CAE.

# Defining initial mass flow rates in forced convection heat transfer elements

In Abaqus/Standard you can define the initial mass flow rate through forced convection heat transfer elements. You can specify a predefined mass flow rate field to vary the value of the mass flow rate within the analysis step (see “Uncoupled heat transfer analysis,” Section 6.5.2).

Input File Usage: \*INITIAL CONDITIONS, TYPE=MASS FLOW RATE

Abaqus/CAE Usage: Initial mass flow rate is not supported in Abaqus/CAE.

# Defining initial values of plastic strain

You can define an initial plastic strain field on elements that use one of the metal plasticity (“Inelastic behavior,” Section 23.1.1), critical state (clay) plasticity (“Critical state (clay) plasticity model,” Section 23.3.4), or Drucker-Prager (“Extended Drucker-Prager models,” Section 23.3.1) material models. The specified plastic strain values will be applied uniformly over the element unless they are defined at each section point through the thickness in shell elements.

If a local coordinate system is defined (see “Orientations,” Section 2.2.5), the plastic strain components must be given in the local system.

Input File Usage: \*INITIAL CONDITIONS, TYPE=PLASTIC STRAIN

Abaqus/CAE Usage: Initial plastic strain conditions are not supported in Abaqus/CAE.

# Defining initial plastic strains for rebars

Initial values of stress can also be defined for rebars within elements ( see “Defining rebar as an element property,” Section 2.2.4).

Input File Usage: \*INITIAL CONDITIONS, TYPE=PLASTIC STRAIN, REBAR

Abaqus/CAE Usage: Initial plastic strain conditions are not supported in Abaqus/CAE.

<!-- source-page: 67 -->

# Defining initial pore fluid pressures in a porous medium

In Abaqus/Standard you can define the initial pore pressure, , for nodes in a coupled pore fluid diffusion/stress analysis (see “Coupled pore fluid diffusion and stress analysis,” Section 6.8.1). The initial pore pressure can be defined either directly as an elevation-dependent function or by user subroutine UPOREP.

# Elevation-dependent initial pore pressures

When an elevation-dependent pore pressure is prescribed for a particular node set, the pore pressure in the vertical direction (assumed to be the z-direction in three-dimensional and axisymmetric models and the y-direction in two-dimensional models) is assumed to vary linearly with this vertical coordinate. You must give two pairs of pore pressure and elevation values to define the pore pressure distribution throughout the node set. Enter only the first pore pressure value (omit the second pore pressure value and the elevation values) to define a constant pore pressure distribution.

Input File Usage: \*INITIAL CONDITIONS, TYPE=PORE PRESSURE

Abaqus/CAE Usage: Load module: Create Predefined Field: Step: Initial: choose Other for the Category and Pore pressure for the Types for Selected Step; select region; Point 1 distribution: Uniform or select an analytical field

# Defining initial pore pressures in user subroutine UPOREP

For complicated cases initial pore pressure values can be defined by user subroutine UPOREP. In this case Abaqus/Standard will make a call to subroutine UPOREP at the start of the analysis for all nodes in the model. You can define the initial pore pressure at each node as a function of coordinates, node number, etc.

Input File Usage: \*INITIAL CONDITIONS, TYPE=PORE PRESSURE, USER

Abaqus/CAE Usage: Load module: Create Predefined Field: Step: Initial: choose Other for the Category and Pore pressure for the Types for Selected Step; select region; Point 1 distribution: User-defined

Defining initial pore pressure values using nodal pore pressure output from a user-specified output database file

You can define initial pore pressure values using nodal pore pressure output variables from a particular step and increment in the output database (.odb) file of a previous Abaqus/Standard analysis. The file extension is optional; however, only the output database file can be used.

For the same mesh pore pressure mapping, both the previous model and the current model must be defined consistently, including node numbering, which must be the same in both models. If the models are defined in terms of an assembly of part instances, the part instance naming must be the same.

Input File Usage: \*INITIAL CONDITIONS, TYPE=PORE PRESSURE, FILE=file, STEP=step, INC=inc

<!-- source-page: 68 -->

Abaqus/CAE Usage: Load module: Create Predefined Field: Step: Initial: choose Other for the Category and Pore pressure for the Types for Selected Step; select region; Point 1 distribution: From output database file

Interpolating initial pore pressure values for dissimilar pore pressure mapping values in a user-specified output database file

For dissimilar mesh pore pressure mapping, interpolation is required. You can also limit the interpolation region by specifying the source region in the form of an element set from which pore pressure is to be interpolated and the target region in the form of a node set onto which the pore pressure is mapped.

Input File Usage: \*INITIAL CONDITIONS, TYPE=PORE PRESSURE, FILE=file, INTERPOLATE, STEP=step, INC=inc \*INITIAL CONDITIONS, TYPE=PORE PRESSURE, FILE=file, INTERPOLATE, STEP=step, INC=inc, DRIVING ELSETS

Abaqus/CAE Usage: You cannot specify the regions where pore pressure values are to be interpolated in Abaqus/CAE.

# Defining initial pressure stress in a mass diffusion analysis

In Abaqus/Standard you can specify the initial pressure stress, $p \ { \stackrel { \mathrm { d e f } } { = } } \ - \mathrm { t r a c e } ( \pmb { \sigma } ) / 3$ , at the nodes in a mass diffusion analysis (see “Mass diffusion analysis,” Section 6.9.1).

Input File Usage: \*INITIAL CONDITIONS, TYPE=PRESSURE STRESS

Abaqus/CAE Usage: Initial pressure stress is not supported in Abaqus/CAE.

Defining initial pressure stress from a user-specified results file

You can define initial values of pressure stress as those values existing at a particular step and increment in the results file of a previous Abaqus/Standard stress/displacement analysis (see “Predefined fields,” Section 34.6.1). The use of the .fil file extension is optional. The initial values of pressure stress cannot be read from the results file when the previous model or the current model is defined in terms of an assembly of part instances (“Defining an assembly,” Section 2.10.1).

Input File Usage: \*INITIAL CONDITIONS, TYPE=PRESSURE STRESS, $\mathrm { F I L E } { = } f i l e , \mathrm { S T E P } { = } s t e p , \mathrm { I N C } { = } i n c$

Abaqus/CAE Usage: Initial pressure stress is not supported in Abaqus/CAE.

# Defining initial void ratios in a porous medium

In Abaqus/Standard you can specify the initial values of the void ratio, e, at the nodes of a porous medium (see “Coupled pore fluid diffusion and stress analysis,” Section 6.8.1). The initial void ratio can be defined either directly as an elevation-dependent function, by interpolation from a previous output database file, or by user subroutine VOIDRI.

<!-- source-page: 69 -->

# Elevation-dependent initial void ratio

When an elevation-dependent void ratio is prescribed for a particular node set, the void ratio in the vertical direction (assumed to be the z-direction in three-dimensional and axisymmetric models and the y-direction in two-dimensional models) is assumed to vary linearly with this vertical coordinate. When the void ratio is specified for a region meshed with fully integrated first-order elements, the nodal values of void ratio are interpolated to the centroid of the element and are assumed to be constant through the element. You must provide two pairs of void ratio and elevation values to define the void ratio throughout the node set. Enter only the first void ratio value (omit the second void ratio value and the elevation values) to define a constant void ratio distribution.

Input File Usage: \*INITIAL CONDITIONS, TYPE=RATIO

Abaqus/CAE Usage: Load module: Create Predefined Field: Step: Initial: choose Other for the Category and Void ratio for the Types for Selected Step; select region; Point 1 distribution: Uniform or select an analytical field

# Defining void ratio from a user-specified output database

You can define initial void ratios from the output database (.odb) file of a previous Abaqus/Standard soil analysis in which the void ratio is requested as output.

Input File Usage: \*INITIAL CONDITIONS, TYPE=RATIO, FILE=file, STEP=step, INC=inc

Abaqus/CAE Usage: Load module: Create Predefined Field: Step: Initial: choose Other for the Category and Void ratio for the Types for Selected Step; select region; Point 1 distribution: From output database file

# Interpolating initial void ratios from values in a user-specified output database

When you define initial void ratios from the output database (.odb) file of a previous Abaqus/Standard soil analysis, you can also limit the interpolation region by specifying the source region in the form of an element set from which void ratios are to be interpolated and the target region in the form of a node set onto which the void ratios are mapped.

Input File Usage: \*INITIAL CONDITIONS, TYPE=RATIO, INTERPOLATE, FILE=file, STEP=step, INC=inc, DRIVING ELSETS

Abaqus/CAE Usage: You cannot specify the regions where void ratios are to be interpolated in Abaqus/CAE.

# Defining void ratios in user subroutine VOIDRI

For complicated cases initial values of the void ratios can be defined by user subroutine VOIDRI. In this case Abaqus/Standard will make a call to subroutine VOIDRI at the start of the analysis for each material integration point in the model. You can then define the initial void ratio at each point as a function of coordinates, element number, etc.

Input File Usage: \*INITIAL CONDITIONS, TYPE=RATIO, USER

<!-- source-page: 70 -->

Abaqus/CAE Usage: Load module: Create Predefined Field: Step: Initial: choose Other for the Category and Void ratio for the Types for Selected Step; select region; Point 1 distribution: User-defined

# Defining a reference mesh for membrane elements

In Abaqus/Explicit you can specify a reference mesh (initial metric) for membrane elements. This is typically useful in finite element airbag simulations to model the wrinkles that arise from the airbag folding process. A flat mesh may be suitable for the unstressed reference configuration, but the initial state may require a corresponding folded mesh defining the folded state. Defining a reference configuration that is different from the initial configuration may result in nonzero stresses and strains in the initial configuration based on the material definition. If a reference mesh is specified for an element, any initial stress or strain conditions specified for the same element are ignored.

If rebar layers are defined in membrane elements, the angular orientation defined in the reference configuration is updated to obtain the same orientation in the initial configuration.

You can define the reference mesh using either the element numbers and the coordinates of the nodes in each element or the node numbers and the coordinates of the nodes. The coordinates of all of the nodes in the element have to be specified for both methods to have a valid initial condition for that element. The two alternatives are mutually exclusive.

Input File Usage: Specifying the reference mesh using element numbers and coordinates of all of the element’s nodes:

\*INITIAL CONDITIONS, TYPE=REF COORDINATE

Specifying the reference mesh using node numbers and the coordinates of the nodes:

\*INITIAL CONDITIONS, TYPE=NODE REF COORDINATE

Abaqus/CAE Usage: The specification of a reference mesh for membrane elements is not supported in Abaqus/CAE.

# Defining initial relative density

You can specify the initial values of the relative density field for a porous metal plasticity material model (see “Porous metal plasticity,” Section 23.2.9) or equations of state (see “Equation of state,” Section 25.2.1).

Input File Usage: \*INITIAL CONDITIONS, TYPE=RELATIVE DENSITY

Abaqus/CAE Usage: Initial relative density is not supported in Abaqus/CAE.

# Defining initial angular and translational velocity

You can prescribe initial velocities in terms of an angular velocity and a translational velocity. This type of initial condition is typically used to define the initial velocity of a component of a rotating machine, such as a jet engine. The initial velocities are specified by giving the angular velocity, ; the axis of rotation, defined from a point a at $\mathbf { X } ^ { a }$ to a point b at $\mathbf { X } ^ { b }$ ; and a translational velocity, $\mathbf { v } ^ { g }$ . The initial velocity of node N at $\mathbf { X } ^ { \bar { N } }$ is then