Initial Condition Types

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 on 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) 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 Volume Fraction of Material

You can prescribe the initial volume fraction of material in an element in analyses with progressive element activation (see Progressive Element Activation). At the beginning of an analysis the element must be either inactive or fully active; therefore, the value of the initial volume fraction must be equal to zero or one.

Input File Usage

INITIAL CONDITIONS, TYPE=ACTIVATION

Abaqus/CAE Usage

Initial volume fraction of material is not supported in Abaqus/CAE.

Defining Initial Volume Fraction of Material by Importing Field Data from an Output Database File

For three-dimensional continuum elements, you can define the initial volume fraction of material by importing field data as initial values of volume fraction at a particular step and increment or a user-specified time from the output database (.sim) file of a previous analysis. For more information, see Importing Data from an Output Database File.

Input File Usage

Use the following options to define initial values of the volume fraction of material using output from an output database (.sim) file:

INITIAL CONDITIONS, TYPE=ACTIVATION
EXTERNAL FIELD, FILE=file name

Abaqus/CAE Usage

Defining the initial volume fraction of material by importing field data from an output database (.sim) file 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).

Input File Usage

INITIAL CONDITIONS, TYPE=CONCENTRATION

Abaqus/CAE Usage

Initial normalized concentration is not supported in Abaqus/CAE.

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). 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 do 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).

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). 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.

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).

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.

Defining Initial Damage Initiation by Importing Field Data from an Output Database File

For three-dimensional continuum elements, you can define initial ductile and shear damage initiation criteria by importing field data as initial values of damage initiation at a particular step and increment or a user-specified time in the output database (.sim) file of a previous analysis. For more information, see Importing Data from an Output Database File.

Input File Usage

Use the following options to define initial values of ductile damage initiation using ductile damage initiation criterion output from an output database (.sim) file:

INITIAL CONDITIONS, TYPE=DAMAGE INITIATION, CRITERION=DUCTILE
EXTERNAL FIELD, FILE=file name

Use the following options to define initial values of shear damage initiation using shear damage initiation criterion output from a user-specified output database (.sim) file.

INITIAL CONDITIONS, TYPE=DAMAGE INITIATION, CRITERION=SHEAR
EXTERNAL FIELD, FILE=file name

Abaqus/CAE Usage

Defining initial damage initiation by importing field data from an output database (.sim) file is not supported in Abaqus/CAE.

Defining 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). 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 Element Solution-Dependent Variables

You can define initial values of solution-dependent state variables (see About User Subroutines and Utilities). The initial values can be defined directly.

Input File Usage

INITIAL CONDITIONS, TYPE=ESDV

Abaqus/CAE Usage

Initial element solution-dependent variables are not supported in Abaqus/CAE.

Defining Initial Values of Element Solution-Dependent Variables from an Output Database File

For three-dimensional continuum elements, you can define initial values of element solution-dependent variables by importing field data as initial values of element solution-dependent variables at a particular step and increment or a user-specified time in the output database (.sim) file of a previous analysis. For more information, see Importing Data from an Output Database File.

Input File Usage

INITIAL CONDITIONS, TYPE=ESDV
EXTERNAL FIELD, FILE=file name
 , , ESDVi, , , ESDVi
…
 , , ESDVn, , , ESDVn

Abaqus/CAE Usage

Defining initial element solution-dependent variables by importing field data from an output database (.sim) file is not supported in Abaqus/CAE.

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).

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.

Input File Usage

INITIAL CONDITIONS, TYPE=FIELD, VARIABLE=n

Abaqus/CAE Usage

Load module: Create Predefined Field: Step: Initial, choose Other for the Category and Field for the Types for Selected Step; select region; Field variable number: n

Defining Uniform Initial Fields

You can apply uniform initial field variables to either the entire model or to node sets that you specify. Omit the node number or node set to apply the specified field variable to all nodes in the model automatically.

You can specify uniform field variables with all element types, including beams and shells. The specified uniform field is applied to all section points in beams and shells. However, the definition of initial field variables must be compatible with the section definition of the element and with adjacent elements, as explained in Predefined Fields. Abaqus issues a warning message during input file preprocessing if an initial field variable is applied to any node that is associated with at least one shell or beam section that specifies field variables using gradients and at least one section that directly specifies the values of the field variables.

Input File Usage

INITIAL CONDITIONS, TYPE=FIELD, VARIABLE=n, SECTION SPECIFICATION=UNIFORM

Abaqus/CAE Usage

Defining uniform initial fields is not supported in Abaqus/CAE.

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). 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 (Assembly Definition). 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

Load module: Create Predefined Field: Step: Initial, choose Other for the Category and Field for the Types for Selected Step; select region; Field variable number: n, File name: file, Step: step, Increment: inc

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.

The part (.prt) file from the previous analysis is required to read initial values from the output database file (see Assembly Definition). 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

Load module: Create Predefined Field: Step: Initial, choose Other for the Category and Field for the Types for Selected Step; select region; Field variable number: n, File name: file, Output variable: scalar nodal output variable, Step: step, Increment: inc

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. 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 Assembly Definition).

Input File Usage

INITIAL CONDITIONS, TYPE=FIELD, VARIABLE=n,
OUTPUT VARIABLE=scalar nodal output variable,
INTERPOLATE, FILE=file,  STEP=step, INC=inc

Abaqus/CAE Usage

Load module: Create Predefined Field: Step: Initial, choose Other for the Category and Field for the Types for Selected Step; select region; Field variable number: n, File name: file, Output variable: scalar nodal output variable, Step: step, Increment: inc, Mesh compatibility: Incompatible

Defining Initial Predefined Field Variables by Importing Field Data from an Output Database File

For three-dimensional continuum elements, you can define initial predefined field variables by importing field data at a particular step and increment or a user-specified time in the output database (.sim) file of a previous analysis. For more information, see Importing Data from an Output Database File.

Input File Usage

Use the following options to define initial values of predefined field variables using output variables from an output database (.sim) file:

INITIAL CONDITIONS, TYPE=FIELD, VARIABLE=n,
EXTERNAL FIELD, FILE=file name

Abaqus/CAE Usage

Defining initial predefined field variables by importing field data from an output database (.sim) file is not supported in Abaqus/CAE.

Defining Initial Predefined Pore Fluid Pressure

You can associate a known (precomputed) pore fluid pressure field with a specific predefined field variable (as discussed in Predefined Fields) and read the field into a static or an explicit dynamic stress analysis. To initialize the pore fluid pressure field, you must initialize the corresponding predefined field variable.

Input File Usage

Use the following option to define initial values of predefined pore fluid pressure, where it is assumed that field variable n is associated with the known pore fluid pressure field:

INITIAL CONDITIONS, TYPE=FIELD, VARIABLE=n

Abaqus/CAE Usage

Defining initial predefined pore fluid pressure is not supported in Abaqus/CAE.

Defining Initial Fluid Electric Potential

In Abaqus/Standard you can define initial fluid electric potential values for use with coupled thermal-electrochemical elements in a coupled thermal-electrochemical analysis (see Coupled Thermal-Electrochemical Analysis).

Input File Usage

INITIAL CONDITIONS, TYPE=FLUID ELECTRIC POTENTIAL

Abaqus/CAE Usage

Initial fluid electric potential is not supported in Abaqus/CAE.

Defining Initial Fluid Pressure in Fluid-Filled Structures

You can prescribe initial pressure for fluid-filled structures (see About Surface-Based Fluid Cavities).

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) or Drucker-Prager (Extended Drucker-Prager Models) 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, $- ε_{vol}^{p l}$ , for elements that use the crushable foam material model with volumetric hardening (Crushable Foam Plasticity Models).

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 Initial Equivalent Plastic Strain by Importing Field Data from an Output Database File

For three-dimensional continuum elements, you can define initial equivalent plastic strain by importing field data as equivalent plastic strain at a particular step and increment or a user-specified time in the output database (.sim) file of a previous analysis. For more information, see Importing Data from an Output Database File.

Input File Usage

INITIAL CONDITIONS, TYPE=HARDENING
EXTERNAL FIELD, FILE=file name

Abaqus/CAE Usage

Defining initial equivalent plastic strain by importing field data from an output database (.sim) file is not supported in Abaqus/CAE.

Defining Initial Equivalent Plastic Strain and Backstress Tensor by Importing Field Data from an Output Database File

For three-dimensional continuum elements, you can define initial equivalent plastic strain and backstress tensor by importing field data as equivalent plastic strain and backstress tensor at a particular step and increment or a user-specified time in the output database (.sim) file of a previous analysis. For more information, see Importing Data from an Output Database File.

Input File Usage

INITIAL CONDITIONS, TYPE=HARDENING, NUMBER BACKSTRESSES=n
EXTERNAL FIELD, FILE=file name
 , , PEEQ, , , PEEQ
 , , ALPHAi, , , ALPHAi
…
 , , ALPHAn, , , ALPHAn

Abaqus/CAE Usage

Defining initial equivalent plastic strain and backstress tensor by importing field data from an output database (.sim) file is not supported in Abaqus/CAE.

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.

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 calls the subroutine at the start of the analysis for 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 and Defining the Constitutive Response of Fluid Transitioning from Darcy Flow to Poiseuille Flow).

Input File Usage

INITIAL CONDITIONS, TYPE=INITIAL GAP

Abaqus/CAE Usage

Initial gap is not supported in Abaqus/CAE.

Defining Initial Ion Concentration

In Abaqus/Standard you can define initial ion concentration values for use with coupled thermal-electrochemical elements in a coupled thermal-electrochemical analysis (see Coupled Thermal-Electrochemical Analysis).

Input File Usage

INITIAL CONDITIONS, TYPE=ION CONCENTRATION

Abaqus/CAE Usage

Initial ion concentration 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).

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), critical state (clay) plasticity (Critical State (Clay) Plasticity Model), Drucker-Prager (Extended Drucker-Prager Models), or soft rock plasticity models. The specified plastic strain values are 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), 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 plastic strains can also be defined for rebars within elements ( see Defining Rebar as an Element Property).

Input File Usage

INITIAL CONDITIONS, TYPE=PLASTIC STRAIN, REBAR

Abaqus/CAE Usage

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

Defining Initial Plastic Strains by Importing Field Data from an Output Database File

For three-dimensional continuum elements, you can define initial plastic strains by importing field data as initial plastic strains at a particular step and increment or a user-specified time in the output database (.sim) file of a previous analysis. For more information, see Importing Data from an Output Database File.

Input File Usage

INITIAL CONDITIONS, TYPE=PLASTIC STRAIN
EXTERNAL FIELD, FILE=file name

Abaqus/CAE Usage

Defining initial plastic strains by importing field data from an output database (.sim) file is not supported in Abaqus/CAE.

Defining Initial Pore Fluid Pressures in a Porous Medium

In Abaqus/Standard you can define the initial pore pressure, $u_{w}$ , for nodes in a coupled pore fluid diffusion/stress analysis (see Coupled Pore Fluid Diffusion and Stress Analysis). 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 makes 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

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, $p \overset{def}{=} - trace (σ) / 3$ , at the nodes in a mass diffusion analysis (see Mass Diffusion Analysis).

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). 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 (Assembly Definition).

Input File Usage

INITIAL CONDITIONS, TYPE=PRESSURE STRESS, FILE=file, STEP=step, INC=inc

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). 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.

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 makes 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

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 and Three-Dimensional Solid Elements

In Abaqus/Explicit you can specify a reference mesh (initial metric) for membrane elements and three-dimensional solid elements. For membrane elements, this is typically useful in airbag simulations to model the wrinkles that arise from the airbag folding process. A flat mesh might be suitable for the unstressed reference configuration, but the initial state might require a corresponding folded mesh defining the folded state. For solid elements, defining a reference mesh provides a convenient way to initialize stresses due to dummy positioning/settling in crash applications. Defining a reference configuration that is different from the initial configuration results in nonzero stresses in the initial configuration based on the elastic response of the material. For membrane elements, it can also result in nonzero strains relative to the reference configuration. For solids elements, initial strains are measured with respect to the initial configuration and are reported as zero. If a reference mesh is specified for an element, any initial stress conditions specified for the same element are ignored.

In the reference mesh method, the deformation gradient defined by the reference and initial configurations is used to update the stress state of the material in total form assuming purely elastic behavior. Therefore, the method is intended primarily for elastic or hyperelastic materials for which the stress state does not depend on deformation history. For plastic materials, the initial stresses computed by the reference mesh method might violate yield, and it might take several increments in an Abaqus/Explicit analysis for the stresses to settle and return back onto the yield surface. The reference mesh method provides a convenient way to initialize stresses in air bags, dummies, and other components in crash applications and provides an alternative solution to running an import analysis. For elements with internal nodes that you cannot access (such as C3D8I, C3D10M, and C3D10 elements), the initial stresses computed based on the user-defined reference mesh might not be the same as the initial stresses obtained from an import analysis. However, for most cases, the initial stresses obtained from these two methods should be reasonably close.

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.

For membrane elements, you can define the reference mesh either with the element numbers and the coordinates of the nodes in each element or with the node numbers and node coordinates. For three-dimensional solid elements, you can only define the reference mesh using the node numbers and the corresponding node coordinates. For both methods, you must specify the coordinates of all the nodes in the element to have a valid initial condition for that element. The two methods are mutually exclusive.

If you define a reference mesh, the strain output is calculated based on the reference configuration for membrane elements; however, for three-dimensional solid elements, the strain output is based on the initial configuration. Therefore, you might observe nonzero initial strains and stresses for membrane elements and only nonzero initial stresses for three-dimensional solid elements.

Input File Usage

Use the following option to specify the reference mesh using element numbers and coordinates of all the element's nodes (applies only to membrane elements):

INITIAL CONDITIONS, TYPE=REF COORDINATE

Use the following option to specify the reference mesh using node numbers and the coordinates of the nodes (applies to membrane elements and three-dimensional solid elements):

INITIAL CONDITIONS, TYPE=NODE REF COORDINATE

Abaqus/CAE Usage

Specifying a reference mesh for membrane and three-dimensional solid 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) or equations of state (see Equation of State).

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, $ω$ ; the axis of rotation, defined from a point a at $X^{a}$ to a point b at $X^{b}$ ; and a translational velocity, $v^{g}$ . The initial velocity of node N at $X^{N}$ is then

$v^{N} = v^{g} + ω \frac{(X^{b} - X^{a})}{| X^{b} - X^{a} |} \times (X^{N} - X^{a}) .$

Input File Usage

INITIAL CONDITIONS, TYPE=ROTATING VELOCITY

Abaqus/CAE Usage

Load module: Create Predefined Field: Step: Initial: choose Mechanical for the Category and Velocity for the Types for Selected Step

Defining Initial Saturation for a Porous Medium

In Abaqus/Standard you can define the initial saturation, s, for elements in a coupled pore fluid diffusion/stress analysis (see Coupled Pore Fluid Diffusion and Stress Analysis). If the porous material's absorption/exsorption behavior under partially saturated flow conditions is not defined, the initial saturation is set to 1.0 by default.

Input File Usage

INITIAL CONDITIONS, TYPE=SATURATION

Abaqus/CAE Usage

Load module: Create Predefined Field: Step: Initial: choose Other for the Category and Saturation for the Types for Selected Step

Defining Initial Solid Electric Potential

In Abaqus/Standard you can define initial solid electric potential values for use with coupled thermal-electrochemical elements in a coupled thermal-electrochemical analysis (see Coupled Thermal-Electrochemical Analysis).

Input File Usage

INITIAL CONDITIONS, TYPE=SOLID ELECTRIC POTENTIAL

Abaqus/CAE Usage

Initial solid electric potential is not supported in Abaqus/CAE.

Defining the Initial Values of Solution-Dependent State Variables

You can define initial values of solution-dependent state variables (see About User Subroutines and Utilities). The initial values can be defined directly or, in Abaqus/Standard, by user subroutine SDVINI. Values given directly are applied uniformly over the element.

Input File Usage

INITIAL CONDITIONS, TYPE=SOLUTION

Abaqus/CAE Usage

Initial solution-dependent variables are not supported in Abaqus/CAE.

Defining the Initial Values of Solution-Dependent State Variables by Importing Field Data from an Output Database File

For three-dimensional continuum elements, you can define initial values of solution-dependent state variables by importing field data as initial values of solution-dependent state variables at a particular step and increment or a user-specified time from the output database (.sim) file of a previous analysis. For more information, see Importing Data from an Output Database File.

Input File Usage

INITIAL CONDITIONS, TYPE=SOLUTION
EXTERNAL FIELD, FILE=file name
 , , SDVi, , , SDVi
…
 , , SDVn, , , SDVn

Abaqus/CAE Usage

Defining initial solution-dependent state variables by importing field data from an output database (.sim) file is not supported in Abaqus/CAE.

Defining the Initial Values of Solution-Dependent State Variables for Rebars

The initial values of solution-dependent variables can also be defined for rebars within elements. Rebars are discussed in Defining Rebar as an Element Property.

Input File Usage

INITIAL CONDITIONS, TYPE=SOLUTION, REBAR

Abaqus/CAE Usage

Initial solution-dependent state variables are not supported in Abaqus/CAE.

Defining the Initial Values of Solution-Dependent State Variables in User Subroutine SDVINI

For complicated cases in Abaqus/Standard user subroutine SDVINI can be used to define the initial values of solution-dependent state variables. In this case Abaqus/Standardmakes a call to subroutine SDVINI at the start of the analysis for each material integration point in the model. You can then define all solution-dependent state variables at each point as functions of coordinates, element number, etc.

Input File Usage

INITIAL CONDITIONS, TYPE=SOLUTION, USER

Abaqus/CAE Usage

User subroutine SDVINI is not supported in Abaqus/CAE.

Defining Initial Specific Energy for Equations of State

In Abaqus/Explicit you can specify the initial values of the specific energy for equations of state (see Equation of State).

Input File Usage

INITIAL CONDITIONS, TYPE=SPECIFIC ENERGY

Abaqus/CAE Usage

Initial specific energy is not supported in Abaqus/CAE.

Defining Spud Can Embedment or Spud Can Preload

In Abaqus/Standard you can define an initial embedment of a spud can. Alternatively, you can define an initial vertical preload of a spud can (see Elastic-Plastic Joints).

Input File Usage

Use one of the following options:

INITIAL CONDITIONS, TYPE=SPUD EMBEDMENT
INITIAL CONDITIONS, TYPE=SPUD PRELOAD

Abaqus/CAE Usage

Initial spud can embedment and preload are not supported in Abaqus/CAE.

Defining Initial Stresses

You can define an initial stress field. Initial stresses can be defined directly or, in Abaqus/Standard, by user subroutine SIGINI. Stress values given directly are applied uniformly over the element unless they are defined at each section point through the thickness in shell elements.

If a local coordinate system was defined (see Orientations), stresses must be given in the local system.

In soils (porous medium) problems the initial effective stress should be given; see Coupled Pore Fluid Diffusion and Stress Analysis for a discussion of defining initial conditions in porous media.

If the section properties of beam elements or shell elements are defined by a general section, the initial stress values are applied as initial section forces and moments. In the case of beams initial conditions can be specified only for the axial force, the bending moments, and the twisting moment. In the case of shells initial conditions can be specified only for the membrane forces, the bending moments, and the twisting moment. In both shells and beams initial conditions cannot be prescribed for the transverse shear forces.

Initial contact stresses are calculated internally (see Initial Contact Stresses in Abaqus/Standard) by default providing initial conditions for contact. These initial contact stress computations use the initial stresses that you specify in the underlying elements of the contact surfaces and are meant to provide an approximate equilibrating contact traction at contact interfaces.

Initial stress fields cannot be defined for spring elements. See Springs for a discussion of defining initial forces in spring elements.

Initial stress fields cannot be defined for elements using a fabric material. However, an initial stress and strain state can be introduced in a fabric material made of membrane elements by defining a reference mesh (see Defining a Reference Mesh for Membrane Elements and Three-Dimensional Solid Elements above).

Input File Usage

INITIAL CONDITIONS, TYPE=STRESS

Abaqus/CAE Usage

Load module: Create Predefined Field: Step: Initial: choose Mechanical for the Category and Stress for the Types for Selected Step

Defining Initial Stresses for Rebars

Initial values of stress can also be defined for rebars within elements (see Defining Rebar as an Element Property).

Input File Usage

INITIAL CONDITIONS, TYPE=STRESS, REBAR

Abaqus/CAE Usage

Initial stress for rebars is not supported in Abaqus/CAE.

Defining Initial Stresses That Vary through the Thickness of Shell Elements

Initial values of stress can be defined at each section point through the thickness of shell elements.

Input File Usage

INITIAL CONDITIONS, TYPE=STRESS, SECTION POINTS

Abaqus/CAE Usage

Defining initial stress that varies through the thickness of shell elements is not supported in Abaqus/CAE.

Defining Initial Stresses in User Subroutine SIGINI

For complicated cases (such as elbow elements) in Abaqus/Standard the initial stress field can be defined by user subroutine SIGINI. In this case Abaqus/Standard makes a call to subroutine SIGINI at the start of the analysis for each material calculation point in the model. You can then define all active stress components at each point as functions of coordinates, element number, etc.

Input File Usage

INITIAL CONDITIONS, TYPE=STRESS, USER

Abaqus/CAE Usage

User subroutine SIGINI is not supported in Abaqus/CAE.

Defining Initial Stresses Using Stress Output from a User-Specified Output Database File

You can define initial stresses using stress output variables from a particular step and increment in the output database (.odb or .sim) file of a previous Abaqus/Standard analysis. This option is available only for continuum elements when the stress output in the previous analysis was requested at the integration points or at the centroid of the element.

In this case both the previous model and the current model must be defined consistently. The element numbering and element types must be the same in both models. If the models are defined in terms of an assembly of part instances, part instance naming must be the same.

The file extension is optional; however, only the output database (.odb or .sim) file can be used. If no extension is specified, the .odb file is used.

Input File Usage

INITIAL CONDITIONS, TYPE=STRESS, FILE=file, STEP=step, INC=inc

Abaqus/CAE Usage

Load module: Create Predefined Field: Step: Initial: choose Mechanical for the Category and Stress for the Types for Selected Step; select region; Specification: From output database file

Defining Initial Stresses by Importing Field Data from an Output Database File

For three-dimensional continuum elements, you can define initial stresses by importing field data from a particular step and increment or a user-specified time in the output database (.sim) file of a previous analysis. For more information, see Importing Data from an Output Database File.

Input File Usage

INITIAL CONDITIONS, TYPE=STRESS
EXTERNAL FIELD, FILE=file name

Abaqus/CAE Usage

Defining initial stresses by importing field data from an output database (.sim) file is not supported in Abaqus/CAE.

Establishing Equilibrium in Abaqus/Standard

When initial stresses are given in Abaqus/Standard (including prestressing in reinforced concrete or interpolation of an old solution onto a new mesh), the initial stress state may not be an exact equilibrium state for the finite element model. Therefore, an initial step should be included to allow Abaqus/Standard to check for equilibrium and iterate, if necessary, to achieve equilibrium.

In a soils analysis (that is, for models containing elements that include pore fluid pressure as a variable) the geostatic stress field procedure (Geostatic Stress State) should be used for the equilibrating step. Any initial loading (such as geostatic gravity loads) that contributes to the initial equilibrium should be included in this step definition. The initial time increment and the total time specified in this step should be the same. The initial stresses are applied in full at time zero; and if equilibrium can be achieved, this step converges in one increment. Therefore, there is no benefit to incrementing.

To achieve equilibrium for all other analyses, a first step using the static procedure (Static Stress Analysis) should be used. It is recommended that you specify the initial time increment to be equal to the total time specified in this step so that Abaqus/Standard attempts to find equilibrium in one increment.

By default, Abaqus/Standard adopts a ramping technique over the first step. This allows Abaqus/Standard to use automatic incrementation if equilibrium cannot be found in one increment. This ramping is achieved in the following manner:

An additional set of artificial or unbalanced stresses is defined at each material point. These stresses are equal in magnitude to the initial stresses but are of opposite sign. Therefore, the sum of the material point initial stresses and these artificial stresses creates zero internal forces at the beginning of the step.
The internal unbalanced stresses are ramped off linearly in time during the first step. Therefore, at the end of the step the artificial stresses have been removed completely and the remaining stresses in the material are the stress state in equilibrium.

You can force Abaqus/Standard to achieve equilibrium in one increment by using a step variation on the initial condition to resolve the unbalanced stress instead of ramping the stress down over the entire step. If Abaqus/Standard cannot achieve equilibrium in one increment, the analysis ends.

If the equilibrating step does not converge, it indicates that the initial stress state is so far from equilibrium with the applied loads that significantly large deformations would be generated. This is generally not the intention of an initial stress state; therefore, it suggests that you should recheck the specified initial stresses and loads.

Input File Usage

Use one of the following options to specify how the unbalanced stress should be resolved:

INITIAL CONDITIONS, TYPE=STRESS,
UNBALANCED STRESS=RAMP (default)
INITIAL CONDITIONS, TYPE=STRESS,
UNBALANCED STRESS=STEP

Abaqus/CAE Usage

Initial equilibrium stress is not supported in Abaqus/CAE.

Establishing Equilibrium in Abaqus/Explicit

Abaqus/Explicit computes the initial acceleration at nodes taking into account the initial stresses, the loads, and the boundary conditions in the initial configuration. For an initially static problem, the specified boundary conditions, the initial stresses, and the initial loading should be consistent with a static equilibrium. Otherwise, the solution is likely to be noisy. The noise may be reduced by introducing a dummy step with a temporary viscous loading to attempt to reestablish a static equilibrium. Alternatively, you can introduce an initial short step in which all degrees of freedom are fixed with boundary conditions (all initial loads should be included in this initial step); in a second step, release all but the actual boundary conditions.

Defining Elevation-Dependent (Geostatic) Initial Stresses

You can define elevation-dependent initial stresses. When a geostatic stress state is prescribed for a particular element set, the stress 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 (piecewise) linearly with this vertical coordinate.

For the vertical stress component, you must give two pairs of stress and elevation values to define the stress throughout the element set. For material points lying between the two elevations given, Abaqus will use linear interpolation to determine the initial stress; for points lying outside the two elevations given, Abaqus will use linear extrapolation. In addition, horizontal (lateral) stress components are given by entering one or two “coefficients of lateral stress,” which define the lateral direct stress components as the vertical stress at the point multiplied by the value of the coefficient. In axisymmetric cases only one value of the coefficient of lateral stress is used and, therefore, only one value need be entered.

Geostatic initial stresses are for use with continuum elements only. In Abaqus/Standard elevation-dependent initial stresses should be specified for beams and shells in user subroutine SIGINI, as explained earlier. In Abaqus/Explicit elevation-dependent initial stresses cannot be specified for beams and shells.

The geostatic stress state specified initially should be in equilibrium with the applied loads (such as gravity) and boundary conditions. An initial step should be included to allow Abaqus to check for equilibrium after this interpolation has been done; see the discussion above on establishing equilibrium when an initial stress field is applied.

Input File Usage

INITIAL CONDITIONS, TYPE=STRESS, GEOSTATIC

Abaqus/CAE Usage

Load module: Create Predefined Field: Step: Initial: choose Mechanical for the Category and Geostatic stress for the Types for Selected Step

Defining Initial Temperatures

You can define initial temperatures at the nodes of either heat transfer or stress/displacement elements. The temperatures of stress/displacement elements can be changed during an analysis (see Predefined Fields).

The definition of initial temperature values must be compatible with the section definition of the element and with adjacent elements, as explained in Predefined Fields.

Input File Usage

INITIAL CONDITIONS, TYPE=TEMPERATURE

Abaqus/CAE Usage

Load module: Create Predefined Field: Step: Initial: choose Other for the Category and Temperature for the Types for Selected Step

Defining Uniform Initial Temperatures

You can apply uniform initial temperatures to either the entire model or to node sets that you specify. Omit the node number or node set to apply the specified temperature to all nodes in the model automatically.

You can specify uniform temperature with all element types, including beams and shells. The specified uniform temperature is applied to all section points in beams and shells. However, the definition of initial temperature values must be compatible with the section definition of the element and with adjacent elements, as explained in Predefined Fields. Abaqus issues a warning message during input file preprocessing if an initial temperature is applied to any node that is associated with at least one shell or beam section that specifies temperatures using gradients and at least one section that directly specifies the values of temperature.

Input File Usage

INITIAL CONDITIONS, TYPE=TEMPERATURE, SECTION SPECIFICATION=UNIFORM

Abaqus/CAE Usage

Defining uniform initial temperatures is not supported in Abaqus/CAE.

Defining Initial Temperatures from a User-Specified Results or Output Database File

You can define initial temperatures as those values existing as nodal temperatures at a particular step and increment in the results or output database file of a previous Abaqus/Standard heat transfer analysis (see Predefined Fields).

The part (.prt) file from the previous analysis is required to read initial temperatures from the results or output database file (see Assembly Definition). Both the previous model and the current model must be consistently defined 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, if both results and output database files exist, the results file will be used.

Input File Usage

INITIAL CONDITIONS, TYPE=TEMPERATURE, FILE=file, STEP=step, INC=inc

Abaqus/CAE Usage

Load module: Create Predefined Field: Step: Initial: choose Other for the Category and Temperature for the Types for Selected Step: select region: Distribution: From results or output database file, File name: file, Step: step, and Increment: inc

Defining Initial Temperatures by Importing Field Data from an Output Database File

For three-dimensional continuum elements, you can define initial temperatures by importing field data as nodal temperatures at a particular step and increment or a user-specified time in the output database (.sim) file of a previous analysis. For more information, see Importing Data from an Output Database File.

Input File Usage

INITIAL CONDITIONS, TYPE=TEMPERATURE
EXTERNAL FIELD, FILE=file name

Abaqus/CAE Usage

Defining initial temperatures by importing field data from an output database (.sim) file is not supported in Abaqus/CAE.

Interpolating Initial Temperatures for Dissimilar Meshes from a User-Specified Results or Output Database File

When the mesh for the heat transfer analysis is different from the mesh for the subsequent stress/displacement analysis, Abaqus can interpolate the temperature values from the nodes in the undeformed heat transfer model to the current nodal temperatures. This technique can also be used in cases where the meshes match but the node number or part instance naming differs between the analyses. Only temperatures from an output database file can be used for the interpolation; Abaqus will look 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 Assembly Definition).

Input File Usage

INITIAL CONDITIONS, TYPE=TEMPERATURE, INTERPOLATE, 
FILE=file, STEP=step, INC=inc

Abaqus/CAE Usage

Load module: Create Predefined Field: Step: analysis_step: choose Other for the Category and Temperature for the Types for Selected Step: select region: Distribution: From results or output database file, File name: file, Mesh compatibility: Incompatible

Interpolating Initial Temperatures for Dissimilar Meshes with User-Specified Regions

When regions of elements in the heat transfer analysis are close or touching, the dissimilar mesh interpolation capability can result in an ambiguous temperature association. For example, consider a node in the current model that lies on or close to a boundary between two adjacent parts in the heat transfer model, and consider a case where temperatures in these parts are different. When interpolating, Abaqus will identify a corresponding parent element at the boundary for this node from the heat transfer analysis. This parent element identification is done using a tolerance-based search method. Hence, in this example the parent element might be found in either of the adjacent parts, resulting in an ambiguous temperature definition at the node. You can eliminate this ambiguity by specifying the source regions from which temperatures are to be interpolated. The source region refers to the heat transfer analysis and is specified by an element set. The target region refers to the current analysis and is specified by a node set.

Input File Usage

INITIAL CONDITIONS, TYPE=TEMPERATURE, INTERPOLATE, 
FILE=file, STEP=step, INC=inc, DRIVING ELSETS

Abaqus/CAE Usage

You cannot specify the regions where temperatures are to be interpolated in Abaqus/CAE.

Interpolating Initial Temperatures for Meshes That Differ Only in Element Order from a User-Specified Results or Output Database File

If the only difference in the meshes is the element order (first-order elements in the heat transfer model and second-order elements in the stress/displacement model), in Abaqus/Standard you can indicate that midside node temperatures in second-order elements are to be interpolated from corner node temperatures read from the results or output database file of the previous heat transfer analysis using first-order elements. You must ensure that the corner node temperatures are not defined using a mixture of direct data input and reading from the results or output database file, since midside node temperatures that give unrealistic temperature fields may result. In practice, the capability for calculating midside node temperatures is most useful when temperatures generated by a heat transfer analysis are read from the results or output database file for the whole mesh during the stress analysis. Once the midside node capability is activated, the capability remains active for the rest of the analysis, including for any predefined temperature fields defined to change temperatures during the analysis. The general interpolation and midside node capabilities are mutually exclusive.

Input File Usage

INITIAL CONDITIONS, TYPE=TEMPERATURE, MIDSIDE, 
FILE=file, STEP=step, INC=inc

Abaqus/CAE Usage

Load module: Create Predefined Field: Step: Initial: choose Other for the Category and Temperature for the Types for Selected Step: select region: Distribution: From results or output database file, File name: file, Step: step, Increment: inc, Mesh compatibility: Compatible, and toggle on Interpolate midside nodes

Defining the Initial Configuration in a One-Step Inverse Analysis

In a one-step inverse analysis you must define the initial configuration by specifying initial conditions for the unfolded coordinates of all nodes in the part. One-step inverse analysis uses the Newton method, which requires an initial estimate of the solution as a starting point in the iterative algorithm. This starting point is defined by specifying unfold coordinate initial conditions.

Input File Usage

INITIAL CONDITIONS, TYPE=UNFOLD COORDINATE

Abaqus/CAE Usage

One-step inverse analysis is not supported in Abaqus/CAE.

Defining Initial Velocities for Specified Degrees of Freedom

You can define initial velocities for specified degrees of freedom. When initial velocities are given for dynamic analysis, they should be consistent with all of the constraints on the model, especially time-dependent boundary conditions. Abaqus ensures that they are consistent with boundary conditions and with multi-point and equation constraints but does not check for consistency with internal constraints such as incompressibility of the material. In case of conflict, boundary conditions take precedence over initial conditions.

Initial velocities must be defined in global directions, regardless of the use of local transformations (Transformed Coordinate Systems).

Input File Usage

INITIAL CONDITIONS, TYPE=VELOCITY

Abaqus/CAE Usage

Load module: Create Predefined Field: Step: Initial: choose Mechanical for the Category and Velocity for the Types for Selected Step

Defining Initial Volume Fractions for Eulerian Elements

You can define initial volume fractions to create material within Eulerian elements in Abaqus/Explicit. By default, these elements are filled with void. See Initial Conditions for a description of strategies for initializing Eulerian materials.

Input File Usage

INITIAL CONDITIONS, TYPE=VOLUME FRACTION

Abaqus/CAE Usage

Load module: Create Predefined Field: Step: Initial: choose Other for the Category and Material Assignment for the Types for Selected Step