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.
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.
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:
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).
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).
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:
Use the following option to specify the damage initiation measure for the Müschenborn
and Sonne forming limit diagram–based damage initiation criterion:
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).
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.
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:
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.
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.
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.
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.
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.
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.
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.
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.
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).
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:
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:
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).
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).
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, , 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.
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.
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.
Defining initial equivalent plastic strain and backstress tensor by importing field
data from an output database (.sim) file is not supported in Abaqus/CAE.
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.
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
Initial slurry concentration 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).
Initial ion concentration is not supported in Abaqus/CAE.
Defining Initial Species Concentration
In Abaqus/Standard you can define initial species concentration values at the cathode that is modeled using
coupled thermal-electrochemical elements in an analysis that uses solid electrolytes (see
Modeling Solid Electrolytes and Solid-State Batteries). "Species" refers to the chemical species that participates in the primary
electrochemical reactions in the battery.
Initial species 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).
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.
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.
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, , 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.
The initial effective stress/pore pressure conditions defined for an element are assumed to
act on the initial configuration of the element. If the initial effective stress/pore
pressure conditions are removed during the step, the element returns to a stress-free
configuration that is different from the initial one. Since displacements and total strain
output are measured relative to the initial configuration, the stress-free configuration
will have nonzero values for the displacement and total strain fields that will depend on
the initial conditions. While it is easy to verify the above behavior analytically in a
one-element problem subjected to an initial stress and pore pressure field, the situation in
a complex boundary value problem is determined by other factors that may make it difficult
to resolve analytically.
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.
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.
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.
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.
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).
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.
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.
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.
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.
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):
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):
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).
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 to a point b at ; and a translational velocity, . The initial velocity of node N at is then
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.
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).
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.
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.
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.
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.
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).
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. The initial effective stress conditions
defined for an element are assumed to act on the initial configuration of the element. If
the initial effective stress conditions are removed during the step, the element returns to
a stress-free configuration that is different from the initial one. Since displacements and
total strain output are measured relative to the initial configuration, the stress-free
configuration will have nonzero values for the displacement and total strain fields that
will depend on the initial conditions. While it is easy to verify the above behavior
analytically in a one-element problem subjected to an initial stress field, the situation in
a complex boundary value problem is determined by other factors that may make it difficult
to resolve analytically.
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.
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.
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.
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.
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 might 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 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 might 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.
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.
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.
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.
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.
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.
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).
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.
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 might 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.
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.
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).
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.