ProductsAbaqus/StandardAbaqus/ExplicitAbaqus/Aqua
TypeModel data LevelModel
Required parameters
-
TYPE
-
Set
TYPE=ACOUSTIC STATIC PRESSURE
to define initial static pressure values at acoustic nodes for use in evaluating the
cavitation status of the acoustic element nodes in Abaqus/Explicit.
Set
TYPE=ACTIVATION
to define the initial volume fraction for elements used in progressive element
activation in an Abaqus/Standard analysis. The value of the volume fraction
must be equal to zero or one, which means that an element at the beginning of an
analysis must be either inactive or fully active.
Set
TYPE=CONCENTRATION
to give initial normalized concentrations for a mass diffusion analysis in Abaqus/Standard.
Set
TYPE=CONTACT
to specify initial bonded contact conditions on part of the secondary surface
identified by a node set in an Abaqus/Standard analysis.
Set
TYPE=DAMAGE INITIATION
to specify initial values of the damage initiation measure. The
CRITERION parameter must also be
used to specify the damage initiation criterion for which initial conditions are being
specified. The REBAR and
SECTION POINTS parameters can be
used with this parameter when
CRITERION=DUCTILE
or
CRITERION=SHEAR.
Set
TYPE=ENRICHMENT
to specify initial location of an enriched feature, such as a crack, in an Abaqus/Standard analysis. 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 describes the crack surface while the second is used to construct an orthogonal
surface so that the intersection of the two surfaces gives the crack front. The first
signed distance function is assigned only to nodes of elements intersected by the
crack while the second signed distance function is assigned only to nodes of elements
containing the crack tips. No explicit representation of the crack is needed as the
crack is entirely described by the nodal data.
Set
TYPE=ESDV
to give initial values for element solution-dependent variables in an Abaqus/Standard analysis.
Set
TYPE=FIELD
to specify initial values of field variables. The
VARIABLE parameter can be used with
this parameter to define the field variable number. The
STEP and
INC parameters can be used in
conjunction with the FILE parameter
to define initial values of field variables from a results (.fil)
or output database (.odb) file. The
STEP and
INC parameters can also be used in
conjunction with the FILE and
OUTPUT VARIABLE parameters to define
initial values of field variables based on scalar nodal output variables read from an
output database file.
Set
TYPE=FLUID ELECTRIC POTENTIAL
to give initial electric potential in the electrolyte for a coupled
thermal-electrochemical analysis.
Set
TYPE=FLUID PRESSURE
to give initial pressures for hydrostatic fluid filled cavities.
Set
TYPE=HARDENING
to prescribe initial equivalent plastic strain and, if relevant, the initial
backstress tensor or to prescribe initial volumetric compacting plastic strain for the
crushable foam model. The REBAR and,
in Abaqus/Standard, SECTION POINTS and
USER parameters can be used with
this parameter. If the USER
parameter is used, the initial conditions on equivalent plastic strain and, if
relevant, the backstress tensor must be specified via user subroutine HARDINI for each section point
and for each rebar. Consequently, in this case the
REBAR and
SECTION POINTS parameters do not
have any effect and are ignored. If the
USER parameter is omitted, Abaqus/Standard assumes that the initial conditions are defined on the data lines.
Set
TYPE=INITIAL GAP
to identify the elements within which tangential fluid flow exists initially and to
set the material initial damage variables at the integration points.
Set
TYPE=ION CONCENTRATION
to give initial concentrations in the electrolyte for a coupled
thermal-electrochemical analysis.
Set
TYPE=MASS FLOW RATE
to specify initial values of mass flow rates in Abaqus/Standard heat transfer analyses involving forced convection modeled with the forced
convection/diffusion heat transfer elements.
Set
TYPE=NODE REF COORDINATE
to define the reference mesh (initial metric) for membrane elements in Abaqus/Explicit using node numbers and the coordinates of each node. If a reference mesh is
specified for an element, no initial stress or strain can be specified for the same
element. The initial stress and strain are computed automatically to account for
deformation from the reference to the initial configuration.
Set
TYPE=PLASTIC STRAIN
to specify initial plastic strains. The
SECTION POINTS and
REBAR parameters can be used with
this parameter. It is assumed that the plastic strain components are defined on each
data line in the order given for the element type, as defined in About the Element Library.
Set
TYPE=PORE PRESSURE
to give initial pore fluid pressures for a coupled pore fluid diffusion/stress
analysis in Abaqus/Standard. The STEP and
INC parameters can also be used with
the FILE parameter to define initial
values of pore fluid pressures based on scalar nodal output variables read from an
output database (.odb) file.
Set
TYPE=POROSITY
to give initial porosity values for materials defined with the EOS COMPACTION option in Abaqus/Explicit or materials defined using the poroelastic acoustic models.
Set
TYPE=PRESSURE STRESS
to give initial pressure stresses for a mass diffusion analysis in Abaqus/Standard. The STEP and
INC parameters can be used in
conjunction with the FILE parameter
to define initial values of pressure stress from the results
(.fil) file of a previous Abaqus/Standard stress/displacement analysis.
Set
TYPE=RATIO
to give initial void ratio values for a coupled pore fluid diffusion/stress analysis
in Abaqus/Standard. The STEP and
INC parameters can be used in
conjunction with the FILE parameter
to define initial values of void ratio from the output database
(.odb) file of a previous Abaqus/Standard soil analysis. The USER parameter
can be used with this parameter to define initial void ratio values in user subroutine
VOIDRI.
Set
TYPE=REF COORDINATE
to define the reference mesh (initial metric) for membrane elements in Abaqus/Explicit using the element number and the coordinates of all of the nodes associated with
the element. If a reference mesh is specified for an element, no initial stress or
strain can be specified for the same element. The initial stress and strain are
computed automatically to account for deformation from the reference to the initial
configuration.
Set
TYPE=RELATIVE DENSITY
to give initial relative density values for materials defined with the POROUS METAL PLASTICITY
option.
Set
TYPE=ROTATING VELOCITY
to prescribe initial velocities in terms of an angular velocity and a global
translational velocity.
Set
TYPE=SATURATION
to give initial saturation values for the analysis of flow through a porous medium in
Abaqus/Standard. If no initial saturation values are given on this option, the default is fully
saturated conditions (saturation of 1.0). For partial saturation the initial
saturation and the pore fluid pressure must be consistent in the sense that the pore
fluid pressure must lie within the range of absorption and exsorption values for the
initial saturation value. If this is not the case, Abaqus/Standard will adjust the saturation value as needed to satisfy this requirement.
Set
TYPE=SOLID ELECTRIC POTENTIAL
to give initial electric potential in the solid phase for a coupled
thermal-electrochemical analysis.
Set
TYPE=SOLUTION
to give initial values of solution-dependent state variables. The
REBAR and
USER parameters can be used with
this parameter. If
TYPE=SOLUTION
is used without the USER parameter,
element average quantities of the solution-dependent state variables must be defined
on each data line.
Set
TYPE=SPECIFIC ENERGY
to give initial specific energy values for materials defined with the EOS option in Abaqus/Explicit.
Set
TYPE=SPUD EMBEDMENT
to give the initial embedment for a spud can in an Abaqus/Aqua analysis.
Set
TYPE=SPUD PRELOAD
to give the initial preload value for a spud can in an Abaqus/Aqua analysis.
Set
TYPE=STRESS
to give initial stresses. (These stresses are effective stresses when the analysis
includes pore fluid flow.) The
GEOSTATIC; the
REBAR; the
SECTION POINTS; and, in Abaqus/Standard, the USER parameters can be used
with this parameter. If
TYPE=STRESS
is used without the USER parameter,
it is assumed that the stress components are defined on each data line in the order
given for the element type, as defined in About the Element Library. The
STEP and
INC parameters can also be used with
the FILE parameter to define initial
stress values based on stress output variables read from an output database
(.odb or .sim) file.
Set
TYPE=TEMPERATURE
to give initial temperatures. The
STEP and
INC parameters can be used in
conjunction with the FILE parameter
to define initial temperatures from the results (.fil) or output
database (.odb) file of a previous Abaqus/Standard heat transfer analysis.
Set
TYPE=UNFOLD COORDINATE
to give initial coordinates in an Abaqus/Standard one-step inverse analysis.
Set
TYPE=VELOCITY
to prescribe initial velocities. Initial velocities should be defined in the global
directions, regardless of the use of the TRANSFORM option.
Set
TYPE=VOLUME FRACTION
to define the initial material content of Eulerian elements in an Abaqus/Explicit analysis.
Optional parameters
-
ABSOLUTE EXTERIOR TOLERANCE
-
This parameter is relevant only for use with the
INTERPOLATE parameter. Set this
parameter equal to the absolute value (given in the units used in the model) by which
nodes of the current model may lie outside the region of the model in the output
database specified by the FILE
parameter. If this parameter is not used or has a value of 0.0, the
EXTERIOR TOLERANCE parameter will
apply.
-
CORRESPONDING CONTACT STRESS
-
This parameter applies only to Abaqus/Standard analyses.
This parameter is used only with
TYPE=STRESS.
Set
CORRESPONDING CONTACT STRESS=YES
(default) to activate initial contact stress calculations.
Set
CORRESPONDING CONTACT STRESS=NO
to turn off initial contact stress calculations.
This parameter is a global setting and affects all contact definitions in a model.
Also, if the INITIAL CONDITIONS options is
repeated multiple times in an input file, the
CORRESPONDING CONTACT STRESS
parameter setting on the last occurrence prevails.
-
CRITERION
-
Set
CRITERION=DUCTILE
to provide the damage initiation measure for the ductile damage initiation criterion.
Set
CRITERION=MSFLD
to provide the damage initiation measure for the Müschenborn and Sonne forming limit
diagram based damage initiation criterion.
Set
CRITERION=SHEAR
to provide the damage initiation measure for the shear damage initiation criterion.
-
DEFINITION
-
Set
DEFINITION=COORDINATES
(default) to define the axis of rotation for
TYPE=ROTATING VELOCITY
by giving the coordinates of the two points, a and
b.
Set
DEFINITION=NODES
to define the axis of rotation for
TYPE=ROTATING VELOCITY
by giving global node numbers for points a and
b.
-
DRIVING ELSETS
-
This parameter is relevant only for use with the
INTERPOLATE parameter. Include this
parameter to indicate that the field (temperature, void ratio, and pore pressure only)
is interpolated from a user-specified element set from the previous analysis to a
user-specified node set in the current job. This parameter is used to eliminate
mapping ambiguity in cases where element regions in the previous analysis are close or
touching. To accomplish part instance to part instance mapping, define your element
and node sets to correspond to the respective instances in the previous and current
analysis.
-
EXTERIOR TOLERANCE
-
This parameter is relevant only for use with the
INTERPOLATE parameter. Set this
parameter equal to the fraction of the average element size by which nodes of the
current model may lie outside the region of the elements of the model in the output
database specified by the FILE
parameter. The default value is 0.05.
If both tolerance parameters are specified, Abaqus uses the tighter tolerance.
-
FILE
-
Set this parameter equal to the name of the results (.fil) file
or output database (.odb) file from which initial field variable,
void ratio, pore pressure, or pressure stress data are to be read.
Set this parameter equal to the name of output database (.odb or
.sim) file from which initial stress is to be read.
This parameter must be used in conjunction with the
STEP and
INC parameters. For more
information, see File Extension Definitions.
This parameter is ignored if the initial field values are specifed with the
EXTERNAL FIELD option.
-
FULL TENSOR
-
Include this parameter if the kinematic shift tensor (backstress) components are
specified using the full tensor format, regardless of the element type to which the
initial conditions are applied.
This parameter can be used only in conjunction with the parameter
TYPE=HARDENING.
It cannot be used if any of the parameters
REBAR,
SECTION POINTS, or
USER has been used.
-
GEOSTATIC
-
This parameter is used only with
TYPE=STRESS
to specify that a geostatic stress state, in which stresses vary with elevation only,
is being defined.
-
INC
-
This parameter is used only with the
FILE parameter. If this parameter is
omitted, the initial conditions will be read from the last increment of the step
specified on the STEP parameter or
from the last step if the STEP
parameter is omitted.
The parameter specifies the increment in the results (.fil)
file of a previous Abaqus analysis from which prescribed fields of
TYPE=FIELD,
TYPE=PRESSURE STRESS,
or
TYPE=TEMPERATURE
are to be read. It can also specify the increment in the output database
(.odb) file of a previous Abaqus analysis from which prescribed fields of
TYPE=FIELD,
TYPE=PORE PRESSURE,
TYPE=RATIO,
or
TYPE=TEMPERATURE
are to be read. For
TYPE=STRESS,
this parameter specifies the increment in the output database
(.odb or .sim) file of a previous Abaqus analysis from which initial stress is to be read.
-
INPUT
-
Set this parameter equal to the name of the alternate input file containing the data
lines for this option. See Input Syntax Rules for the
syntax of such file names. If this parameter is omitted, it is assumed that the data
follow the keyword line.
-
INTERPOLATE
-
Include this parameter in conjunction with the
FILE,
STEP, and
INC parameters to indicate that the
nodal temperatures being read into the temperature field or the scalar nodal output
variable being read into a predefined field needs to be interpolated between
dissimilar meshes. This feature is used to read nodal values from an output database
(.odb) file generated during a previous Abaqus analysis.
For void ratio initialization from a previous output database file, this parameter is
automatically activated and the old void ratios from either the element integration
points or the element nodes are read and mapped onto the current nodes.
For temperature fields this parameter and the
MIDSIDE parameter are mutually
exclusive. For temperature fields if the initial analysis uses first-order elements
and the current mesh is the same but uses second-order elements, use the
MIDSIDE parameter instead. The
MIDSIDE parameter is not supported
for predefined fields; therefore, the
INTERPOLATE parameter is the only
option for initializing predefined fields using scalar nodal output values from a
dissimilar mesh.
-
MIDSIDE
-
This parameter applies only to Abaqus/Standard analyses.
Include this parameter in conjunction with the
FILE,
STEP, and
INC parameters to indicate that
midside node temperatures in second-order elements are to be interpolated from corner
node temperatures. This feature is used to read temperatures from a results
(.fil) or output database (.odb) file
generated during a heat transfer analysis using first-order elements. This parameter
and the INTERPOLATE parameter are
mutually exclusive.
-
NORMAL
-
This parameter applies only to Abaqus/Standard analyses.
This parameter can be used only with
TYPE=CONTACT
to specify that the nodes in the node set (or the contact pair, if a node set is not
defined) are bonded only in the normal (contact) direction and are allowed to move
freely in the tangential direction. If the nodes in the node set (or the contact pair)
are to be bonded in all directions, this parameter should be omitted.
-
NUMBER BACKSTRESSES
-
Set this parameter equal to the number of backstresses. This parameter can be used
only in conjunction with
TYPE=HARDENING.
The default number of backstresses is 1, and the maximum allowed is 10.
-
OUTPUT VARIABLE
-
This parameter is required when
TYPE=FIELD
and the FILE parameter references an
output database.
Set this parameter equal to the scalar nodal output variable that will be read from
an output database and used to initialize a specified predefined field. For a list of
scalar nodal output variables that can be used to initialize a predefined field, see
Predefined Fields.
-
REBAR
-
This parameter can be used with
TYPE=DAMAGE INITIATION,
TYPE=HARDENING,
TYPE=PLASTIC STRAIN,
TYPE=SOLUTION,
or
TYPE=STRESS.
When used with
TYPE=DAMAGE INITIATION,
it specifies the initial value of the damage initiation measure in the rebar.
When used with
TYPE=HARDENING,
it specifies that rebars are in a work hardened state, with initial equivalent plastic
strain and, possibly, initial backstress.
When used with
TYPE=PLASTIC STRAIN,
it specifies the initial plastic strain in the rebar.
When used with
TYPE=SOLUTION,
it specifies that rebars are being assigned initial solution-dependent state variable
values.
When used with
TYPE=STRESS,
it specifies that prestress in rebars is being defined. When performing an Abaqus/Standard analysis, some iteration will usually be needed in this case to establish a
self-equilibrating stress state in the rebar and concrete. The PRESTRESS HOLD option can be
useful for post-tensioning simulations (see Defining Rebar as an Element Property).
-
SECTION POINTS
-
This parameter is used only with
TYPE=DAMAGE INITIATION,
TYPE=HARDENING,
TYPE=PLASTIC STRAIN,
and
TYPE=STRESS
to specify damage initiation measures, hardening variables, plastic strains, and stresses at individual
section points through the thickness of a shell element. This parameter can be used
only when shell properties are defined using the SHELL SECTION option. It
cannot be used when properties are defined using the SHELL GENERAL SECTION option.
-
SECTION SPECIFICATION
-
This parameter is relevant only for
TYPE=TEMPERATURE
and
TYPE=FIELD.
Set
SECTION SPECIFICATION=UNIFORM
to specify uniform temperatures and field variables.
The INPUT and
VARIABLE parameters can be used with
this parameter.
-
STEP
-
This parameter is used only with the
FILE parameter. If this parameter is
omitted, the initial conditions will be read from the last step.
The parameter specifies the step in the results (.fil) file of a
previous Abaqus analysis from which prescribed fields of
TYPE=FIELD,
TYPE=PRESSURE STRESS,
or
TYPE=TEMPERATURE
are to be read. It can also specify the step in the output database
(.odb) file of a previous Abaqus analysis from which prescribed fields of
TYPE=FIELD,
TYPE=PORE PRESSURE,
TYPE=RATIO,
or
TYPE=TEMPERATURE
are to be read. For
TYPE=STRESS,
this parameter specifies the step in the output database (.odb or
.sim) file of a previous Abaqus analysis from which initial stress is to be read.
-
UNBALANCED STRESS
-
This parameter applies only to Abaqus/Standard analyses.
This parameter is used only with
TYPE=STRESS.
Set
UNBALANCED STRESS=RAMP
(default) if the unbalanced stress is to be resolved linearly over the step.
Set
UNBALANCED STRESS=STEP
if the unbalanced stress is to be resolved in the first increment.
If the INITIAL CONDITIONS option is
repeated multiple times in an input file, the
UNBALANCED STRESS parameter setting
on the last occurrence prevails.
-
USER
-
In Abaqus/Standard, this parameter can be used with
TYPE=HARDENING,
TYPE=PORE PRESSURE,
TYPE=RATIO,
TYPE=SOLUTION,
or
TYPE=STRESS.
When used with
TYPE=HARDENING,
it specifies that the initial conditions on equivalent plastic strain and, if
relevant, backstress tensor are to be given via user subroutine HARDINI.
When used with
TYPE=PORE PRESSURE,
it specifies that initial pore pressures are to be given via user subroutine UPOREP.
When used with
TYPE=RATIO,
it specifies that initial void ratios are to be given via user subroutine VOIDRI.
When used with
TYPE=SOLUTION,
it specifies that initial solution-dependent state variable fields are to be given via
user subroutine SDVINI.
When used with
TYPE=STRESS,
it specifies that stresses are to be given in user subroutine SIGINI.
In Abaqus/Explicit, this parameter can be used only with
TYPE=SOLUTION.
It specifies that initial solution-dependent state variable fields are to be given in
user subroutine VSDVINI.
-
VARIABLE
-
This parameter is used only with
TYPE=FIELD
when it is used to define the field variable number. The default is
VARIABLE=1.
Any number of separate field variables can be used: each must be numbered
consecutively (1, 2, 3, etc.)
No data lines are required if the initial conditions are read from a file (the
FILE parameter is included) unless the
DRIVING ELSETS parameter is used; if the
initial conditions are defined with the
EXTERNAL FIELD option; or if the initial
conditions are defined in a user subroutine (the
USER parameter is
included)
Data line for
TYPE=ACOUSTIC STATIC PRESSURE
- First (and only) line
-
Node set or node number.
Hydrostatic pressure at the first reference point.
X-coordinate of the first reference point.
Y-coordinate of the first reference point.
Z-coordinate of the first reference point.
Hydrostatic pressure at the second reference point.
X-coordinate of the second reference point.
Y-coordinate of the second reference point.
Z-coordinate of the second reference point.
Data lines for
TYPE=ACTIVATION
- First line
-
Element set or element number.
Initial volume fraction of material in the element.
Repeat this data line as often as necessary to define the initial
volume fraction of material in various elements or element sets.
Data lines for
TYPE=CONCENTRATION
- First line
-
Node set or node number.
Initial normalized concentration value at the node.
Repeat this data line as often as necessary to define the initial
normalized concentration at various nodes or node sets.
Data lines for
TYPE=CONTACT
- First line
-
Secondary surface name.
Main surface name.
Name of the node set associated with the secondary surface.
Repeat this data line as often as necessary to define partially
bonded surfaces.
Data lines for
TYPE=DAMAGE INITIATION,
CRITERION=DUCTILE
or
CRITERION=SHEAR
if the REBAR and
SECTION POINTS parameters are
omitted
- First line
-
Element number or element set label.
Damage initiation measure for either the ductile or the shear damage
initiation criterion,
or
.
Repeat this data line as often as necessary to define initial damage
initiation measures in various elements or element sets.
Data lines for
TYPE=DAMAGE INITIATION,
CRITERION=DUCTILE
or
CRITERION=SHEAR
with the REBAR parameter
included
- First line
-
Element number or element set label.
Rebar name. If this field is left blank, the initial conditions will be
applied to all rebars in the model.
Damage initiation measure for either the ductile or the shear damage
initiation criterion,
or
.
Repeat this data line as often as necessary to define initial damage
initiation measures for rebars in various elements or element
sets.
Data lines for
TYPE=DAMAGE INITIATION,
CRITERION=DUCTILE
or
CRITERION=SHEAR
with the SECTION POINTS parameter
included
- First line
-
Element number or element set label.
Section point number.
Damage initiation measure for either the ductile or the shear damage
initiation criterion,
or
.
Repeat this data line as often as necessary to define initial damage
initiation measures in various elements or element sets. The initial damage initiation
measures must be defined at all section points within an element.
Data lines for
TYPE=DAMAGE INITIATION,
CRITERION=MSFLD
- First line
-
Element number or element set label.
Damage initiation measure for the Müschenborn and Sonne forming limit
diagram based damage initiation criterion,
.
Ratio of the principal strain rates,
.
Repeat this data line as often as necessary to define initial damage
initiation measures in various elements or element sets.
Data lines for
TYPE=ENRICHMENT
- First line
-
Element number or element set label.
Relative position of the node forming the element connectivity.
Name of the enriched feature specified on the ENRICHMENT option.
Value of first signed distance function.
Value of second signed distance function. Leave this entry blank if only
the first signed distance function is needed.
Repeat this data line as often as necessary to define initial signed
distance functions in various elements or element sets. The signed distance functions
must be defined at all nodes within an element.
Data lines for
TYPE=ESDV
- First line
-
Element number or element set label.
Value of first element solution-dependent variable.
Value of second element solution-dependent variable.
Etc., up to seven element solution-dependent variables.
- Subsequent lines (only needed if more than seven element solution-dependent
variables exist in the model)
-
Value of eighth element solution-dependent variable.
Etc., up to eight element solution-dependent variables per line.
The total number of variables that Abaqus expects to read for any element is based on the maximum number of element
solution-dependent variables for all the elements in the model. Therefore, it may be
necessary to leave blank data lines for some elements if any other element in the
model has more element solution-dependent variables. These trailing initial values
will be zero and will not be used in the analysis.
Repeat this set of data lines as often as necessary to define initial
values of element solution-dependent variables for various elements or element
sets.
Data lines for
TYPE=FIELD,
VARIABLE=n
- First line
-
Node set or node number.
Initial value of this field variable at the first temperature point. For
shells and beams several values (or a value and the field variable gradients
across the section) can be given at each node (see About Beam Modeling as
well as About Shell Elements). For
heat transfer shells the field variables at each temperature point through the
shell thickness must be specified. The number of values depends on the (maximum)
number of points specified on the data lines associated with the SHELL SECTION options.
Initial value of this field variable at the second temperature point.
Etc., up to seven values.
- Subsequent lines (only needed if initial values must be specified at more
than seven temperature points at any node)
-
Eighth initial value of this field variable at this temperature point.
Etc., up to eight initial values per line.
The total number of field variables that Abaqus expects to read for any node is based on the maximum number of field variable
values for all the nodes in the model. Therefore, it may be necessary to leave blank
data lines for some nodes if any other node in the model has more than seven field
variable points. These trailing initial values will be zero and will not be used in
the analysis.
Repeat this set of data lines as often as necessary to define initial
temperatures at various nodes or node sets.
Data lines for
TYPE=FIELD,
SECTION SPECIFICATION=UNIFORM
- First line
-
Node set, node number, or blank.
Uniform field variable value.
Repeat this data line as often as necessary to define uniform field
variables at various nodes and node sets. If you omit both node numbers and node sets
(that is, enter a blank space), the specified uniform field variable is applied to all
nodes in the model.
Data lines for
TYPE=FLUID ELECTRIC POTENTIAL
- First line
-
Node set or node number.
Initial value of electric potential in the electrolyte at the node.
Repeat this data line as often as necessary to define the initial
electric potential in the electrolyte at various nodes or node
sets.
Data lines for
TYPE=FLUID PRESSURE
- First line
-
Node set or node number of fluid cavity reference node.
Fluid pressure.
Repeat this data line as often as necessary to define initial fluid
pressure for various fluid-filled cavities.
Data lines to prescribe initial equivalent plastic strain or backstresses using
TYPE=HARDENING
if the REBAR,
SECTION POINTS, and
USER parameters are
omitted
- First line
-
Element number or element set label.
Initial equivalent plastic strain,
.
First value of the initial first backstress,
.
Second value of the initial first backstress,
.
Etc., up to six backstress components.
- Subsequent lines (only needed if the
NUMBER BACKSTRESSES parameter has a
value greater than one)
-
First value of the initial second backstress,
.
Second value of the initial second backstress,
.
Etc., backstress components for each backstress must be specified on a
separate data line.
The backstress components are relevant only for the kinematic hardening models. Give
the backstress components as defined for this element type in About the Element Library. Values
given on the data lines are applied uniformly over the element. In any element for
which an ORIENTATION option applies,
backstresses must be given in the local system (Orientations).
Repeat this set of data lines as often as necessary to define the
hardening parameters for various elements or element sets.
Data lines to prescribe initial volumetric compacting plastic strain for the
crushable foam model using
TYPE=HARDENING
- First line
-
Element number or element set label.
Initial volumetric compacting plastic strain,
.
Repeat this data line as often as necessary to define the initial
volumetric compacting plastic strain for various elements or element
sets.
Data lines for
TYPE=HARDENING,
REBAR
- First line
-
Element number or element set label.
Rebar name. If this field is left blank, the initial conditions will be
applied to all rebars in the model.
Initial equivalent plastic strain,
.
Initial first backstress,
. (Only relevant for the kinematic hardening models.)
- Subsequent lines (only needed if the
NUMBER BACKSTRESSES parameter has a
value greater than one)
-
Initial second backstress,
. (Only relevant for the kinematic hardening models.)
Etc., backstress components for each backstress must be specified on a
separate data line.
Repeat this set of data lines as often as necessary to define the
hardening parameters for rebars in various elements or element
sets.
Data lines for
TYPE=HARDENING,
SECTION POINTS
- First line
-
Element number or element set label.
Section point number.
Initial equivalent plastic strain,
.
First value of the first initial backstress,
. (Only relevant for the kinematic hardening models.)
Second value of the first initial backstress,
.
Third value of the first initial backstress,
.
- Subsequent lines (only needed if the
NUMBER BACKSTRESSES parameter has a
value greater than one)
-
First value of the initial second backstress,
.
Second value of the initial second backstress,
.
Etc., backstress components for each backstress must be specified on a
separate data line.
The backstress components are relevant only for the kinematic hardening model. Give
the backstress components as defined for this element type in About the Element Library. In any
element for which an ORIENTATION option applies,
the backstress components must be given in the local system (Orientations).
Repeat this set of data lines as often as necessary to define the
hardening parameters in various elements or element sets. The hardening parameters
must be defined at all section points within an element.
Data lines for
TYPE=INITIAL GAP
- First line
-
Element number or element set label.
The material initial damage variable,
, at the first integration point.
The material initial damage variable,
, at the second integration point.
The material initial damage variable,
, at the third integration point.
The material initial damage variable,
, at the fourth integration point.
Repeat this data line as often as necessary to identify various
elements or element sets. Assigning the material initial damage variables at the
integration points is optional. If no initial damage variables are assigned, the
elements are considered fully damaged; that is,
. If you assign an initial damage variable to any of the integration
points and leave the other fields blank, a value of
is assigned to the integration points of the blank
fields.
Data lines for
TYPE=ION CONCENTRATION
- First line
-
Node set or node number.
Initial ion concentration value at the node.
Repeat this data line as often as necessary to define the initial ion
concentrations in the electrolyte at various nodes or node sets.
Data lines for
TYPE=MASS FLOW RATE
- First line
-
Node set or node number.
Initial mass flow rate per unit area in the
x-direction or total initial mass flow rate in the
cross-section for one-dimensional elements.
Initial mass flow rate per unit area in the
y-direction (not needed for nodes associated with
one-dimensional convective flow elements).
Initial mass flow rate per unit area in the
z-direction (not needed for nodes associated with
one-dimensional convective flow elements).
Repeat this data line as often as necessary to define mass flow rates
at various nodes or node sets.
Data lines for
TYPE=NODE REF COORDINATE
- First line
-
Node number.
X-coordinate of the node.
Y-coordinate of the node.
Z-coordinate of the node.
Repeat this data line as often as necessary to define the initial
coordinates of the mesh using nodal coordinates.
Data lines to prescribe initial plastic strains using
TYPE=PLASTIC STRAIN
if the REBAR and
SECTION POINTS parameters are
omitted
- First line
-
Element number or element set label.
Value of first plastic strain component,
.
Value of second plastic strain component,
.
Etc., up to six plastic strain components.
Give the plastic strain components as defined for this element type in About the Element Library. Values
given on the data lines are applied uniformly over the element. In any element for
which an ORIENTATION option applies,
the plastic strains must be given in the local system (Orientations).
Repeat this data line as often as necessary to define initial plastic
strains in various elements or element sets.
Data lines for
TYPE=PLASTIC STRAIN,
REBAR
- First line
-
Element number or element set label.
Rebar name. If this field is left blank, the initial conditions will be
applied to all rebars in the model.
Initial plastic strain value.
Repeat this data line as often as necessary to define the initial
plastic strain in the rebars of various elements or element sets.
Data lines for
TYPE=PLASTIC STRAIN,
SECTION POINTS
- First line
-
Element number or element set label.
Section point number.
Value of first plastic strain component,
.
Value of second plastic strain component,
.
Value of third plastic strain component,
.
Give the initial plastic strain components as defined for this element type in About the Element Library. In any
element for which an ORIENTATION option applies,
the plastic strain components must be given in the local system (Orientations).
Repeat this data line as often as necessary to define initial plastic
strains in various elements or element sets. Plastic strains must be defined at all
section points within an element.
Data lines for
TYPE=PORE PRESSURE
if the USER parameter is
omitted
- First line
-
Node set or node number.
First value of fluid pore pressure,
.
Vertical coordinate corresponding to the above value.
Second value of fluid pore pressure,
.
Vertical coordinate corresponding to the above value.
Omit the elevation values and the second pore pressure value to define a constant
pore pressure distribution.
Repeat this data line as often as necessary to define the fluid pore
pressure at various nodes or node sets.
Data lines for
TYPE=PORE PRESSURE,
FILE=file,
STEP=step,
INC=inc,
INTERPOLATE,
DRIVING ELSETS
- First line
-
Element set, node set.
Repeat this data line as often as necessary. The node set identified
on the data lines will be assigned values from the element set in the output database
(.odb) file. If a duplicate node is defined on a subsequent
data line, it will be removed from the subsequent void ratio mapping and printed out
to the data (.dat) file.
Data lines for
TYPE=POROSITY
- First line
-
Element number or element set label.
Initial porosity.
Repeat this data line as often as necessary to define initial
porosity in various elements or element sets.
Data lines for
TYPE=PRESSURE STRESS
- First line
-
Node set or node number.
Equivalent pressure stress, p.
Repeat this data line as often as necessary to define the pressure
stress at various nodes or node sets.
Data lines for
TYPE=RATIO
if the USER parameter is
omitted
- First line
-
Node set or node number.
First value of void ratio.
Vertical coordinate corresponding to the above value.
Second value of void ratio.
Vertical coordinate corresponding to the above value.
Omit the elevation values and the second void ratio value to define a constant void
ratio distribution.
Repeat this data line as often as necessary to define void ratios at
various nodes or node sets.
Data lines for
TYPE=RATIO,
FILE=file,
STEP=step,
INC=inc,
INTERPOLATE,
DRIVING ELSETS
- First line
-
Element set, node set.
Repeat this data line as often as necessary. The node set identified
on the data lines will be assigned values from the element set in the output database
(.odb) file. If a duplicate node is defined on a subsequent
data line, it will be removed from the subsequent void ratio mapping and printed out
to the data (.dat) file.
Data lines for
TYPE=REF COORDINATE
- First line
-
Element number.
X-coordinate of the first node.
Y-coordinate of the first node.
Z-coordinate of the first node.
X-coordinate of the second node.
Y-coordinate of the second node.
Z-coordinate of the second node.
- Second line
-
X-coordinate of the third node.
Y-coordinate of the third node.
Z-coordinate of the third node.
X-coordinate of the fourth node.
Y-coordinate of the fourth node.
Z-coordinate of the fourth node.
Repeat this pair of data lines as often as necessary to define the
reference mesh in various elements. The order of the nodal coordinates must be
consistent with the element connectivity.
Data lines for
TYPE=RELATIVE DENSITY
- First line
-
Node set or node number.
Initial relative density.
Repeat this data line as often as necessary to define initial
relative density at various nodes or node sets.
Data lines for
TYPE=ROTATING VELOCITY,
DEFINITION=COORDINATES
- First line
-
Node set or node number.
Angular velocity about the axis defined from point a
to point b, where the coordinates of a
and b are given below.
Global X-component of translational velocity.
Global Y-component of translational velocity.
Global Z-component of translational velocity.
- Second line
-
Global X-component of point a
on the axis of rotation.
Global Y-component of point a
on the axis of rotation.
Global Z-component of point a
on the axis of rotation.
Global X-component of point b
on the axis of rotation.
Global Y-component of point b
on the axis of rotation.
Global Z-component of point b
on the axis of rotation.
Repeat this pair of data lines as often as necessary to define the angular
and translational velocities at various nodes or node sets.
Data lines for
TYPE=ROTATING VELOCITY,
DEFINITION=NODES
- First line
-
Node set or node number.
Angular velocity about the axis defined from point a
to point b, where the coordinates of a
and b are given below.
Global X-component of translational velocity.
Global Y-component of translational velocity.
Global Z-component of translational velocity.
- Second line
-
Node number of the node at point a.
Node number of the node at point b.
Repeat this pair of data lines as often as necessary to define the
angular and translational velocities at various nodes or node
sets.
Data lines for
TYPE=SATURATION
- First line
-
Node set or node number.
Saturation value, s. Default is 1.0.
Repeat this data line as often as necessary to define saturation at
various nodes or node sets.
Data lines for
TYPE=SOLID ELECTRIC POTENTIAL
- First line
-
Node set or node number.
Initial value of electric potential in the solid phase at the node.
Repeat this data line as often as necessary to define the initial
electric potential in the solid phase at various nodes or node
sets.
Data lines for
TYPE=SOLUTION
if the USER and
REBAR parameters are
omitted
- First line
-
Element number or element set label.
Value of first solution-dependent state variable.
Value of second solution-dependent state variable.
Etc., up to seven solution-dependent state variables.
- Subsequent lines (only needed if more than seven solution-dependent state
variables exist in the model)
-
Value of eighth solution-dependent state variable.
Etc., up to eight solution-dependent state variables per line.
The total number of variables that Abaqus expects to read for any element is based on the maximum number of
solution-dependent state variables for all the elements in the model. Therefore, it
may be necessary to leave blank data lines for some elements if any other element in
the model has more solution-dependent state variables. These trailing initial values
will be zero and will not be used in the analysis. Values given on the data lines will
be applied uniformly over the element.
Repeat this set of data lines as often as necessary to define initial
values of solution-dependent state variables for various elements or element
sets.
Data lines for
TYPE=SOLUTION,
REBAR
- First line
-
Element number or element set label.
Rebar name. If this field is left blank, the solution-dependent state
variables are applied to all rebars in these elements.
Value of first solution-dependent state variable.
Value of second solution-dependent state variable.
Etc., up to six solution-dependent state variables.
- Subsequent lines (only needed if more than six solution-dependent state
variables exist in the model)
-
Value of seventh solution-dependent state variable.
Etc., up to eight solution-dependent state variables per line.
The total number of variables that Abaqus expects to read for any element is based on the maximum number of
solution-dependent state variables for all the elements in the model. Therefore, it
may be necessary to leave blank data lines for some elements if any other element in
the model has more solution-dependent state variables. These trailing initial values
will be zero and will not be used in the analysis. Values given on the data lines will
be applied uniformly over the element.
Repeat this set of data lines as often as necessary to define initial
values of solution-dependent state variables for various elements or element
sets.
Data lines for
TYPE=SPECIFIC ENERGY
- First line
-
Element number or element set label.
Initial specific energy.
Repeat this data line as often as necessary to define initial
specific energy in various elements or element sets.
Data lines for
TYPE=SPUD EMBEDMENT
- First line
-
Element set or element number.
Spud can embedment,
.
Repeat this data line as often as necessary to define initial
embedment for various elements or element sets.
Data lines for
TYPE=SPUD PRELOAD
- First line
-
Element set or element number.
Spud can preload,
.
Repeat this data line as often as necessary to define initial preload
for various elements or element sets.
Data lines for
TYPE=STRESS
if the GEOSTATIC,
REBAR,
SECTION POINTS, and
USER parameters are
omitted
- First line
-
Element number or element set label.
Value of first (effective) stress component, axial force when used with
the BEAM GENERAL SECTION or
FRAME SECTION options, or
direct membrane force per unit width in the local 1-direction when used with the
SHELL GENERAL SECTION
option.
Value of second stress component.
Etc., up to six stress components.
Give the stress components as defined for this element type in About the Element Library. Stress
values given on data lines are applied uniformly and equally over all integration
points of the element. In any element for which an ORIENTATION option applies,
the stresses must be given in the local system (Orientations).
Repeat this data line as often as necessary to define initial
stresses in various elements or element sets.
Data lines for
TYPE=STRESS,
GEOSTATIC
- First line
-
Element number or element set label.
First value of vertical component of (effective) stress.
Vertical coordinate corresponding to the above value.
Second value of vertical component of (effective) stress.
Vertical coordinate corresponding to the above value.
First coefficient of lateral stress. This coefficient defines the
x-direction stress components.
Second coefficient of lateral stress. This coefficient defines the
y-direction stress component in three-dimensional cases and
the thickness or hoop direction component in plane or axisymmetric cases. If this
value is omitted, it is assumed to be the same as the first lateral stress
coefficient given in the previous field.
Repeat this data line as often as necessary to define an initial
geostatic stress state in various elements or element sets.
Data lines for
TYPE=STRESS,
REBAR
- First line
-
Element number or element set label.
Rebar name. If this field is left blank, the stress is applied to all
rebars in these elements.
Prestress value.
Repeat this data line as often as necessary to define initial stress
in the rebars of various elements or element sets.
Data lines for
TYPE=STRESS,
SECTION POINTS
- First line
-
Element number or element set label.
Section point number.
Value of first stress component.
Value of second stress component.
Etc., up to three stress components.
Give the stress components as defined for this element type in About the Element Library. Stress
values given on data lines are applied uniformly over the element. In any element for
which an ORIENTATION option applies,
the stresses must be given in the local system (Orientations).
Repeat this data line as often as necessary to define initial
stresses in various elements or element sets. Stresses must be defined at all section
points within an element.
Data lines for
TYPE=TEMPERATURE
- First line
-
Node set or node number.
First initial temperature value at the node or node set. For shells and
beams several values (or a value and the temperature gradients across the section)
can be given at each node (see Using a Beam Section Integrated during the Analysis to Define the Section Behavior, Using a General Beam Section to Define the Section Behavior, Using a Shell Section Integrated during the Analysis to Define the Section Behavior, and
Using a General Shell Section to Define the Section Behavior). For
heat transfer shells the temperature at each point through the shell thickness
must be specified. The number of values depends on the (maximum) number of points
specified on the data lines associated with the SHELL SECTION options.
Second initial temperature value at the node or node set.
Etc., up to seven initial temperature values at this node or node set.
- Subsequent lines (only needed if there are more than seven temperature
values at any node)
-
Eighth initial temperature value at this node or node set.
Etc., up to eight initial temperature values per line.
If more than seven temperature values are needed at any node, continue on the next
line. The total number of temperatures that Abaqus expects to read for any node is based on the maximum number of temperature values
of all the nodes in the model. Therefore, it may be necessary to leave blank data
lines for some nodes if any other node in the model has more than seven temperature
points. These trailing initial values will be zero and will not be used in the
analysis.
Repeat this data line (or set of lines) as often as necessary to
define initial temperatures at various nodes or node sets.
Data lines for
TYPE=TEMPERATURE,
FILE=file,
STEP=step,
INC=inc,
INTERPOLATE,
DRIVING ELSETS
- First line
-
Element set, node set.
Repeat this data line as often as necessary. The node set identified
on the data lines will be assigned values from the element set in the output database
(.odb) file. If a duplicate node is defined on a subsequent
data line, it will be removed from the subsequent temperature mapping and printed out
to the data (.dat) file.
Data lines for
TYPE=TEMPERATURE,
SECTION SPECIFICATION=UNIFORM
- First line
-
Node set, node number, or blank.
Uniform temperature value.
Repeat this data line as often as necessary to define uniform
temperatures at various nodes and node sets. If you omit both node numbers and node
sets (that is, enter a blank space), the specified uniform temperature is applied to
all nodes in the model.
Data lines for
TYPE=UNFOLD COORDINATE
- First line
-
Node number.
X-coordinate of the first node.
Y-coordinate of the first node.
Z-coordinate of the first node.
Repeat this data line as often as necessary to define the initial
coordinates at various nodes.
Data lines for
TYPE=VELOCITY
- First line
-
Node set or node number.
Degree of freedom.
Value of initial velocity.
Repeat this data line as often as necessary to define the initial
velocity at various nodes or node sets.
Data lines for
TYPE=VOLUME FRACTION
- First line
-
Eulerian element number or element set label.
Name of the material instance as defined in the EULERIAN SECTION.
Initial volume fraction, EVF, for this
material (0.0 < EVF ≤ 1.0).
EVF=0.0 indicates that none of this material is
present in the element, while EVF=1.0 indicates
that the element is completely full of this material.
Repeat this data line as often as necessary to define the initial
geometry of all Eulerian material instances. An element may appear in more than one
data line if it initially contains more than one material. Elements are filled
incrementally by reading the data lines in the input file from bottom to top; once the
volume fraction for an element reaches one, additional volume fractions assigned to
that element are ignored. If the final volume fraction for an element is less than
one, the remainder of that element is filled with void; similarly, uninitialized
elements are filled with void.
|