Products: ABAQUS/Standard ABAQUS/Explicit ABAQUS/CAE
Initial conditions are specified for particular nodes or elements, as appropriate. The data can be provided directly; in an external input file; or, in some cases, by a user subroutine or by the results or output database file from a previous ABAQUS analysis.
If initial conditions are not specified, all initial conditions are zero except relative density in the porous metal plasticity model, which will have the value 1.0.
Various types of initial conditions can be specified, depending on the analysis to be performed. Each type of initial condition is explained below, in alphabetical order.
In ABAQUS/Explicit you can define initial acoustic static pressure values at the acoustic nodes. These values should correspond to static equilibrium and cannot be changed during the analysis. You can specify the initial acoustic static pressure at two reference locations in the model, and ABAQUS/Explicit interpolates these data linearly to the acoustic nodes in the specified node set. The linear interpolation is based upon the projected position of each node onto the line defined by the two reference nodes. If the value at only one reference location is given, the initial acoustic static pressure is assumed to be uniform. The initial acoustic static pressure is used only in the evaluation of the cavitation condition (see “Acoustic medium,” Section 12.3.1) when the acoustic medium is capable of undergoing cavitation.
| Input File Usage: | *INITIAL CONDITIONS, TYPE=ACOUSTIC STATIC PRESSURE |
| ABAQUS/CAE Usage: | Initial acoustic static pressure is not supported in ABAQUS/CAE. |
In ABAQUS/Standard you can define initial normalized concentration values for use with diffusion elements in mass diffusion analysis (see “Mass diffusion analysis,” Section 6.8.1).
| Input File Usage: | *INITIAL CONDITIONS, TYPE=CONCENTRATION |
| ABAQUS/CAE Usage: | Initial normalized concentration is not supported in ABAQUS/CAE. |
In ABAQUS/Standard you can define initially bonded or partially bonded contact surfaces. This type of initial condition is intended for use with the crack propagation capability (see “Crack propagation analysis,” Section 7.10.3). The surfaces specified have to be different; this type of initial condition cannot be used with self-contact.
If the crack propagation capability is not activated, the bonded portion of the surfaces will not separate. In this case defining initially bonded contact surfaces would have the same effect as defining tied contact, which generates a permanent bond between two surfaces during the entire analysis (“Defining tied contact in ABAQUS/Standard,” Section 21.2.5).
| Input File Usage: | *INITIAL CONDITIONS, TYPE=CONTACT |
| ABAQUS/CAE Usage: | Initially bonded surfaces are not supported in ABAQUS/CAE. |
You can define initial values of predefined field variables. The values can be changed during an analysis (see “Predefined fields,” Section 19.6.1).
You must specify the field variable number being defined, n. Any number of field variables can be used; each must be numbered consecutively (1, 2, 3, etc.). Repeat the initial conditions definition, with a different field variable number, to define initial conditions for multiple field variables. The default is n=1.
The definition of initial field variable values must be compatible with the section definition and with adjacent elements, as explained in “Predefined fields,” Section 19.6.1.
| Input File Usage: | *INITIAL CONDITIONS, TYPE=FIELD, VARIABLE=n |
| ABAQUS/CAE Usage: | Initial predefined field variables are not supported in ABAQUS/CAE. |
You can define initial values of predefined field variables from a particular step and increment of a results file from a previous ABAQUS analysis (see “Predefined fields,” Section 19.6.1). The previous analysis is most commonly an ABAQUS/Standard heat transfer analysis. The use of the .fil file extension is optional.
The part (.prt) file from the previous analysis is required to read the initial values of predefined field variables from the results file (“Defining an assembly,” Section 2.9.1). Both the previous model and the current model must be consistently defined in terms of an assembly of part instances.
| Input File Usage: | *INITIAL CONDITIONS, TYPE=FIELD, VARIABLE=n, FILE=file, STEP=step, INC=inc |
| ABAQUS/CAE Usage: | Initial predefined field variables are not supported in ABAQUS/CAE. |
You can prescribe initial pressure for hydrostatic fluid elements (see “Modeling fluid-filled cavities,” Section 7.12.1).
Do not use this type of initial condition to define initial conditions in porous media in ABAQUS/Standard; use initial pore fluid pressures instead (see below).
| Input File Usage: | *INITIAL CONDITIONS, TYPE=FLUID PRESSURE |
| ABAQUS/CAE Usage: | Initial fluid pressure is not supported in ABAQUS/CAE. |
You can prescribe initial equivalent plastic strain and, if relevant, the initial backstress tensor for elements that use one of the metal plasticity (“Inelastic behavior,” Section 11.1.1) or Drucker-Prager (“Extended Drucker-Prager models,” Section 11.3.1) material models. These initial quantities are intended for materials in a work hardened state; they can be defined directly or by user subroutine HARDINI. You can also prescribe initial values for the volumetric compacting plastic strain, 
, for elements that use the crushable foam material model with volumetric hardening (“Crushable foam plasticity models,” Section 11.3.5).
| Input File Usage: | *INITIAL CONDITIONS, TYPE=HARDENING |
| ABAQUS/CAE Usage: | Initial hardening conditions are not supported in ABAQUS/CAE. |
In ABAQUS/Standard the hardening parameters can also be defined for rebars within elements. Rebars are discussed in “Defining rebar as an element property,” Section 2.2.4.
| Input File Usage: | *INITIAL CONDITIONS, TYPE=HARDENING, REBAR |
| ABAQUS/CAE Usage: | Initial hardening conditions are not supported in ABAQUS/CAE. |
For complicated cases in ABAQUS/Standard user subroutine HARDINI can be used to define the initial work hardening (see “HARDINI,” Section 25.2.11). In this case ABAQUS/Standard will call the subroutine at the start of the analysis for each material point in the model. You can then define the initial conditions at each point as a function of coordinates, element number, etc.
| Input File Usage: | *INITIAL CONDITIONS, TYPE=HARDENING, USER |
| ABAQUS/CAE Usage: | User subroutine HARDINI is not supported in ABAQUS/CAE. |
In ABAQUS/Standard you can define the initial mass flow rate through forced convection heat transfer elements. You can specify a predefined mass flow rate field to vary the value of the mass flow rate within the analysis step (see “Uncoupled heat transfer analysis,” Section 6.5.2).
| Input File Usage: | *INITIAL CONDITIONS, TYPE=MASS FLOW RATE |
| ABAQUS/CAE Usage: | Initial mass flow rate is not supported in ABAQUS/CAE. |
In ABAQUS/Standard you can define the initial pore pressure, 
, for nodes in a coupled pore fluid diffusion/stress analysis (see “Coupled pore fluid diffusion and stress analysis,” Section 6.7.1). The initial pore pressure can be defined either directly as an elevation-dependent function or by user subroutine UPOREP.
When an elevation-dependent pore pressure is prescribed for a particular node set, the pore pressure in the vertical direction (assumed to be the 
-direction in three-dimensional and axisymmetric models and the 
-direction in two-dimensional models) is assumed to vary linearly with this vertical coordinate. You must give two pairs of pore pressure and elevation values to define the pore pressure distribution throughout the node set. Enter only the first pore pressure value (omit the second pore pressure value and the elevation values) to define a constant pore pressure distribution.
| Input File Usage: | *INITIAL CONDITIONS, TYPE=PORE PRESSURE |
| ABAQUS/CAE Usage: | Initial pore pressure is not supported in ABAQUS/CAE. |
For complicated cases initial pore pressure values can be defined by user subroutine UPOREP (see “UPOREP,” Section 25.2.35). In this case ABAQUS/Standard will make a call to subroutine UPOREP at the start of the analysis for all nodes in the model. You can define the initial pore pressure at each node as a function of coordinates, node number, etc.
| Input File Usage: | *INITIAL CONDITIONS, TYPE=PORE PRESSURE, USER |
| ABAQUS/CAE Usage: | User subroutine UPOREP is not supported in ABAQUS/CAE. |
In ABAQUS/Standard you can specify the initial pressure stress, 
, at the nodes in a mass diffusion analysis (see “Mass diffusion analysis,” Section 6.8.1).
| Input File Usage: | *INITIAL CONDITIONS, TYPE=PRESSURE STRESS |
| ABAQUS/CAE Usage: | Initial pressure stress is not supported in ABAQUS/CAE. |
You can define initial values of pressure stress as those values existing at a particular step and increment in the results file of a previous ABAQUS/Standard stress/displacement analysis (see “Predefined fields,” Section 19.6.1). The use of the .fil file extension is optional. The initial values of pressure stress cannot be read from the results file when the previous model or the current model is defined in terms of an assembly of part instances (“Defining an assembly,” Section 2.9.1).
| Input File Usage: | *INITIAL CONDITIONS, TYPE=PRESSURE STRESS, FILE=file, STEP=step, INC=inc |
| ABAQUS/CAE Usage: | Initial pressure stress is not supported in ABAQUS/CAE. |
In ABAQUS/Standard you can specify the initial values of the void ratio, 
, at the nodes of a porous medium (see “Coupled pore fluid diffusion and stress analysis,” Section 6.7.1). The initial void ratio can be defined either directly as an elevation-dependent function or by user subroutine VOIDRI.
When an elevation-dependent void ratio is prescribed for a particular node set, the void ratio in the vertical direction (assumed to be the -direction in three-dimensional and axisymmetric models and the -direction in two-dimensional models) is assumed to vary linearly with this vertical coordinate. You must provide two pairs of void ratio and elevation values to define the void ratio throughout the node set. Enter only the first void ratio value (omit the second void ratio value and the elevation values) to define a constant void ratio distribution.
| Input File Usage: | *INITIAL CONDITIONS, TYPE=RATIO |
| ABAQUS/CAE Usage: | Initial void ratio is not supported in ABAQUS/CAE. |
For complicated cases initial values of the void ratios can be defined by user subroutine VOIDRI (see “VOIDRI,” Section 25.2.45). In this case ABAQUS/Standard will make a call to subroutine VOIDRI at the start of the analysis for each material integration point in the model. You can then define the initial void ratio at each point as a function of coordinates, element number, etc.
| Input File Usage: | *INITIAL CONDITIONS, TYPE=RATIO, USER |
| ABAQUS/CAE Usage: | User subroutine VOIDRI is not supported in ABAQUS/CAE. |
You can specify the initial values of the relative density field for a porous metal plasticity material model (see “Porous metal plasticity,” Section 11.2.9) or equations of state (see “Equation of state,” Section 10.9.1).
| Input File Usage: | *INITIAL CONDITIONS, TYPE=RELATIVE DENSITY |
| ABAQUS/CAE Usage: | Initial relative density is not supported in ABAQUS/CAE. |
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 
at 
to a point 
at 
; and a translational velocity, 
. The initial velocity of node 
at 
is then
| Input File Usage: | *INITIAL CONDITIONS, TYPE=ROTATING VELOCITY |
| ABAQUS/CAE Usage: | Initial rotating velocity is not supported in ABAQUS/CAE. |
In ABAQUS/Standard you can define the initial saturation, 
, for elements in a coupled pore fluid diffusion/stress analysis (see “Coupled pore fluid diffusion and stress analysis,” Section 6.7.1).
| Input File Usage: | *INITIAL CONDITIONS, TYPE=SATURATION |
| ABAQUS/CAE Usage: | Initial saturation is not supported in ABAQUS/CAE. |
You can define initial values of solution-dependent state variables (see “User subroutines: overview,” Section 25.1.1). The initial values can be defined directly or, in ABAQUS/Standard, by user subroutine SDVINI. Values given directly will be applied uniformly over the element.
| Input File Usage: | *INITIAL CONDITIONS, TYPE=SOLUTION |
| ABAQUS/CAE Usage: | Initial solution-dependent variables are not supported in ABAQUS/CAE. |
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,” Section 2.2.4.
| Input File Usage: | *INITIAL CONDITIONS, TYPE=SOLUTION, REBAR |
| ABAQUS/CAE Usage: | Initial solution-dependent state variables are not supported in ABAQUS/CAE. |
For complicated cases in ABAQUS/Standard user subroutine SDVINI can be used to define the initial values of solution-dependent state variables (see “SDVINI,” Section 25.2.16). In this case ABAQUS/Standard will make a call to subroutine SDVINI at the start of the analysis for each material integration point in the model. You can then define all solution-dependent state variables at each point as functions of coordinates, element number, etc.
| Input File Usage: | *INITIAL CONDITIONS, TYPE=SOLUTION, USER |
| ABAQUS/CAE Usage: | User subroutine SDVINI is not supported in ABAQUS/CAE. |
In ABAQUS/Explicit you can specify the initial values of the specific energy for equations of state (see “Equation of state,” Section 10.9.1).
| Input File Usage: | *INITIAL CONDITIONS, TYPE=SPECIFIC ENERGY |
| ABAQUS/CAE Usage: | Initial specific energy is not supported in ABAQUS/CAE. |
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,” Section 18.11.1).
| Input File Usage: | Use one of the following options: |
*INITIAL CONDITIONS, TYPE=SPUD EMBEDMENT *INITIAL CONDITIONS, TYPE=SPUD PRELOAD |
| ABAQUS/CAE Usage: | Initial spud can embedment and preload are not supported in ABAQUS/CAE. |
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 will be applied uniformly over the element unless they are defined at each section point through the thickness in shell elements.
If a local coordinate system was defined (see “Orientations,” Section 2.2.5), 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,” Section 6.7.1, for a discussion of defining initial conditions in porous media.
If the section properties of beam elements or shell elements are defined by a general section, the initial stress values are applied as initial section forces and moments. In the case of beams initial conditions can be specified only for the axial force, the bending moments, and the twisting moment. In the case of shells initial conditions can be specified only for the membrane forces, the bending moments, and the twisting moment. In both shells and beams initial conditions cannot be prescribed for the transverse shear forces.
Initial stress fields cannot be defined for spring elements. See “Springs,” Section 18.1.1, for a discussion of defining initial forces in spring elements.
Initial values of stress can also be defined for rebars within elements (see “Defining rebar as an element property,” Section 2.2.4).
| Input File Usage: | *INITIAL CONDITIONS, TYPE=STRESS, REBAR |
| ABAQUS/CAE Usage: | Initial stress is not supported in ABAQUS/CAE. |
Initial values of stress can be defined at each section point through the thickness of shell elements.
| Input File Usage: | *INITIAL CONDITIONS, TYPE=STRESS, SECTION POINTS |
| ABAQUS/CAE Usage: | Initial stress is not supported in ABAQUS/CAE. |
For complicated cases (such as elbow elements) in ABAQUS/Standard the initial stress field can be defined by user subroutine SIGINI (see “SIGINI,” Section 25.2.17). In this case ABAQUS/Standard will make a call to subroutine SIGINI at the start of the analysis for each material calculation point in the model. You can then define all active stress components at each point as functions of coordinates, element number, etc.
| Input File Usage: | *INITIAL CONDITIONS, TYPE=STRESS, USER |
| ABAQUS/CAE Usage: | User subroutine SIGINI is not supported in ABAQUS/CAE. |
When initial stresses are given in ABAQUS/Standard (including prestressing in reinforced concrete or interpolation of an old solution onto a new mesh), the initial stress state may not be an exact equilibrium state for the finite element model. Therefore, an initial step should be included to allow ABAQUS/Standard to check for equilibrium and iterate, if necessary, to achieve equilibrium.
In a soils analysis (that is, for models containing elements that include pore fluid pressure as a variable) the geostatic stress field procedure (“Geostatic stress state,” Section 6.7.2) 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 will converge 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,” Section 6.2.2) 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 will attempt to find equilibrium in one increment. By default, ABAQUS/Standard ramps down the unbalanced stress 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 stresses is defined at each material point. These stresses are equal in magnitude to the initial stresses but are of opposite sign. The sum of the material point stresses and these artificial stresses creates zero internal forces at the beginning of the step.
The internal artificial stresses are ramped off linearly in time during the first step. Thus, at the end of the step the artificial stresses have been removed completely and the remaining stresses in the material will be the stress state in equilibrium.
If the equilibrating step does not converge, it indicates that the initial stress state is so far from equilibrium with the applied loads that significantly large deformations would be generated. This is generally not the intention of an initial stress state; therefore, it suggests that you should recheck the specified initial stresses and loads.
| Input File Usage: | Use one of the following options to specify how the unbalanced stress should be resolved: |
*INITIAL CONDITIONS, TYPE=STRESS, UNBALANCED STRESS=RAMP (default) *INITIAL CONDITIONS, TYPE=STRESS, UNBALANCED STRESS=STEP |
| ABAQUS/CAE Usage: | Initial stress is not supported in ABAQUS/CAE. |
In the current release ABAQUS/Explicit does not include initial stresses when calculating the initial accelerations. This is not a problem if the initial stress field is in static equilibrium with the initial external forces. In other cases this may introduce some noise in the solution. If this is a concern, it can be avoided by introducing an initial short step in which all degrees of freedom are fixed with boundary conditions. All initial loads should be included in that step. Then, 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 -direction in three-dimensional and axisymmetric models and the -direction in two-dimensional models) is assumed to vary (piecewise) linearly with this vertical coordinate.
For the vertical stress component, you must give two pairs of stress and elevation values to define the stress throughout the element set. For material points lying between the two elevations given, ABAQUS will use linear interpolation to determine the initial stress; for points lying outside the two elevations given, ABAQUS will use linear extrapolation. In addition, horizontal (lateral) stress components are given by entering one or two “coefficients of lateral stress,” which define the lateral direct stress components as the vertical stress at the point multiplied by the value of the coefficient. In axisymmetric cases only one value of the coefficient of lateral stress is used and, therefore, only one value need be entered.
Geostatic initial stresses are for use with continuum elements only. In ABAQUS/Standard elevation-dependent initial stresses should be specified for beams and shells in user subroutine SIGINI, as explained earlier. In ABAQUS/Explicit elevation-dependent initial stresses cannot be specified for beams and shells.
The geostatic stress state specified initially should be in equilibrium with the applied loads (such as gravity) and boundary conditions. An initial step should be included to allow ABAQUS to check for equilibrium after this interpolation has been done; see the discussion above on establishing equilibrium when an initial stress field is applied.
| Input File Usage: | *INITIAL CONDITIONS, TYPE=STRESS, GEOSTATIC |
| ABAQUS/CAE Usage: | Initial stress is not supported in ABAQUS/CAE. |
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,” Section 19.6.1).
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,” Section 19.6.1.
| Input File Usage: | *INITIAL CONDITIONS, TYPE=TEMPERATURE |
| ABAQUS/CAE Usage: | Load module: Create Field: Step: Initial: choose Other for the Category and Temperature for the Types for Selected Step |
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,” Section 19.6.1).
The part (.prt) file from the previous analysis is required to read initial temperatures from the results or output database file (“Defining an assembly,” Section 2.9.1). Both the previous model and the current model must be consistently defined in terms of an assembly of part instances.
The file extension is optional; however, if both results and output database files exist, the results file will be used.
| Input File Usage: | *INITIAL CONDITIONS, TYPE=TEMPERATURE, FILE=file, STEP=step, INC=inc |
| ABAQUS/CAE Usage: | Load module: Create 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 |
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. Only temperatures from an output database file can be used for the interpolation; ABAQUS will look for the .odb extension automatically.
| Input File Usage: | *INITIAL CONDITIONS, TYPE=TEMPERATURE, INTERPOLATE, FILE=file, STEP=step, INC=inc |
| ABAQUS/CAE Usage: | Load module: Create 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 |
If the only difference in the meshes is the element order (first-order elements in the heat transfer model and second-order elements in the stress/displacement model), in ABAQUS/Standard you can indicate that midside node temperatures in second-order elements are to be interpolated from corner node temperatures read from the results or output database file of the previous heat transfer analysis using first-order elements. You must ensure that the corner node temperatures are not defined using a mixture of direct data input and reading from the results or output database file, since midside node temperatures that give unrealistic temperature fields may result. In practice, the capability for calculating midside node temperatures is most useful when temperatures generated by a heat transfer analysis are read from the results or output database file for the whole mesh during the stress analysis. Once the midside node capability is activated, the capability will remain active for the rest of the analysis, including for any predefined temperature fields defined to change temperatures during the analysis. The general interpolation and midside node capabilities are mutually exclusive.
| Input File Usage: | *INITIAL CONDITIONS, TYPE=TEMPERATURE, MIDSIDE, FILE=file, STEP=step, INC=inc |
| ABAQUS/CAE Usage: | Load module: Create 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 |
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 will ensure that they are consistent with boundary conditions and with multi-point and equation constraints but will 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,” Section 2.1.5).
| Input File Usage: | *INITIAL CONDITIONS, TYPE=VELOCITY |
| ABAQUS/CAE Usage: | Load module: Create Field: Step: Initial: choose Mechanical for the Category and Velocity for the Types for Selected Step |
The input data for an initial conditions definition can be contained in a separate file. See “Input syntax rules,” Section 1.2.1, for the syntax of such file names.
| Input File Usage: | *INITIAL CONDITIONS, INPUT=file_name |
| ABAQUS/CAE Usage: | Initial conditions cannot be read from a separate file in ABAQUS/CAE. |
ABAQUS does not ensure that initial conditions are consistent with multi-point or equation constraints for nodal quantities other than velocity (see “General multi-point constraints,” Section 20.2.2, and “Linear constraint equations,” Section 20.2.1). Initial conditions on nodal quantities such as temperature in heat transfer analysis, pore pressure in soils analysis, or acoustic pressure in acoustic analysis must be prescribed to be consistent with any multi-point constraint or equation constraint governing these quantities.