Initial Conditions

You can specify initial conditions as follows:

• Directly in an input file.
• In an alternate input file (see Reading the Input Data from an External File).
• In a user subroutine.
• From the results or output database file of a previous Abaqus analysis. For more details on reading from output databases in the .odb or .sim file format, see Importing Data from an Output Database File and Initial Condition Types.

You can specify various types of initial conditions, depending on the analysis to be performed. For information about each type of initial condition, see Initial Condition Types.

The input data for an initial conditions definition can be contained in a separate file. See Input Syntax Rules for the syntax of such file names.

INITIAL CONDITIONS, INPUT=file_name

You can use field results from a prior simulation as initial conditions for another simulation in many cases. This method uses functionality associated with importing external fields, discussed in General Capability for Importing External Fields. The output database from the prior simulation must be in the .sim format. If the previous analysis is performed with third-party software, you must convert the results file to the .sim file format.

This method for specifying initial conditions cannot be used for initial acoustic static pressure, initial location of an enriched feature, initial fluid pressure, initial gap, initial mass flow rate, reference mesh (initial metric) for membrane elements, initial velocities specified either directly or in terms of an angular velocity and a global translational velocity, initial spud embedment, initial spud preload, initial unfold coordinates, and initial volume fraction.

You can use any appropriate result from the output database by specifying an output variable identifier (see Abaqus/Standard Output Variable Identifiers and Abaqus/Explicit Output Variable Identifiers, for available output variable identifiers). The results data can be associated with nodes or elements.

You can specify a source region (node or element set in the previous model) if data are imported only from a subset of the previous model. Sometimes a source region is also specified to eliminate ambiguity during mapping. You can specify a target region if data are specified only on a subset of the current model.

You must specify the full name of the output database file including the file extension .sim.

You can import only results data requested on two- and three-dimensional continuum elements and three-dimensional conventional shell elements, and you can specify imported data only for elements with matching types. You cannot import data from three-dimensional continuum elements to shell elements, or vice versa. When importing tensor field data, the source region must contain only elements with the same number of components of the tensor field. For example, when specifying initial stress with stress data from a previous analysis, you must separate the solid elements and shell elements in the previous analysis into separate source regions.

When you use results data to specify some initial conditions, data are mapped directly to all integration points and section points of a target element. These conditions include initial stress, initial plastic strain, initial damage initiation, initial hardening, and initial specific energy.

The following considerations pertain to importing data from shell elements to shell elements:

• You can import data from shell elements to shell elements with a different number of section points, except for initial temperatures and initial field variables.
• When importing element data, Abaqus requires that the elements in the same source/target region have the same number of layers, section points, and integration rules.
• When importing element data between shell elements with multiple layers, Abaqus requires the source and target elements to have the same number of layers. If results data are found only at the default output points, the same shell thickness between source and target elements is also required. Abaqus also requires that the elements in the same source/target region have the same shell thickness for each layer in this case.
• When results data are requested at all section points in the previous analysis, if a different number of section points are detected in the source and target elements, Abaqus automatically interpolates linearly in the thickness direction between the two closest section points in the source element to find the value at the section point in the target element. When results data are requested only at the default output points in the previous analysis, Abaqus interpolates linearly in the thickness direction using data at the top and bottom of the source shell elements.

You can specify mapping tolerances and special tensor averaging methods if mapping is performed. If the model in the previous analysis is repositioned in the current analysis, you must specify the translation and rotation so that the source region can be repositioned before data are imported, except in the following cases;

• Scalar data are imported from a matching mesh.
• Tensor data are imported from a matching mesh, and there is no rotation between the source region and the target region.

INITIAL CONDITIONS
EXTERNAL FIELD, FILE=file name
blank, target_set, blank, NODES/ELEMENTS, source_set, outputvar, mapcontrol, fieldop

*FIELD MAPPER CONTROLS, NAME=mapcontrol
 , , 1.0

*FIELD OPERATIONS, NAME=fieldop
x, y, z
x1, y1, z1, x2, y2, z2, rotation

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 and Linear Constraint Equations). 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.

When you define initial conditions using a method that interpolates between dissimilar meshes, Abaqus operates by interpolating results from nodes in the old mesh to nodes in the new mesh. For each node:

1. The element (in the old mesh) in which the node lies is found, and the node's location in that element is obtained. (This procedure assumes that all nodes in the new mesh lie within the bounds of the old mesh: warning messages are issued if this is not so.)

2. The initial condition values are then interpolated from the nodes of the element (in the old mesh) to the new node.

Elements that do not support spatial interpolation include the complete libraries of convective heat transfer elements, axisymmetric elements with nonlinear axisymmetric deformation, axisymmetric surface elements, truss elements, beam elements, link elements, hydrostatic fluid elements, solid infinite stress elements, and coupled thermal/electrical elements. Other specific elements that are not supported include: GKPS6, GKPE6, GKAX6, GK3D18, GK3D12M, GK3D4L,GK3D6L, GKPS4N, GKAX6N, GK3D18N, GK3D12MN, GK3D4LN, and GK3D6LN.