General Capability for Importing External Fields

You can import external fields from an output database (.sim) file, also referred to as a SIM database (see The Output Database). Once imported, the external field can be used to define distributions, initial conditions, and history-dependent fields (such as loads, boundary conditions, and predefined fields). External fields can also be used for node-based submodeling as discussed in About Submodeling. Importing external fields to define history-dependent fields or node-based submodeling is supported only in Abaqus/Standard.

The external field can be evaluated at nodes, integration points, or element centers. Conservative mapping is performed automatically if the fields are evaluated at different locations or if the meshes are different. Importing an external field is supported for most two-dimensional and three-dimensional continuum elements. When used to define distributions and initial conditions, external fields are also supported for three-dimensional conventional shell elements made of a single material. All field quantities are exchanged in the global Cartesian coordinate system.

Abaqus offers alternate interfaces for sequential coupling (see Predefined Fields for Sequential Coupling, Sequentially Coupled Thermal-Stress Analysis, and Predefined Loads for Sequential Coupling). These interfaces are limited to importing temperatures, normalized concentrations, and electromagnetic loads of a previous Abaqus analysis.

You can import external fields from an output database (.sim) file. You specify the file name (including the file extension) from which to import external fields.

You can import external fields to define distributions (see Defining Distributions by Importing Field Data from an Output Database File). A common case is an injection molding manufacturing process where a molten fibrous material is injected into a mold. You can use injection molding software to model the manufacturing process and then import the section and material properties (such as local element orientation and fiber dispersion) into a subsequent stress-displacement simulation.

You can import an external field to adjust nodal coordinates.

One common case is to introduce a geometric imperfection into a model for a postbuckling analysis. In this case, the previous analysis must contain the mode shapes from an eigenfrequency extraction analysis or nodal displacements from a static or dynamic analysis. Mapping is performed if the postbuckling analysis uses a dissimilar mesh. The imperfection is introduced by adjusting the nodal coordinates using the imported modal shapes or nodal displacements.

Another common case is to adjust nodal coordinates using the deformed configuration from a previous analysis. In this case, the previous analysis must write the nodal displacements to a SIM database.

You can import an external field to define initial conditions (see Initial Conditions). A common case is a geomechanics analysis where you import an initial pore pressure field. You can compute a pore pressure field using a reservoir code and then import the field into a subsequent geostatic stress state procedure (see Geostatic Stress State). This procedure is used to compute the equilibrium state before performing a geotechnical analysis using the coupled pore fluid diffusion and stress analysis procedure in Abaqus (see Coupled Pore Fluid Diffusion and Stress Analysis). In this case, the reservoir code must write the pore pressure to a SIM database.

You can import external fields to define loads, boundary conditions, and predefined fields. A common case is a sequential thermal-stress analysis, where you first perform a heat transfer analysis (see Uncoupled Heat Transfer Analysis) to compute a temperature field and then import the temperatures into a subsequent stress-displacement analysis (see Static Stress Analysis).

You can import external fields for the following time-based analysis procedures:

• Static Stress Analysis

• Implicit Dynamic Analysis Using Direct Integration

• Uncoupled Heat Transfer Analysis

• Fully Coupled Thermal-Stress Analysis

• Piezoelectric Analysis

• Coupled Thermal-Electrical Analysis

• Eddy Current Analysis

• Coupled Pore Fluid Diffusion and Stress Analysis

• Mass Diffusion Analysis

External fields can be imported only in one analysis step per analysis. The analysis step must be a general analysis (nonperturbation) step. For any subsequent analysis steps, the applied external fields remain constant based on the last imported values.

If the previous analysis is an Abaqus analysis, you request the source fields to write to the output database (.sim) file. When importing external fields over a time range, you must request output at a frequency to achieve sufficient solution accuracy (see Controlling the Frequency of Output to the Output Database).

When importing an external field, you define the target and source fields. The target field is the field defined in the current analysis. The source field is the field computed in a previous analysis. A field is a physical quantity that spans a region. The field is a node-based field if evaluated at nodes or an element-based field if evaluated at element centroids, integration points, or surface facets. You define a region by specifying a node set, an element set, or a surface regardless of where the field is evaluated.

When a node-based field is imported and an element set from the previous model is specified, the field is extracted from nodes of the elements in the specified element set. Similarly, when a node-based field is imported and a surface from the previous model is specified, the field is extracted from the nodes belonging to the surface facets of the specified surface. When an element-based field is imported and a node set from the previous model is specified, the element field is extracted from elements containing the nodes in the node set. Elements connected to nodes that are not in the node set are not included.

When importing an external field, you specify the region name space, the region name, and the physics quantity for the target field and the source field. The region name space specifies whether the region is a node set, an element set, or a surface. The region name is the name of a node set, element set, or surface.

When specifying the target field and source field parameters, you should consider the following conditions:

• The source field region name is optional. If it is not specified, the entire model is used. However, you are encouraged to provide the source field region name to reduce the computational cost associated with mapping and data transfer.
• When defining initial conditions, the target field region name space and physics quantities are defined by the initial condition definition and, consequently, are not used.
• When defining distributions, the target field region name space, region name, and physics quantities are defined by the distribution definition and, consequently, are not used.
• When used for node-based submodeling, the target region is a node set.

The physics quantities for the target field and the source field are defined using identifiers. The physics quantity identifiers for the target field depend on the analysis procedure. Table 1 lists the supported identifiers. If the source analysis is an Abaqus analysis, the identifiers are defined in Abaqus/Standard output variable identifiers. Most field-type quantities can be extracted from the output database file.

Table 1. Supported target field identifiers.

Analysis	Physics Quantity ID	Description
Analysis procedures supporting mechanical degrees of freedom*	U	Displacement
	V	Velocity
	CF	Force
Analysis procedures supporting thermal degrees of freedom*	NT	Nodal temperature
	CFL	Concentrated heat flux at a node
Analysis procedures supporting pore fluid pressure degree of freedom	POR	Pore pressure
	CFF	Concentrated fluid flow at a node
Analysis procedures supporting mass concentration	CFL	Concentrated mass flux at a node
	SINV	Equivalent pressure stress
	NNC	Normalized concentration
Analysis procedures supporting electric potential	EPOT	Electric potential
	ECD	Electric current density
All procedures*	TEMP	Predefined temperature field
	FVn	Predefined field
	ESDVn	Element solution-dependent variable
*Procedures excluding explicit dynamics.

Field are mapped automatically when the source and target meshes are topologically different. However, Abaqus performs a mesh check internally before importing distributions and initial conditions, and, if the following conditions are satisfied, no mapping is performed:

• All of the nodes and elements in the target region are found in the source output database (.sim) file with matching labels.
• Matching elements in the target region and the source .sim file have the same connectivities and element types.
• Source data are requested at the same location (nodes or element integration points) where distributions are specified.

When importing field variables and temperature as a field variable, you might notice differences when you compare the source and target fields. There are two possible causes of these differences:

• Field variables and temperature as a field variable are mapped accurately and imported at nodes. However, when saved to the output database, these quantities are interpolated to element integration points. When contouring, some averaging can occur depending on the contouring parameters selected.
• For fully integrated first-order elements, a selective reduced-integration technique is employed (see Solid isoparametric quadrilaterals and hexahedra). In this case field variables and temperature as a field variable are averaged at the element center and saved to the output database.

The values correctly reflect the internal magnitudes used by Abaqus.

To define distributions or initial conditions, you can specify the step and the increment from which to extract the field values. You must ensure that the field is saved to the SIM database at the specified step and increment. If the increment is omitted, the values at the end of the step are imported.

You can import fields at a specified time. You specify the time to extract field data from the SIM database. Abaqus linearly interpolates between the time points available in the output database to obtain field values at the requested time.

You can specify the analysis step, in which case the time refers to the step time to extract field values in the output database. If you specify a step without any time parameters, the last available field values for the analysis step are obtained, which might be useful when reading from a steady-state analysis where time has no physical meaning.

You can import fields over a specified time range when importing fields to define history-dependent fields. You specify the start and end times to define the time range in the source analysis to extract field values. Typically, data corresponding to these time points are not present in the output database. Abaqus linearly interpolates between the time points stored in the output database to obtain values at the required time. Because the interpolation is linear, you must ensure that sufficient data is available in the output database to achieve meaningful interpolation.

You can specify the analysis step, in which case the time range refers to the analysis step time to extract field values in the output database.

The physics time scales might be different when performing a sequential analysis. For example, you can perform an electromagnetic analysis followed by a thermal-stress analysis importing heat losses. The time scale for the electromagnetic analysis might be significantly shorter than the time scale for conduction in the thermal-stress analysis. When the requested time range of the source analysis is different from the analysis step time of the current analysis, Abaqus automatically scales the time periods.

Typically, the source and target regions have different meshes. Fields are mapped conservatively between the source and target meshes, and Abaqus selects the most appropriate mapping algorithm based on the field properties. For most cases, the default settings for the mapping algorithm are adequate, but you can modify the mapper settings by specifying field mapper controls when importing distributions and initial conditions. You cannot specify mapping controls when importing step-dependent field data or when used for a submodel analysis.

Orphan members might be reported during the mapping operation. Orphan members are nodes or elements for which the mapper cannot find a correspondence with the source mesh. Consequently, the mapper does not compute field values at these locations. In this case, you can modify the default search tolerances or specify how to treat orphan members.

You can apply one or more field operations when importing fields.

You can scale a field by a constant value by providing a scale factor. The scaling factor is intended to scale a field by a physical constant. It is not intended for unit conversion; for example, where you might need additional parameters to convert a temperature field.

You can extract a component of a vector or tensor field by providing a component index, i. The i^th component of the source vector or tensor field is extracted and then mapped and imported as a scalar field. The components are extracted in the local coordinate system of the source field. You can apply component extraction when importing distributions, initial conditions, and history-dependent fields; it cannot be used for a submodel analysis.

If a region in the previous analysis is not colocated with the region in the current analysis, you must specify the translation and rotation to reposition the source region before field values are imported. You specify a rotation by giving two points, a and b, to define a rotation axis and a right-handed angular rotation about the axis. Local coordinate systems defined within the source region are translated and rotated according to the specified positioning data.