transfer analysis (field variables and temperatures) or stress/displacement analysis (pressure stress). The .fil file extension is optional. # Reading initial values of a temperature field from a user-specified output database file An Abaqus/Standard output database file (in ODB or SIM format) can be used to specify initial values of temperature (see “Defining initial temperatures” in “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.2.1). The part (.prt) file from the original analysis is also required when reading data from the output database file. Temperature values can be read between dissimilar meshes, as described in “Interpolating initial temperatures for dissimilar meshes from a user-specified results or output database file” in “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.2.1. # Initializing predefined field variables from a user-specified output database file in Abaqus/Standard In Abaqus/Standard nodal values of temperature (NT), normalized concentrations (NNC), and electric potential (EPOT) can be used to initialize predefined fields (see “Defining initial values of predefined field variables” in “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.2.1). The part (.prt) file from the original analysis is also required when reading data from the output database file. The scalar nodal values can be mapped between dissimilar meshes, as described in “Defining initial predefined field variables by interpolating scalar nodal output variables for dissimilar meshes from a user-specified output database file” in “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.2.1. # Defining time-dependent fields The prescribed magnitude of a field can vary with time during a step according to an amplitude function. See “Prescribed conditions: overview,” Section 34.1.1, and “Amplitude curves,” Section 34.1.2, for details.

Input File Usage:	Use one of the following options:*TEMPERATURE, AMPLITUDE=amplitude_name*FIELD, AMPLITUDE=amplitude_name*PRESSURE STRESS, AMPLITUDE=amplitude_name*MASS FLOW RATE, AMPLITUDE=amplitude_name
Abaqus/CAE Usage:	In Abaqus/CAE only predefined temperature fields are available.Load module:Create Predefined Field: Step: analysis_step: chooseOther for the Category and Temperature for the Types for SelectedStep: select region: Distribution: Direct specification or select an analytical field or a discrete field, Amplitude: amplitude_name

# Field propagation By default, all fields defined in the previous general analysis step remain unchanged in the subsequent general step or in subsequent consecutive linear perturbation steps. Fields do not propagate between linear perturbation steps. You define the fields in effect for a given step relative to the preexisting fields. At each new step the existing fields can be modified and additional fields can be specified. If you specify additional values for a field, the definition of the field will be extended to those nodes where it was previously undefined. Alternatively, you can release all previously applied fields of a given type in a step and specify new ones. In this case any fields of that type that are to be retained must be respecified. # Modifying fields By default, when you modify existing temperatures, field variables, pressure stresses, or mass flow rates, all existing values of the field remain. Input File Usage: Use one of the following options to modify an existing field or to specify an additional field: \*TEMPERATURE, OP=MOD \*FIELD, OP=MOD \*PRESSURE STRESS, OP=MOD \*MASS FLOW RATE, OP=MOD Abaqus/CAE Usage: In Abaqus/CAE only predefined temperature fields are available. Load module: Create Predefined Field or Predefined Field Manager: Edit # Removing fields A field that is removed is reset to the value given as an initial condition or to zero if no initial condition was defined. When fields are reset to their initial conditions, the amplitude referred to in the field definition does not apply. In Abaqus/Standard the amplitude variation defined for the step governs the behavior; in most Abaqus/Standard procedures the default is to ramp the fields back to their initial conditions (see “Defining an analysis,” Section 6.1.2). In Abaqus/Explicit the values are always ramped linearly over the step back to their initial conditions. If the temperatures, field variables, pressure stresses, or mass flow rates are reset to a new value (not to their initial conditions), the amplitude referred to in the field definition applies. If you choose to remove any field in a step, no fields of that type will be propagated from the previous general step. All fields of the same type that are in effect during this step must be respecified. Input File Usage: Use one of the following options to release all previously applied fields of a particular type and to specify new fields: \*TEMPERATURE, OP=NEW \*FIELD, OP=NEW \*PRESSURE STRESS, OP=NEW \*MASS FLOW RATE, OP=NEW If the OP=NEW parameter is used on any field option in a step, it must be used on all field options of the same type within the step. Abaqus/CAE Usage: Use the following option to reset a temperature field to the value prescribed in the initial step (or to zero if no initial value was defined): Load module: temperature field editor: Reset to initial # Reading the values of a field directly from an alternate input file The data for predefined temperature, field variables, pressure stress, or mass flow rate can be contained in a separate input file (see “Input syntax rules,” Section 1.2.1). Input File Usage: Use one of the following options: \*TEMPERATURE, INPUT=file\_name \*FIELD, INPUT=file\_name \*PRESSURE STRESS, INPUT=file\_name \*MASS FLOW RATE, INPUT=file\_name If the INPUT parameter is omitted, it is assumed that the data lines follow the keyword line. Abaqus/CAE Usage: You cannot read field data from a separate input file in Abaqus/CAE. # Reading the values of a field from a user-specified file Nodal temperatures calculated during an Abaqus/Standard heat transfer or coupled thermal-electrical analysis can be used to define temperatures in a subsequent analysis. The temperatures must have been written to the results or output database file. If nodal temperatures are written to the results file during an Abaqus/Standard heat transfer or coupled thermal-electrical analysis, they can be used to define field variables in a subsequent analysis. In Abaqus/Standard if nodal values of temperature (NT), normalized concentrations (NNC), or electric potential (EPOT) are written to the output database file, they can be used to define field variables in a subsequent Abaqus/Standard analysis. In Abaqus/Standard equivalent pressure stresses calculated during a mechanical analysis can be used in a subsequent mass diffusion analysis if the element output variable SINV was written to the results file averaged at the nodes (see “Element output” in “Output to the data and results files,” Section 4.1.2). Once the data are available in a results file or output database file, they can be read into a subsequent analysis as a predefined field. Data for field variables and pressure stress can be read from a previously generated results file. In Abaqus/Standard data can also be read from a previously generated output database file. Data for temperatures can be read from a previously generated results or output database file. Data for temperatures (and field variables in Abaqus/Standard) to be interpolated between dissimilar meshes can be read only from the output database file. The part (.prt) file from the original analysis is also required when reading data from the results or output database file. When the output file of an Abaqus analysis involving beam and/or shell elements is used to define temperatures, you must ensure that the number of temperature points through the section defined for corresponding elements is consistent between the two analyses. Inconsistent temperature point definition will result in an incorrect transfer of prescribed field quantities. # Reading field values from a user-specified results file To read field values from a user-specified results file, the data must have been written to the results file as nodal output (see “Node output” in “Output to the data and results files,” Section 4.1.2). Only nodal quantities can be read from the results file. Since field variables can be written to the results file only as element quantities (record key 9), they cannot be read directly into a subsequent analysis. In this case you must generate a results file with the field data in the temperature record, even if the field variable in the current analysis is the same as a field variable in the previous analysis. Multiple results files must be generated for multiple field variables. To generate the results file, you can write a program to create a results file (without running an Abaqus analysis) according to the format described in Chapter 5, “File Output Format.” Examples of such programs are shown in that chapter. If the values will be read in as temperatures or field variables, the data must be written as nodal quantities with record key 201. If the values will be read in as a pressure stress field, the data must be averaged at the nodes (as explained in “Output to the data and results files,” Section 4.1.2) and written as record key 12. # Specifying the results file to be read You must specify the name of the results file from which the data are to be read for a temperature, field variable, or pressure stress. The .fil file extension is optional. If both .fil and .odb files exist for a temperature field and no extension is specified, the results file will be used. ```txt Input File Usage: *TEMPERATURE, FILE=file *FIELD, FILE=file *PRESSURE STRESS, FILE=file ``` Abaqus/CAE Usage: In Abaqus/CAE only predefined temperature fields are available. Load module: Create Predefined Field: Step: analysis\_step: choose Other for the Category and Temperature for the Types for Selected Step: select region: Distribution: From results or output database file, File name: file # Creating a cyclic temperature history In a direct cyclic analysis in Abaqus/Standard the temperature values must be cyclic over the step: the start value must be equal to the end value. To create a cyclic temperature history from a prior heat transfer analysis that is not cyclic, you can set the starting time, f (measured relative to the total step time period, $t ^ { \sigma } )$ , after which the temperatures read from the results file will be ramped back to their initial condition values. At any time point $t \geq f t ^ { \sigma }$ , the temperature value is equal to $$ p T e m p ^ {\theta} + (1 - p) T e m p ^ {i n i}, $$ where $\begin{array} { r } { p \ = \ \frac { \left( t ^ { \sigma } - t \right) } { \left( t ^ { \sigma } - f t ^ { \sigma } \right) } } \end{array}$ , $T e m p ^ { i n i }$ is the initial condition value, and $T e m p ^ { \theta }$ is the interpolated value obtained from the results file at time t, as illustrated in Figure 34.6.1–1. Input File Usage: Use the following option to set the starting time for a cyclic temperature history: \*TEMPERATURE, FILE=file, BTRAMP=f Abaqus/CAE Usage: Cyclic temperature histories are not supported in Abaqus/CAE. 

line

| t | Temp | |-------|-------| | ft^σ | ~0.5 | | t^σ | ~0.2 |

Figure 34.6.1–1 Ramp temperatures to their initial condition values after $t = f t ^ { \sigma }$ to create a cyclic temperature history. # Reading temperature values from a user-specified output database file To read temperature values from a user-specified database file, the temperatures must have been written to the output database file (in ODB or SIM format) as nodal output (see “Node output” in “Output to the output database,” Section 4.1.3). Specifying the output database file to be read for a temperature field You must specify the name of the output database file (in ODB or SIM format) from which the data are to be read for a temperature field. The file extension must be included if any two of the following files exist: the results file, the ODB output database file, or the SIM database file. Only the data for the part instances that are common to both the analyses will be transferred. If the part instance names differ, you must activate the general interpolation capability. Input File Usage: \*TEMPERATURE, FILE=file Abaqus/CAE Usage: Load module: Create Predefined Field: Step: analysis\_step: choose Other for the Category and Temperature for the Types for Selected Step: select region: Distribution: From results or output database file, File name: file Reading temperatures from a SIM database file is not supported in Abaqus/CAE. # Defining fields using nodal scalar output values from a user-specified output database file In Abaqus/Standard if nodal values of temperature (NT), normalized concentrations (NNC), or electric potential (EPOT) are written to the output database file, they can be used to define field variables in a subsequent Abaqus/Standard analysis. To read these values from a user-specified output database file, they must have been written to the output database file as nodal output (see “Node output” in “Output to the output database,” Section 4.1.3). Specifying the output database file to be read for a field variable You must specify the name of the output database file from which the data are to be read for a field variable. The .odb extension must be included if both results and output database files exist. Input File Usage: \*FIELD, FILE=file, OUTPUT VARIABLE=scalar nodal output variable, Abaqus/CAE Usage: Predefined field variables are not supported in Abaqus/CAE. # Interpolating data between meshes Data can be mapped between the same meshes, between meshes that differ only in the element order (first-order element in heat transfer analysis and second-order element in thermal-stress analysis), or between dissimilar meshes of matching element dimensionality (solid element to solid element or shell element to shell element). If data are mapped between the same meshes, no additional computations are required. To transfer data between meshes that differ only in the element order, you must activate the midside node capability. To map data between dissimilar meshes, you must activate the general interpolation capability. The midside node capability is available only for temperatures. The midside node capability and the general interpolation capability are mutually exclusive. Using second-order stress elements with first-order heat transfer elements (the midside node capability) In some cases it makes sense to perform an Abaqus/Standard heat transfer analysis using first-order elements followed by a thermal-stress analysis using second-order elements (and an otherwise similar mesh). For example, a heat transfer analysis including latent heat effects—for which first-order elements are best suited—can be followed by a stress analysis using second-order elements, which generally have superior deformation characteristics. In addition, the first-order temperature field calculated in the heat transfer analysis is consistent with the first-order thermal strain field provided by the second-order stress/displacement elements. For the instances in which there is a change in the order of interpolation of element temperature variables between the heat transfer analysis and the stress analysis, temperatures must be assigned to the midside nodes of the stress/displacement elements based on the temperatures of the corner nodes of the heat transfer elements. If you specify that the midside node temperatures are needed, Abaqus will interpolate the temperatures of the midside nodes of the second-order stress/displacement elements from the corner nodes using first-order interpolation. If the midside node capability is activated in cases where both the heat transfer analysis and the stress analysis are performed with second-order elements, it is ignored. One exception is that if variable-node second-order stress/displacement elements are used in the stress analysis, activating the midside node capability will cause Abaqus to interpolate the temperatures of the midface nodes in the variable node elements from the corner or midside nodes using first-order interpolation. Since it is assumed that the corner node temperatures have been generated in a previous heat transfer analysis, the midside node capability can be used only when the temperature field values are read from a user-specified results or output database file. You must ensure that the nodal temperatures calculated during the heat transfer analysis are written to the results or output database file. Once the temperatures of the corner nodes are read in the subsequent stress/displacement analysis, Abaqus interpolates the midside node temperatures so that all nodes have temperatures assigned to them. You must ensure that all temperatures of the corner nodes belonging to elements for which midside node temperatures are to be interpolated are read from the heat transfer analysis results or output database file. If the corner node temperatures are defined using a mixture of direct data input, reading from the results file or output database file, and user subroutine UTEMP, 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 in a step, the capability will remain active throughout the remainder of the analysis. Values of temperature for nodes that existed in the original analysis but do not exist in the current analysis will be ignored. Similarly, if additional nodes (but not midside nodes) exist in the current analysis, the values of fields at these nodes cannot be prescribed by reading the output files. # Input File Usage: Use the following option to interpolate temperatures between meshes that differ only in the element order: \*TEMPERATURE, FILE=file, MIDSIDE # Abaqus/CAE Usage: Load module: Create Predefined Field: Step: analysis\_step: choose Other for the Category and Temperature for the Types for Selected Step: select region: Distribution: From results or output database file, File name: file, Mesh compatibility: Compatible, and toggle on Interpolate midside nodes Interpolating temperatures between dissimilar meshes (the general interpolation capability) In some cases the model for a heat transfer analysis and the model for a thermal-stress analysis may require different meshes; for example, you may want to model a smooth temperature distribution in the heat transfer analysis and stress concentration regions in the thermal-stress analysis. Both meshes have to be different and independent of each other in such cases. Abaqus offers a general interpolation capability that allows for the use of dissimilar meshes for heat transfer and thermal-stress analyses. The interpolation is always based on the initial (undeformed) configurations. If the mesh for which the temperature field is obtained is quite different from the initial (undeformed) configuration for the thermal-stress analysis, the interpolation may not work properly even when using the tolerance parameters discussed below. Temperatures can be interpolated between dissimilar meshes only when the temperatures are read from an output database file (in ODB or SIM format). If temperatures for nodes in the heat transfer analysis that are needed for interpolation are not written to the output database file, the values at those nodes are assumed to be zero, which may lead to incorrect results for the temperature values in the stress analysis. Similarly, if additional nodes exist in the mesh for the stress analysis, the values of temperatures at these nodes are assumed to be zero. Interpolation of temperatures can also be used for specifying temperature as a field variable in a submodel thermal-stress analysis where the temperature values are read directly from a global heat transfer analysis. You can specify an interpolation tolerance for use in locating the nodes in the heat transfer analysis. The tolerance can be specified as an absolute value or as a fraction of the average element size. In a multistep thermal-stress analysis in which several steps read the temperature values from the same file, Abaqus interpolates the temperature values only once. If different interpolation tolerance values are used for each step, the interpolation is based on the largest specified tolerance value. If a restart analysis is performed from a particular step in the thermal-stress analysis, the restart interpolation is based on the tolerance value specified for that step. Input File Usage: Use the following option to interpolate temperatures between dissimilar meshes: \*TEMPERATURE, FILE=file.odb/file.sim, INTERPOLATE Use the following option to specify the interpolation tolerance as an absolute value: \*TEMPERATURE, FILE=file.odb/file.sim, INTERPOLATE, ABSOLUTE EXTERIOR TOLERANCE=tolerance Use the following option to specify the interpolation tolerance as a fraction of the average element size: \*TEMPERATURE, FILE=file.odb/file.sim, INTERPOLATE, EXTERIOR TOLERANCE=tolerance Abaqus/CAE Usage: Load module: Create Predefined Field: Step: analysis\_step: choose Other for the Category and Temperature for the Types for Selected Step: select region: Distribution: From results or output database file, File name: file.odb, Mesh compatibility: Incompatible, exterior tolerance: absolute or relative tolerance Interpolating temperatures from a SIM database file is not supported in Abaqus/CAE. Interpolating temperatures between dissimilar meshes with user-specified regions When regions of elements in the heat transfer analysis are close or touching, the dissimilar mesh interpolation capability can result in an ambiguous temperature association. For example, consider a node in the current model that lies on or close to a boundary between two adjacent parts in the heat transfer model, and consider a case where temperatures in these parts are different. When interpolating, Abaqus will identify a corresponding parent element at the boundary for this node from the heat transfer analysis. This parent element identification is done using a tolerance-based search method. Hence, in this example the parent element might be found in either of the adjacent parts, resulting in an ambiguous temperature definition at the node. You can eliminate this ambiguity by specifying the source regions from which temperatures are to be interpolated. The source region refers to the heat transfer analysis and is specified by an element set. The target region refers to the current analysis and is specified by a node set. Input File Usage: Use the following option to interpolate temperatures between dissimilar meshes with user-specified regions: $$ \begin{array}{l} * \text { TEMPERATURE, FILE = file.odb / file. sim, INTERPOLATE, } \\ \text { DRIVING ELSETS } \end{array} $$ Abaqus/CAE Usage: You cannot specify the regions where temperatures are to be interpolated in Abaqus/CAE. Interpolating scalar nodal output variables between dissimilar meshes (the general interpolation capability) onto field variables in Abaqus/Standard Abaqus/Standard offers a general interpolation capability that allows for nodal values of temperature, normalized concentration, and electric potential from one analysis to be mapped onto field variables in a subsequent analysis in the cases where the meshes in the two analyses are dissimilar. The interpolation is always based on the initial (undeformed) configurations. If the mesh for which the field variable is obtained is quite different from the initial (undeformed) configuration for the original analysis, the interpolation may not work properly even when using the tolerance parameters discussed below. Temperatures, normalized concentrations, and electric potentials can be interpolated between dissimilar meshes onto field variables only when they are read from an output database file. If scalar values for nodes in the current analysis that are needed for interpolation are not written to the output database file, the values at those nodes are assumed to be zero, which may lead to incorrect results for the field variables. Similarly, if additional nodes exist in the mesh for the current analysis, the values of the field variables at these nodes are assumed to be zero. You can specify an interpolation tolerance for use in locating the nodes in the original analysis. The tolerance can be specified as an absolute value or as a fraction of the average element size. In a multistep analysis in which several steps read nodal output variables values from the same file, Abaqus interpolates the nodal values only once. If different interpolation tolerance values are used for each step, the interpolation is based on the largest specified tolerance value. If a restart analysis is performed from a particular step in the original analysis, the restart interpolation is based on the tolerance value specified for that step. Input File Usage: Use the following option to interpolate scalar nodal output variables between dissimilar meshes: $$ \begin{array}{l} * \text {FIELD, FILE = file.odb, OUTPUT VARIABLE = scalar nodal} \\ \text {output variable, INTERPOLATE} \end{array} $$ Use the following option to specify the interpolation tolerance as an absolute value: \*FIELD, FILE=file.odb, OUTPUT VARIABLE=scalar nodal output variable, INTERPOLATE, ABSOLUTE EXTERIOR TOLERANCE=tolerance Use the following option to specify the interpolation tolerance as a fraction of the average element size: \*FIELD, FILE=file.odb, OUTPUT VARIABLE=scalar nodal output variable, INTERPOLATE, EXTERIOR TOLERANCE=tolerance Abaqus/CAE Usage: Predefined field variables are not supported in Abaqus/CAE. # Specifying the step and increment to be read from the file You can specify the first and last step, respectively, from which results will be read. Similarly, you can specify the first and last increment, respectively, from which results will be read. You can specify any combination of these values. Any zero-increment file output that is present in the results file of an Abaqus/Standard analysis (written only if the zero increment results are requested; see “Obtaining results at the beginning of a step” in “Output,” Section 4.1.1) will be ignored. Results must have been written to the results or output database file at the specified step and increment. If you do not specify the first step from which to read, Abaqus will begin reading results from the first step available in the results or output database file. If you do not specify the first increment from which to read, Abaqus will begin reading results from the first increment available in the first step from which results will be read (the first increment following the zero increment if zero-increment file output is present in the results file). If you do not specify the last step from which to read, the first step from which results will be read will also be the last step. If you do not specify the last increment from which to read, Abaqus will read the results or output database file until it reaches the last available increment in the last step from which results will be read. Input File Usage: Use one of the following options: \*TEMPERATURE, FILE=file, BSTEP=bstep, BINC=binc, ESTEP=estep, EINC=einc \*FIELD, FILE=file, BSTEP=bstep, BINC=binc, ESTEP=estep, EINC=einc \*PRESSURE STRESS, FILE=file, BSTEP=bstep, BINC=binc, ESTEP=estep, EINC=einc For example, the following input would read temperature data from output database file heat.odb beginning at Step 2, increment 2, and ending at Step 3, increment 5: \*TEMPERATURE, FILE=heat.odb, BSTEP=2, BINC=2,ESTEP=3, EINC=5 Abaqus/CAE Usage: In Abaqus/CAE only predefined temperature fields are available.