3.2.27 Mapping thermal and magnetic loads
Product: Abaqus/Standard
References
Overview
The abaqus emloads utility converts results output from a time-harmonic eddy current analysis for use as loads in a subsequent heat transfer, coupled temperature-displacement, or stress/displacement analysis. For example, magnetic body force intensity output is converted to point loads. You specify the names of the time-harmonic eddy current analysis results output database (.odb) file and the input file for the subsequent analysis on the command line. The utility creates an output database file containing a mesh that matches the mesh in your subsequent analysis and steady-state concentrated nodal fields consistent with the time-harmonic eddy current analysis results. Your time-harmonic eddy current and subsequent analysis meshes can be dissimilar, and results transfer ensures global conservation of the flux quantities when your model domains match; i.e., the model boundaries are the same. You can then use this new output database file to apply concentrated loads and concentrated heat fluxes in the subsequent analysis.
Results conversion
The utility converts whole element output quantities from a time-harmonic eddy current analysis to nodal results. You use the options listed in Table 3.2.27–1 in the subsequent analysis to specify the output database file (and optionally the step and increment) from which the data are to be read.
Table 3.2.27–1 Supported results conversion.
| Electromagnetic analysis output variable | Converted output variable | Input file option |
|---|---|---|
| Rate of Joule heat dissipation EMJH | Concentrated heat flux CFL11 | *CFLUX, FILE=odb-name, STEP=step-number, INC=inc |
| Magnetic body force intensity EMBF | Point load components CF | *CLOAD, FILE=odb-name, STEP=step-number, INC=inc |
Utility execution
The utility executes in two phases. Abaqus writes progress information and, if appropriate, error messages to the screen during each phase.
In the first phase a datacheck analysis is performed on your subsequent analysis input file to create an output database representation of a “target” mesh. This phase requires that your input file be sufficiently complete to successfully run abaqus datacheck, with the exception that you can have *CFLUX and *CLOAD options that include the FILE parameter to refer to files that are not available. If this phase is successful, the utility proceeds to the second phase; otherwise, an error message is issued.
In the second phase time-harmonic eddy current analysis load data are mapped from the source to the target output database. In this phase all steps and increments found in the original analysis are defined in the target output database. This phase requires that your target model domain lie within the source model domain. If it does not, an appropriate error message is issued.
Command line options
This option specifies the name of the resulting “target” output database file.
This option specifies the name of the subsequent analysis Abaqus input file. This file must be sufficiently complete to successfully run, as described above.
This option specifies the name of the time-harmonic eddy current analysis output database file.