Predefined Loads for Sequential Coupling

The values of the following whole element output quantities, generated in an Abaqus/Standard time-harmonic eddy current analysis, can be read into subsequent Abaqus/Standard analyses as point loads for sequentially coupled multiphysics workflows:

  • Rate of Joule heat dissipation

  • Magnetic body force intensity

A sequentially coupled multiphysics analysis can be used to apply electromagnetically generated loads (from a time-harmonic eddy current analysis) in a heat transfer, coupled temperature-displacement, or stress/displacement analysis. In many cases coupling is important only from the time-harmonic eddy current analysis; the impact of loading on the structure's mechanical or thermal response is not great enough to affect the validity of the original time-harmonic eddy current analysis.

This page discusses:

See Also
Defining an Analysis
Eddy Current Analysis
In Other Guides
Mapping Thermal and Magnetic Loads
Concentrated Loads

Products Abaqus/Standard

Saving Joule Heat Dissipation or Magnetic Body Force Intensity for Use in Subsequent Analyses

You can request Joule heat dissipation output (EMJH) or magnetic body force intensity output (EMBF) in a time-harmonic eddy current analysis. Only values stored in the output database (.odb) file are available for use with sequential coupling.

Converting Results for Subsequent Use

The whole element quantities are converted to nodal load quantities using the abaqus emloads utility. The utility converts Joule heat dissipation output to concentrated heat flux and magnetic body force intensity output to point loads. This utility also enables conversion of results between dissimilar meshes. For more information, see Mapping Thermal and Magnetic Loads.

Conversion Limitations

When converting results values between dissimilar meshes, global conservation of the net flux is ensured provided that the model domain in the heat transfer, coupled temperature-displacement, or stress/displacement analysis matches the model domain in the time-harmonic eddy current analysis. The conservative mapping algorithm used in the abaqus emloads utility also provides a locally smooth distribution of point flux values (either body force or concentrated heat flux) in cases where the mesh in the time-harmonic eddy current analysis is finer than the “target” representative mesh. In situations where this is not the case and the “target” representative mesh is finer or of similar size to the mesh in the time-harmonic eddy current analysis, you may observe nodal locations with zero converted flux values. In these cases you will still observe global conservation of the flux, but your solution may be adversely affected locally. You can correct for these situations by always performing the time-harmonic eddy current analysis with a finer mesh.

Transferring Nodal Loads from the Output Database to Concentrated Loads

To define loads in a heat transfer, coupled temperature-displacement, or stress/displacement analysis, you can read nodal concentrated heat fluxes and point loads from the output database (.odb) file created by the abaqus emloads utility.

Input File Template

In this example heat flux values are stored in the output database from a time-harmonic eddy current analysis. These values, after conversion to point heat fluxes, are read into a subsequent analysis as a concentrated flux.

The following template shows the input for the time-harmonic eddy current analysis electromagnetic.inp:

HEADING
…
ELEMENT, TYPE=EMC3D8
(Choose the electromagnetic element type)
…
STEP
ELECTROMAGNETIC, LOW FREQUENCY, TIME HARMONIC
…
Apply loads and boundary conditions
…
** Write element Joule heat dissipation results to the output
** database file, electromagnetic.odb
OUTPUT, FIELD
ELEMENT OUTPUT, ELSET=CONDUCTOR
 EMJH
END STEP

The following template shows the input for the heat transfer analysis, heattransfer.inp, which refers to an output database, pointflux.odb, created using the abaqus emloads utility, and which has mapped quantities from the results of the time-harmonic eddy current analysis, stored in electromagnetic.odb:

HEADING
…
ELEMENT, TYPE=DC3D8
(Choose the heat transfer continuum element type)
…
STEP
HEAT TRANSFER, STEADY STATE
…
Apply heat transfer loads and boundary conditions
…
CFLUX, FILE=pointflux.odb
Read in all nodal heat flux values from the output database and apply as concentrated nodal fluxes 
…
END STEP