Electromagnetic-to-Structural and Electromagnetic-to-Thermal Co-Simulation

This section discusses analysis setup and execution details specific to electromagnetic-to-structural and electromagnetic-to-thermal co-simulation using Abaqus/Standard procedures. Co-simulation between a time-harmonic or transient electromagnetic analysis and a static, transient implicit dynamic, coupled temperature-displacement, or transient heat transfer analysis is supported.

An electromagnetic to a heat transfer co-simulation analysis is useful for applications such as induction heating, which involves two-way coupling: the Joule heat production from the electromagnetic analysis drives a heat transfer analysis and determines the temperature distribution, while the temperature distribution, in turn, affects the electromagnetic fields through temperature-dependent material properties (such as electrical conductivity and magnetic permeability). For electromagnetic-to-thermal coupling, co-simulation between a time-harmonic or transient electromagnetic analysis and a transient heat transfer analysis is supported.

An electromagnetic to transient implicit dynamic analysis is useful for applications such as electromagnetic forming, where the Lorentz body forces from an electromagnetic analysis drive a transient dynamic analysis. Co-simulation between a transient electromagnetic analysis and a static or transient implicit dynamic analysis is supported. However, the coupling is only one way; that is, the effects of deformation of parts of the domain (metal work piece, in this case) on the electromagnetic fields is not accounted for. Hence, such analysis should be used only when the effects of deformation on the electromagnetic fields are relatively small.

This page discusses:

Identifying the Abaqus Step for the Co-Simulation Analysis
Identifying the Co-Simulation Interface Region
Identifying the Fields Exchanged across a Co-Simulation Interface
Defining the Rendezvousing Scheme
Executing the Coupled Analysis
Limitations

Identifying the Abaqus Step for the Co-Simulation Analysis

The following Abaqus/Standard analysis procedures can be used for an electromagnetic-to-structural co-simulation:

The following Abaqus/Standard analysis procedures can be used for electromagnetic-to-thermal co-simulation:

Input File Usage

Use the following option within a step definition for an Abaqus/Standard to Abaqus/Standard co-simulation:

CO-SIMULATION, PROGRAM=MULTIPHYSICS

Identifying the Co-Simulation Interface Region

Interaction between the electromagnetic and structural models occurs through a common volume interface region.

You must specify the volume interface region using element sets between the Abaqus/Standard analyses. You must be consistent in your region definition in both the Abaqus/Standard simulations; in other words, you must define the same interface region in both the analyses.

You can have dissimilar meshes in regions shared in the two model definitions.

Input File Usage

Use the following option to define an element-based co-simulation region in an Abaqus/Standard model:

CO-SIMULATION REGION, TYPE=VOLUME
elset_A

Only one CO-SIMULATION REGION option can be defined in each Abaqus/Standard analysis. In addition, only one element set can be defined.

Identifying the Fields Exchanged across a Co-Simulation Interface

For Abaqus/Standard to Abaqus/Standard co-simulation, see the tables in Identifying the Fields Exchanged across a Co-Simulation Interface for lists of fields that are available for co-simulation exchange.

Defining the Rendezvousing Scheme

The SIMULIA Co-Simulation Engine configuration file is used to define the time incrementation process and the frequency of exchange between the two Abaqus/Standard analyses.

Predefined templates are available for commonly used coupling schemes. You can refer to these templates when you create your configuration files. This section describes the rendezvous scheme settings and the predefined configuration file templates.

Time Incrementation Scheme

You can force the two transient Abaqus/Standard analyses to use the same increment size, or you can allow the increment sizes to differ (subcycling). The time incrementation scheme that you choose for coupling affects the solution computational cost and accuracy but not the solution stability. When using the subcycling method, this data exchange does not represent a constraint on Abaqus/Standard incrementation; the Abaqus/Standard analysis advances in time using its normal time incrementation logic but performs data exchanges as needed at the coupling step size intervals.

A time-harmonic electromagnetic procedure is defined in the frequency domain and does not have a solution time-scale associated with it in the sense that a transient analysis does. It is convenient to introduce a pseudo-solution time scale that is associated with the time-harmonic electromagnetic procedure involved in a co-simulation analysis, thereby facilitating coupling with a transient analysis at certain solution time intervals of the latter analysis. The pseudo-time scale of the time-harmonic electromagnetic analysis follows the solution time scale in the transient heat transfer analysis and is reset in every coupling step in a manner described below.

Defining the Coupling Scheme

The sequential explicit coupling scheme (also referred to as the Gauss-Seidel coupling algorithm) and the iterative coupling scheme are available for electromagnetic-to-structural and electromagnetic-to-thermal co-simulation. The electromagnetic analysis must always lead the co-simulation, while the heat transfer or the stress analysis always lags the co-simulation. All the predefined templates are set up with the above lead-lag sequence.

Coupling Step Size

The coupling step size is the period between two consecutive co-simulation data exchanges between the two Abaqus/Standard analyses. For transient electromagnetic to transient heat transfer or transient implicit dynamic co-simulation, the coupling step size can be specified to be equal to the minimum of the time step sizes determined by the automatic time incrementation schemes of the individual analyses or to a constant user-defined value.

When the leading electromagnetic analysis is time harmonic, the coupling step size can be specified to be equal to the time step size of the lagging transient heat transfer or implicit dynamic analysis or to a constant user-defined value. In the latter case, the time-harmonic electromagnetic analysis would solve for the fields at the end of each successive constant user-defined coupling step size, while the lagging heat transfer or stress analysis would typically subcycle until the target coupling step time is reached.

For iterative coupling, the two analyses must be coupled at the end of each time increment, and subcycling should not be used. If subcycling is used in this situation, the exchanged updated solutions during the iterations will be utilized only for the very last increment and the cumulative effect of the updates over the previous increments (between the last coupling and the current coupling) will be lost.

Creating a Configuration File

You can use predefined templates to create the configuration file for the coupling schemes described above. Table 1 describes the predefined templates available for electromagnetic to transient heat transfer analyses and for electromagnetic to stress-displacement analyses and lists example configuration files that you can review.

Table 1. Templates for electromagnetic co-simulation.
Electromagnetic to transient heat transfer co-simulation	Coupling scheme: Electromagnetic analysis leads Heat transfer analysis defines the coupling step size
	template_em_std_export
	Example file: exa_em_std_export
	Coupling scheme: Electromagnetic analysis leads Allow heat transfer analysis to subcycle
	template_em_std_fixed
	Example file: exa_em_std_fixed
	Coupling scheme: Electromagnetic analysis leads Heat transfer analysis defines the coupling step size Iterative coupling
	template_em_std_iterative
	Example file: exa_em_std_iterative
Electromagnetic to Abaqus/Standard stress/displacement co-simulation	Coupling scheme: Electromagnetic analysis leads Step size is determined based on the minimum suggested step size of the electromagnetic and Abaqus/Standard stress/displacement analyses. Either analysis can subcycle Body forces are transferred from the electromagnetic to Abaqus/Standard stress/displacement analysis. No other co-simulation transfer occurs.
	template_em_std_force_oneway
	Example file: exa_em_std_force_oneway

To obtain an example configuration file, you can use the abaqus fetch utility. For example, to obtain the example for which the heat transfer analysis serves as the main analysis in determining the coupling step size, use the following command:

abaqus fetch job=exa_em_std_export

The example file exa_em_std_export.xml is shown below.

<?xml version="1.0" encoding="utf-8"?>
<CoupledMultiphysicsSimulation>
   <template_em_std_export>
      <EM_Job>em_job_name</EM_Job>
      <HeatTransfer_Job>ht_job_name</HeatTransfer_Job>
      <duration>duration_value</duration>
   </template_em_std_export>
</CoupledMultiphysicsSimulation>

In certain cases you may need to use co-simulation configuration features that are not described in the predefined templates. For example, you may wish to change the dissimilar mesh mapping search tolerances; these tolerances are available generally in the configuration file but are not described in the predefined templates. For these cases, you must create an elaborated configuration file; for more information, see Using Elaborated Configuration Files.

Executing the Coupled Analysis

You execute the co-simulation from the command line, as described in Executing a Co-Simulation.

Limitations

The limitations discussed in Preparing an Abaqus Analysis for Co-Simulation apply to electromagnetic-to-structural and electromagnetic-to-thermal co-simulation.