김경종
15 KiB
Executing the coupled analysis
You execute the co-simulation interactively in Abaqus/CAE or from the command line, as described in “Executing a co-simulation,” Section 17.3.4. By default, when coupling Abaqus/CFD to Abaqus/Explicit, the Abaqus/Explicit packager and analysis are both run in single precision.
Limitations
The following limitations apply to Abaqus/CFD to Abaqus/Standard or to Abaqus/Explicit co-simulation in addition to the limitations discussed in “Preparing an Abaqus analysis for co-simulation,” Section 17.2.1.
General limitation
Only a single region can be defined as the interface region; multiple interface regions are not supported.
Abaqus/Standard and Abaqus/Explicit analysis limitations
The following Abaqus/Standard and Abaqus/Explicit elements cannot be used in a co-simulation with Abaqus/CFD:
• Axisymmetric elements with twist degrees of freedom (the CGAX element family)
• Axisymmetric solid elements with asymmetric deformation (the CAXA element family)
• Generalized plane strain elements (the CPEG element family)
• Coupled pore pressure-displacement elements
• Acoustic elements
• Piezoelectric elements
17.3.3 ELECTROMAGNETIC-TO-STRUCTURAL AND ELECTROMAGNETIC-TO-THERMAL CO-SIMULATION
Product: Abaqus/Standard
References
• “Co-simulation: overview,” Section 17.1.1
• “Preparing an Abaqus analysis for co-simulation,” Section 17.2.1
• *CO-SIMULATION
Overview
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.
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:
• “Static stress analysis,” Section 6.2.2
• “Implicit dynamic analysis using direct integration,” Section 6.3.2
• “Uncoupled heat transfer analysis,” Section 6.5.2
• “Eddy current analysis,” Section 6.7.5
The following Abaqus/Standard analysis procedures can be used for electromagnetic-to-thermal co-simulation:
• “Uncoupled heat transfer analysis,” Section 6.5.2
• “Eddy current analysis,” Section 6.7.5
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” in “Preparing an Abaqus analysis for co-simulation,” Section 17.2.1, 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 17.3.3–1 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 17.3.3–1 Templates for electromagnetic co-simulation.
| Electromagnetic to transient heat transfer co-simulation | Coupling scheme:Electromagnetic analysis leadsHeat transfer analysis defines the coupling step size |
| template_em_std_export | |
| Example file:exa_em_std_export | |
| Coupling scheme:Electromagnetic analysis leadsAllow heat transfer analysis to subcycle | |
| template_em_std_fixed | |
| Example file:exa_em_std_fixed | |
| Coupling scheme:Electromagnetic analysis leadsHeat transfer analysis defines the coupling step sizeIterative coupling | |
| template_em_std_iterative | |
| Example file:exa_em_std_iterative | |
| Electromagnetic to Abaqus/Standard stress/displacement co-simulation | Coupling scheme:Electromagnetic analysis leadsStep size is determined based on the minimum suggested step size of the electromagnetic and Abaqus/Standard stress/displacement analyses.Either analysis can subcycleBody 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 master 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” in “Preparing an Abaqus analysis for co-simulation,” Section 17.2.1.
Executing the coupled analysis
You execute the co-simulation from the command line, as described in “Executing a co-simulation,” Section 17.3.4.
Limitations
The limitations discussed in “Preparing an Abaqus analysis for co-simulation,” Section 17.2.1, apply to electromagnetic-to-structural and electromagnetic-to-thermal co-simulation.
17.3.4 EXECUTING A CO-SIMULATION
Products: Abaqus/Standard Abaqus/Explicit Abaqus/CFD Abaqus/CAE
References
• “Abaqus/Standard, Abaqus/Explicit, Abaqus/CFD, AND FMU co-simulation execution,” Section 3.2.4
• “Understanding co-executions,” Section 19.4 of the Abaqus/CAE User’s Guide
Overview
You can execute the following types of co-simulations from the command line:
• Structural-to-structural
• Fluid-to-structural
• Conjugate heat transfer
• Electromagnetic-to-structural
• Electromagnetic-to-thermal
You can also execute structural-to-structural, fluid-to-structural, and conjugate heat transfer co-simulations in Abaqus/CAE.
Executing a co-simulation from Abaqus/CAE
You can execute the coupled analysis interactively in Abaqus/CAE as described in “Understanding co-executions,” Section 19.4 of the Abaqus/CAE User’s Guide. You are not required to create a configuration file; Abaqus/CAE creates the file automatically.
Abaqus/CAE Usage: Job module:
Co-execution→Create: select the Abaqus/Standard model and the
Abaqus/Explicit model; Communication time out: timeout-value
Co-execution→Manager: Submit
Executing a co-simulation from the command line
You execute the Abaqus jobs as described in “Abaqus/Standard, Abaqus/Explicit, Abaqus/CFD, AND FMU co-simulation execution,” Section 3.2.4.
Command usage example
Use the following command to submit a co-simulation between two Abaqus analyses, “job-1” and “job-2”:
abaqus cosimulation cosimjob=beam job=job-1,job-2 configure=config
Considerations for using the timeout parameter
The timeout execution parameter specifies the amount of time in seconds that each analysis waits to receive the co-simulation message expected from the other analysis that is running. The default timeout value is 60 minutes when submitting jobs using the command line options and 10 minutes when executing the jobs in Abaqus/CAE. When the timeout period is large compared to typical analysis increment wallclock times, you have greater flexibility in starting jobs and performing operations that precede the co-simulation analysis step. Examples where this flexibility is needed include: job submission using queues, analyses where steps that precede the co-simulation step have long run times, and cases where one job is resubmitted because of an input error. However, a large timeout period can cause problems when one of the co-simulation jobs fails (for reasons such as convergence issues or availability of computer resources) before the initial co-simulation communication is established. In these cases you may prefer to terminate the job left running rather than have it wait the entire timeout period.
Limitations
Electromagnetic-to-structural and electromagnetic-to-thermal co-simulations are not supported in Abaqus/CAE.