17.3.2 Fluid-to-structural and conjugate heat transfer co-simulation
Products: Abaqus/Standard Abaqus/Explicit Abaqus/CFD Abaqus/CAE
Overview
This section discusses analysis setup, execution, and limitation details specific to fluid-to-structural co-simulation and conjugate heat transfer using Abaqus/CFD and Abaqus/Standard or Abaqus/Explicit.
Refer to “Conjugate heat transfer analysis of a component-mounted electronic circuit board,” Section 6.1.1 of the Abaqus Example Problems Guide, for an example of conjugate heat transfer.
Identifying the Abaqus step for the co-simulation analysis
The following Abaqus/CFD analysis procedure can be used for co-simulation with Abaqus/Standard or Abaqus/Explicit:
The following Abaqus/Standard analysis procedures can be used for co-simulation with Abaqus/CFD:The following Abaqus/Explicit analysis procedures can be used for co-simulation with Abaqus/CFD:| Input File Usage: | Use the following option within a step definition for an Abaqus/CFD to Abaqus/Standard or to Abaqus/Explicit co-simulation: |
*CO-SIMULATION, PROGRAM=MULTIPHYSICS |
| Abaqus/CAE Usage: | Use the following option for an Abaqus/CFD to Abaqus/Standard or to Abaqus/Explicit co-simulation: |
Interaction module: Create Interaction: Fluid-Structure Co-simulation boundary |
Identifying the co-simulation interface region
You specify an interface region using surfaces when coupling Abaqus/CFD to Abaqus/Standard or to Abaqus/Explicit. You must define an element-based surface, and you can specify only one surface to be used as the interface region in the analysis. You may have dissimilar meshes in regions shared in the model definitions.
| Input File Usage: | Use the following option to define an element-based surface as a co-simulation region: |
*CO-SIMULATION REGION, TYPE=SURFACE surface_A |
| Abaqus/CAE Usage: | Interaction module: Create Interaction: Fluid-Structure Co-simulation boundary: select surface region |
Identifying the fields exchanged across a co-simulation interface
For Abaqus/CFD to Abaqus/Standard or to Abaqus/Explicit 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. When using Abaqus/CAE, the fields exchanged are determined automatically by Abaqus/CAE.
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 analyses. Abaqus/CAE automatically creates and uses this configuration file. If you are not using Abaqus/CAE to perform the co-simulation, you must create the configuration file manually.
Predefined templates are available for commonly used coupling schemes. You refer to these templates when you create configuration files. This section describes the rendezvous scheme settings and predefined configuration file templates.
Defining the coupling scheme
The sequential explicit coupling scheme (also referred to as the Gauss-Seidel coupling algorithm) is the only coupling scheme available for Abaqus/CFD to Abaqus/Standard or to Abaqus/Explicit co-simulation. In all of the predefined templates, the Abaqus/CFD analysis lags the co-simulation and the Abaqus/Standard or Abaqus/Explicit analysis leads the co-simulation. For conjugate heat transfer, the Abaqus/CFD analysis can either lag or lead the co-simulation. For fluid-structure interaction, the Abaqus/CFD analysis must lag the co-simulation and the Abaqus/Standard or Abaqus/Explicit analysis must lead the co-simulation.
Coupling step size
The coupling step size is the period between two consecutive co-simulation data exchanges. The coupling step size is determined automatically based on the type of analysis and is used to obtain time-accurate solutions for the coupled physics problem. For fluid-structure interaction (FSI) and conjugate heat transfer (CHT) analyses that couple Abaqus/CFD and Abaqus/Standard, the coupling step size is the minimum of the time step sizes determined by the automatic time incrementation schemes of the individual analyses. For FSI problems that couple Abaqus/CFD and Abaqus/Explicit, Abaqus/Explicit imports the coupling step size from Abaqus/CFD; consequently, Abaqus/CFD exports the coupling step size to Abaqus/Explicit.
Time incrementation scheme
Depending on the type of analysis, Abaqus may either perform one increment (referred to as “lockstep”) or several increments (referred to as “subcycling”) per coupling step. For FSI analyses that couple Abaqus/CFD and Abaqus/Explicit, Abaqus/Explicit typically uses subcycling while Abaqus/CFD uses lockstep behavior.
Creating a configuration file
You can use predefined templates to create a configuration file for the coupling schemes described above. Table 17.3.2–1 describes the predefined templates available for fluid-to-structural co-simulation and conjugate heat transfer and lists example configuration files that you can review.
Table 17.3.2–1 Templates for fluid-to-structural co-simulation and conjugate heat transfer.
| Fluid-to-structural co-simulation: Abaqus/Standard and Abaqus/CFD | Coupling scheme:
|
| template_std_cfd_fsi | |
| Example file: exa_std_cfd_fsi | |
| Fluid-to-structural co-simulation: Abaqus/Explicit and Abaqus/CFD | Coupling scheme:
|
| template_xpl_cfd_fsi | |
| Example file: exa_xpl_cfd_fsi | |
| Conjugate heat transfer: Abaqus/Standard and Abaqus/CFD | Coupling scheme:
|
| template_std_cfd_cht | |
| Example file: exa_std_cfd_cht | |
| Conjugate heat transfer: Abaqus/Explicit and Abaqus/CFD | Coupling scheme:
|
| template_xpl_cfd_cht | |
| Example file: exa_xpl_cfd_cht |
To obtain an example configuration file, you can use the abaqus fetch utility. For example, to obtain the example for Abaqus/Standard to Abaqus/CFD conjugate heat transfer, use the following command:
abaqus fetch job=exa_std_cfd_chtThe example file exa_std_cfd_cht is shown below.
<?xml version="1.0" encoding="utf-8"?>
<CoupledMultiphysicsSimulation>
<template_std_cfd_cht>
<Standard_Job>standard_job_name</Standard_Job>
<Cfd_Job>cfd_job_name</Cfd_Job>
<duration>duration_value</duration>
</template_std_cfd_cht>
</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 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