Products: Abaqus/Standard Abaqus/Explicit Abaqus/CFD Abaqus/CAE
This section discusses analysis setup, execution, and limitation details specific to Abaqus/CFD to Abaqus/Standard or to Abaqus/Explicit co-simulation for fluid-structure interaction and conjugate heat transfer.
Refer to “Conjugate heat transfer analysis of a component-mounted electronic circuit board,” Section 6.1.1 of the Abaqus Example Problems Manual, for an example of Abaqus/CFD to Abaqus/Standard co-simulation.
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 |
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 |
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.
Co-simulation controls are used to control the time incrementation process and the frequency of exchange between the two Abaqus analyses. These controls are specified automatically in Abaqus/CAE.
| Input File Usage: | Use both of the following options to specify co-simulation controls: |
*CO-SIMULATION, PROGRAM=MULTIPHYSICS, CONTROLS=name *CO-SIMULATION CONTROLS, NAME=name |
| Abaqus/CAE Usage: | Interaction module: Create Interaction: Fluid-Structure Co-simulation boundary |
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. By default, 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.
| Input File Usage: | Use the following option to specify that the analysis leads the co-simulation: |
*CO-SIMULATION CONTROLS, SCHEME MODIFIER=LEAD Use the following option to specify that the analysis lags the co-simulation: *CO-SIMULATION CONTROLS, SCHEME MODIFIER=LAG |
| Abaqus/CAE Usage: | The coupling scheme is specified automatically in Abaqus/CAE when you define a fluid-structure co-simulation interaction. |
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.
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. By default, for FSI and CHT analyses that couple Abaqus/CFD and Abaqus/Standard, there is no subcycling involved because the coupling step size is based on the minimum of the individual analyses. For FSI analyses that couple Abaqus/CFD and Abaqus/Explicit, Abaqus/Explicit typically uses subcycling while Abaqus/CFD uses lockstep behavior.
| Input File Usage: | Use the following option to allow the analysis to subcycle: |
*CO-SIMULATION CONTROLS, TIME INCREMENTATION=SUBCYCLE Use the following option to force the analysis to use a single increment per coupling step: *CO-SIMULATION CONTROLS, TIME INCREMENTATION=LOCKSTEP |
| Abaqus/CAE Usage: | The time incrementation scheme is specified automatically in Abaqus/CAE when you define a fluid-structure co-simulation interaction. |
The Abaqus target times can be reached in an exact or loose manner. By default, Abaqus exchanges the data in an exact manner; that is, Abaqus temporarily reduces the time increment so that the solution exchange occurs exactly at the target time. When subcycling Abaqus may reach the target time in a loose manner; that is, when the current simulation time, t, is within half of an Abaqus increment size away from the target time,
| Input File Usage: | Use the following option to reach target times in an exact manner: |
*CO-SIMULATION CONTROLS, TIME MARKS=YES (default) Use the following option to reach target times in a loose manner: *CO-SIMULATION CONTROLS, TIME MARKS=NO |
| Abaqus/CAE Usage: | The manner is which target times are reached is specified automatically in Abaqus/CAE when you define a fluid-structure co-simulation interaction. |
You execute the Abaqus/CFD and Abaqus/Standard or Abaqus/Explicit jobs as described in “Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD co-simulation execution,” Section 3.2.4. By default, when coupling Abaqus/CFD to Abaqus/Explicit, the Abaqus/Explicit packager and analysis are both run in single precision.
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 Manual.
| Input File Usage: | Enter the following input on the command line: |
abaqus cosimulation cosimjob=cosim-job-name job=job-name-A,job-name-B |
| Abaqus/CAE Usage: | Job module: |
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 kill the job left running rather than have it wait the entire timeout period.
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.
An interface region can be used for fluid-structure interaction or conjugate heat transfer but not both.
Abaqus/Standard elements that have no equivalent degree-of-freedom counterpart in Abaqus/CFD cannot be connected to co-simulation region nodes. These elements include the following:
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
