Products: Abaqus/Standard Abaqus/Explicit Abaqus/CFD Abaqus/CAE
“Preparing an Abaqus/Standard or Abaqus/Explicit analysis for co-simulation,” Section 14.1.2
“Preparing an Abaqus/CFD analysis for co-simulation,” Section 14.1.3
Chapter 25, “Co-simulations,” of the Abaqus/CAE User's Manual
This section discusses analysis setup and execution details specific to Abaqus/CFD to Abaqus/Standard or Abaqus/Explicit co-simulation for fluid-structure interaction and conjugate heat transfer. In addition to defining the individual analysis models and procedures and identifying matching interface regions as described in “Preparing an Abaqus/Standard or Abaqus/Explicit analysis for co-simulation,” Section 14.1.2, and “Preparing an Abaqus/CFD analysis for co-simulation,” Section 14.1.3, you must specify the co-simulation controls that define the coupling and rendezvousing scheme. These specifications complete the model setup and allow you to execute the coupled analysis. For conjugate heat transfer, only Abaqus/CFD to Abaqus/Standard co-simulation is available.
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.
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. The coupling step size is the period between two consecutive co-simulation data exchanges. To determine the coupling step size, each analysis suggests a coupling step size, which is the next increment suggested by its automatic incrementation scheme.
When coupling Abaqus/Standard and Abaqus/CFD, the minimum of the suggested coupling step sizes is used as the coupling step size. When coupling Abaqus/Explicit and Abaqus/CFD, Abaqus/Explicit imports the coupling step size from Abaqus/CFD and Abaqus/CFD exports the coupling step to Abaqus/Explicit.
Abaqus/CFD always uses a time increment size that is the same as the coupling step size (no subcycling), while Abaqus/Standard and Abaqus/Explicit are allowed to subcycle.
| Input File Usage: | You can generate the input file using Abaqus/CAE. |
| Abaqus/CAE Usage: | Interaction module: Create Interaction: Fluid-Structure Co-simulation boundary |
You can execute the coupled analysis interactively in Abaqus/CAE. Alternatively, you can write the input files for each job from Abaqus/CAE and submit the jobs using the Abaqus commands. Submitting jobs this way provides additional flexibility; for example, you can use job submission queuing systems that are not configured for your installation of Abaqus/CAE.
You execute the Abaqus jobs in Abaqus/CAE as described in “Understanding co-executions,” Section 18.4 of the Abaqus/CAE User's Manual.
| Input File Usage: | You can generate the input file using Abaqus/CAE. |
| Abaqus/CAE Usage: | Job module: |
You execute the Abaqus/CFD and Abaqus/Standard or Abaqus/Explicit jobs as described in “Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD execution,” Section 3.2.2, using the listenerport, remoteconnections, and, optionally, the timeout execution parameters to control the identification of one Abaqus analysis to the other.
The timeout parameter specifies the amount of time that each analysis waits to receive the co-simulation message expected from the other analysis that is running. The default timeout value when executing the jobs in Abaqus/CAE is 10 minutes; the default timeout value when submitting jobs using the command line options is 3600 seconds. 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.
| Input File Usage: | You can generate the input file using Abaqus/CAE. |
| Abaqus/CAE Usage: | Job module: Co-execution |
Use the following command to run an Abaqus/Standard or Abaqus/Explicit job called “solid” running on a machine called “abc” that will establish a co-simulation connection to an Abaqus/CFD job called “fluid” running on a machine called “xyz.” Job “solid” will listen to job “fluid” on port 48000, and job “fluid” will listen to job “solid” on port 48001:
abaqus job=solid listenerport=48000 remoteconnections=xyz:48001Use the following command to run an Abaqus/CFD job called “fluid” that communicates to the above described job “solid” and to specify a timeout value:
abaqus job=fluid listenerport=48001 remoteconnections=abc:48000 timeout=3600
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/Standard or Abaqus/Explicit analysis for co-simulation,” Section 14.1.2, and “Preparing an Abaqus/CFD analysis for co-simulation,” Section 14.1.3.
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
