Double-Precision Solver
System Coupling cases may benefit from the use of Fluent’s double-precision solver. For coupling cases with moving and deforming meshes (MDM), it is a best practice to use Fluent’s double-precision solver. For more information about Fluent’s single- and double-precision solvers, see Single-Precision and Double-Precision Solvers in the Fluent Getting Started Guide.
In the Fluent Launcher, select Double Precision to use Fluent’s double-precision solver.
Dynamic Mesh
The System Coupling option must be selected on the desired moving and deforming wall boundaries in order to obtain displacements from other co-simulation participants taking part in the coupled analysis.
Make sure the appropriate solution stabilization options are selected in the Solver Options tab for the System Coupling boundary zone (and possibly other boundary zones nearby). Solution stabilization should be activated if you find that the Fluent solution is particularly sensitive to the data obtained through system couplings. For example, it is often beneficial for FSI problems in which the fluid is incompressible.
Heat Transfer
The via System Coupling option must be selected on the desired wall boundaries in order to obtain heat transfer data (temperature or heat flow) from other participants taking part in the coupled analysis.
Run Calculation
When running as part of a transient coupled analysis, the step size for and duration of the analysis are controlled by the System Coupling service.
The Time Step Size(s) specified in the Fluent setup is currently ignored; the Fluent solution will be advanced using the time step size specified as part of the System Coupling setup.
The Number of Time Steps is also ignored.
The specified Max Iterations/Time Step corresponds to the maximum number of nonlinear solver iterations performed per coupling iteration.
For steady-state, system–coupled Fluent analyses, the
number of iterations specified in Fluent is equal to the maximum
number of solver iterations solved per coupling iteration in a coupling
step. Prior to ANSYS FLUENT 14.5, the number of iterations specified
in Fluent was equal to the solver iterations solved in a coupling
step and was divided equally between the coupling iterations in a
coupling step. You can recover the previous behavior by using the
following command: (rpsetvar ’sc/steady/default-iteration-method?
#f).
For pseudo-transient cases, refer to Performing Pseudo Transient Calculations in the Fluent User's Guide.
For steady-state dynamic mesh applications, refer to Steady-State Dynamic Mesh Applications in the Fluent User's Guide.