Mechanical supports the following capabilities when used in a System Coupling analysis:
Data exchange across the fluid-solid interface. The fluid-solid interface defines the interface between the fluid in the coupled participant system (for example, Fluent) and the solid in the Mechanical system. This interface is defined on regions in the Mechanical model (see Fluid Solid Interface).
Thermal-fluid-structural coupling between Mechanical and another participant system (for example, Fluent) is supported as an expert option, and requires the use of appropriate coupled field elements (SOLID226 and SOLID227). See Thermal-Fluid-Structural Analyses using System Coupling for details about how to set up this type of analysis.
Shared memory parallel mode. Note that convergence and therefore results will change between repeated runs of Mechanical in shared memory parallel mode. These changes will occur even if no setup changes were applied. The changes in the coupled analysis’ convergence and results are due to the segregated solution algorithm used and the inherent sensitivity of the coupled physics problems being solved.
Distributed parallel mode. Note that in order to run Mechanical in distributed parallel mode from within the Workbench interface, the working directory must be a shared network directory with the same path for all computer servers. Alternatively, the analysis can run in different working directories on all servers if Mechanical is run as a System Coupling Participant from the command line. For more information, see Running Mechanical as a System Coupling Participant from the Command Line.
SOLID and SHELL elements. For a complete list of elements, see Load Transfer Coupled Analysis - Workbench: System Coupling in the Mechanical APDL Coupled-Field Analysis Guide.
Structural convergence information and Result Tracker information are provided to the System Coupling system for display in System Coupling Chart.
When using the Result Tracker in a System Coupling analysis, note that Kinetic Energy and Stiffness Energy are only computed at the end of a coupling step, and values of zero are reported for the intermediate coupling iterations. The Kinetic Energy and Stiffness Energy values reported in System Coupling are lagged, so the value reported at the start of a coupling step is actually the value corresponding to the end of the previous coupling step. The value corresponding to the last coupling step will not be reported in System Coupling.
Data transfer regions are the regions upon which the Fluid Solid Interface condition is applied. In a coupled analysis, at each data transfer region, only one type of variable can be sent, and one type of variable received.
In a coupled structural analysis, force and displacement can be transferred at data transfer regions.
In a coupled thermal analysis, heat transfer coefficients and near wall temperatures, temperatures, and heat flows can be transferred at data transfer regions.
See Variables Available for System Coupling for more information about the variables transferred.
Note the following limitations when using Mechanical in a System Coupling analysis:
System Coupling requires participants to use 3D meshes, with data transfer regions consisting of element faces within the 3D mesh. Data transfer regions cannot exist in 2D meshes (where the data transfer would be a line/curve). Line elements such as BEAM elements in Mechanical cannot form Data Transfer regions, but may be included elsewhere in the Mechanical model.
In a System Coupling setup, if you apply an external force or external heat flow on the same region as a Fluid-Structure Interaction interface, this external variable will not be acknowledged by the Mechanical APDL solver.
When Mechanical participates in a System Coupling analysis only one load step can be defined in Mechanical. Loads can still vary as a function of time within this load step. Other operations that would normally require multiple load steps will require a System Coupling restart to be performed. For example, a pre-stressed analysis can be performed by executing a System Coupling simulation using the pre-stressing load conditions in Mechanical, then continuing the analysis by restarting System Coupling after making the necessary changes in Mechanical.
Note that the internally computed contact damping is a function of the total number of substeps. The internal damping is reduced in subsequent substeps within a load step, and very little damping is applied in the last substep. Therefore, the solution convergence pattern is different when solving a contact analysis that has only one substep (or a few substeps) per load step compared to an analysis having multiple substeps per load step. Often times, the solution fails to converge if a small number of substeps is used per load step. You can specify absolute damping coefficients to overwrite internal damping values by inserting a Command object under the Contact Region and setting appropriate values for the real constants, FDMN and FDMT.
The Save Project Before Solution and Save Project After Solution properties of the Project object are not supported if you are using the Workbench System Coupling component system in combination with your Mechanical analysis.
When transferring data to or from a wall boundary in a sliding mesh zone, you must make sure that Mechanical does not rotate the mesh. You can accomplish this by using a Rotational Velocity. For information about sliding meshes in ANSYS Fluent, see the Using Sliding Meshes Help in the Fluent User's Guide.