Mechanical supports the following capabilities when used in a System Coupling analysis:
Data exchange across System Coupling Region interfaces defined on regions in the Mechanical model. This boundary condition defines the interface between the fluid in the coupled participant system (for example, Fluent) and the solid in the Mechanical system.
Data transfer regions are the regions upon which the System Coupling Region condition is applied. In a coupled analysis, at each data transfer region, the following variables can be sent and received:
In a coupled structural analysis, Force and Displacement can be transferred at data transfer regions.
Both Force and Force Density transfers are available. They are very similar, except that the Force Density variable uses follower effects within the Mechanical solution: as the structural geometry deforms within a time step, the Force rotates along with it. This can lead to a more robust solution, especially for soft materials such as hyperelastic solids.
When the solver receiving the motion (such as Fluent) solves before or simultaneously with the solver sending the motion (such as Mechanical), then the Incremental Displacement transferred during the first coupling iteration of each coupling step is identically zero.
In a coupled thermal analysis, Heat Transfer Coefficients and Near Wall Temperatures, Temperatures, and Heat Flows can be transferred at data transfer regions.
Heat Transfer Coefficient is also known as "convection coefficient."
Near Wall Temperature is also known as "bulk temperature," or "ambient temperature."
In a coupled thermal-structural analysis, Mechanical can send Displacements along with only one Temperature or Heat Flow condition, and can in turn receive a Force load and either one Temperature or Heat Flow, or a combined Heat Transfer Coefficient and Reference Temperature.
In a coupled thermal-structural-fluid analysis (performed using a coupled field system), both Displacement and thermal data can be transferred on data transfer regions.
For a listing of Mechanical's data transfer variables, see Variables Available for System Coupling.
Surface and volume meshes that include higher-order elements.
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 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 coupling participant from one of System Coupling's user interfaces. For more information, see Running Mechanical as a Coupling Participant in System Coupling's GUI or CLI.
SOLID and SHELL elements. For a complete list of elements, see Load-Transfer Coupled Analysis -- Workbench: System Coupling in the Coupled-Field Analysis Guide.
Structural convergence information and Result Tracker information are provided to System Coupling for display in the charts generated by System Coupling in Workbench.
When using the Result Tracker in a System Coupling in Workbench analysis, note that Kinetic Energy and Stiffness Energy values 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.
Custom restart files are available when using System Coupling's GUI or CLI. These files allow for the insertion of pre-solve command snippets into Mechanical's restart file. Mechanical APDL commands that are supported for coupled analysis restarts (such as TIMINT) may be used.
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 System Coupling Region interface, this external variable will be ignored by the Mechanical APDL solver.
Transfers of Force Density are not supported for:
Cases where Mechanical uses shell elements and Force Density is transferred to both sides of any shell.
Execution using System Coupling in Workbench. To make the FDNS input variable available in a coupled analysis created in Workbench, export the coupling setup so the analysis can be executed in System Coupling's GUI or CLI. For details, see Exporting a System Coupling Setup and Running an Exported System Coupling Setup in the System Coupling User's Guide.
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.
Mechanical restarts are not supported for the transfer of thermal variables.
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. In some cases, the solution may fail 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.
If you are using a System Coupling in Workbench component system in combination with your Mechanical analysis, the Save Project Before Solution and Save Project After Solution properties of the Project object are not supported.
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 documentation in the Fluent User's Guide.