Using MFX, data are transferred throughout the fluid-solid interaction analysis. The points at which data are transferred are called synchronization points. Data can be sent or received only at a synchronization point, as shown in Figure 4.1: "MFX Method Data Communication".

At each synchronization point, the ANSYS and CFX codes shift their client privileges sequentially: the client code queries the server code to get information and the server code serves data until it receives a command to get client privileges or is asked to go to the next synchronization point. For the load transfer, each code gets all interface boundary conditions from the other code before solving. Depending on whether the field solvers are being solved simultaneously (in the same group defined by the MFPSIMUL command) or sequentially, the codes will serve loads before or after solving, respectively.

At the synchronization point, the ANSYS and CFX codes transfer loads across the fluid-solid interface to each other. The MFX solver automatically detects whether the meshes on each side of the interface are the same or not. Two interpolations methods, profile preserving and conservative, are available. The profile preserving interpolation used in MFX is the same as that in MFS (see Load Transfer in Chapter 3: "The ANSYS Multi-field (TM) Solver - MFS Single-Code Coupling" for more information.

The conservative interpolation in MFX replaces the globally conservative interpolation used in MFS. It differs from the other two interpolations in the fundamental interpolation technology:

In the conservative interpolation, each element face is first divided into n number of IP faces, where n is the number of nodes on the face. The three-dimensional IP faces are then converted onto a two-dimensional polygon made up of rows and columns of dots called pixels. By default, these pixels have a resolution of 100 x 100; use the MFCI command to increase the resolution and improve the accuracy of the algorithm. Be aware that increasing the resolution will also increase the time and memory requirements. Next, the converted polygons on the sending side are intersected with the IP polygons on the receiving side using the pixel images. The polygon intersection creates many overlapped areas, called control surfaces. Those control surfaces are then used to transfer loads between the two sides. See Three-dimensional Navier Stokes predictions of steady state rotor / stator interaction with pitch change, 3rd Annual conference of the CFD, Society of Canada, Banff, Alberta, Canada, Advanced Scientific Computing Ltd. By P.F. Galpin, R.B. Broberg and B.R. Hutchinson, June 25-27, 1995, for a more detailed description of the algorithm.

The conservative interpolation can generally preserve local distributions and thus can also be used to interpolate the mesh displacement and temperature. The displacement and temperature variables are interpolated in an area-weighted manner from all IP faces on the sending side that intersect with the nodal IP areas surrounding the given node; therefore, the conservative interpolation can smooth any numerical oscillations present in the local profiles from the sending side. However, profiles of local distributions may not be preserved to the same degree as the profile preserving interpolation in certain special problems.

If the surface on the sending side matches the surface on the receiving side, then the total forces and heat flows are first transferred to the control surfaces and then redistributed to the faces on the receiving side without any loss. Therefore, the overall load transfer is conservative, both globally and locally at the element level. The conservation property is maintained regardless of the mesh shape and size, grid topology, and face distribution across the interface.

If the surface on the sending side does not match the surface on the receiving side, then the total force and heat flow on the unmapped region of the sending side will not be transferred onto the control surfaces, and total force and heat flow on the receiving side will not be equal to that on the sending side. The overall imbalance is exactly the amount of total force and heat flow in the unmapped region on the sending side.

On the unmapped region of the receiving side, however, the conservative interpolation will set values of all loads in this region to zero. Therefore, the ANSYS CFX solver disregards values of temperature and mesh displacement on the unmapped region of the receiving side. Instead, it implements an adiabatic boundary condition for temperature and an unspecified boundary condition for mesh displacement in this unmapped region.

MFX supports all ANSYS 3-D elements, including structural (solid and shell), thermal, electromagnetic, and coupled-field elements. However, only those elements that support the SF family of commands (SF, SFA, SFE, or SFL) for surface load transfer with the field surface interface (FSIN) flag can participate in the load transfer. You need to flag these elements at the surface (FSIN) for load transfer to other fields during the analysis. Other element types can be used in the analysis, but they will not participate in load transfer and should not be located on the interface. See Table 3.2: "Structural and Thermal Elements" and Table 3.3: "Electromagnetic, Fluid, and Coupled-Field Elements" in "The ANSYS Multi-field (TM) Solver - MFS Single-Code Coupling" for a list of element types that support the SF family of commands for surface load transfer with the field surface interface (FSIN) flag. MFX supports only mechanical and thermal load transfer between fields.

The solution process for MFX is shown in the figure below. The ANSYS code acts as the master and reads all MFX commands, does the mapping, and serves the time step and stagger loop controls to the CFX slave. The MFANALYSIS command activates a master multi-field solution. The solution loop consists of two loops: the multi-field time loop and the multi-field stagger loop.

The ANSYS field solver supports transient and static analyses. CFX supports only a transient analysis. If you want a static solution, running a static analysis on ANSYS will help CFX to reach a solution more quickly.

The time loop corresponds to the time step loop of the multi-field analysis, set with the MFTIME command. Use the MFDTIME command to specify time step size.

Within each time step is the stagger loop. The stagger loop allows for implicit coupling of the fields in the MFX solution. The number of stagger iterations applies to each time step in the MFX analysis. Within each step in the time step loop, the field solutions are repeated in the stagger loop until convergence. The number of iterations executed within the stagger loop is determined by the convergence of the loads transfer between fields or the maximum number of stagger iterations specified by the MFITER command. For a transient analysis performed in CFX, the stagger iteration contains many CFX coefficient iterations, which loop until convergence or until the maximum number of coefficient iterations is reached. Load transfers between fields occur at each stagger loop. Global convergence is checked after the load transfer. If global convergence of the load transfer is not achieved, another stagger loop is performed.

Use the MFLCOMM command to specify surface load transfer between field solvers. The meshes used in the individual field solvers can be dissimilar across the interface. Before solving a given field, all necessary loads are collected from the other field solver. Loads are transferred either before or after solution of the field solver, depending on whether the field solver groups are set to solve sequentially or simultaneously.