The procedure for an MFX solution consists of the following steps:
To perform an MFX analysis, you must first create the ANSYS and CFX models (e.g., mesh, boundary conditions, analysis options, output options, etc.) For information on creating the ANSYS model, refer to the Structural Analysis Guide, the Thermal Analysis Guide, and the other ANSYS analysis guides. For information on creating the CFX model, see the discussion on Solver Modeling in the CFX documentation.
The next step is to flag field surfaces for load transfer. ANSYS surfaces are flagged by interface number and CFX surfaces are flagged by interface name. The ANSYS interface is defined by the SF family of commands (SF, SFA, or SFE) with the FSIN surface load label. The CFX interface is defined as a boundary condition with an option set to . Load transfer occurs between ANSYS and CFX field solvers on the flagged interface(s). Use the MFLCOMM command to specify the surface load transfer. You can specify multiple interface numbers or interface names in an MFX run by issuing multiple MFLCOMM commands.
Beam elements are not allowed on an ANSYS flagged interface. If the SF command with a FSIN load label is applied on node groups that are attached to underlying beam and solid or shell elements, the beam elements will also be incorrectly flagged as a load transfer interface. In such a case, use the SFE command to flag the solid or shell elements.
The procedure for setting up the master input consists of the following main steps:
The following table lists the steps to set up the global MFX controls. You must specify the solution order (MFSORDER); there is no default setting.
| Step | Command/Option | GUI Path |
|---|---|---|
| Turn on the ANSYS Multi-field solver. | MFANALYSIS |
|
| Set up the field solver groups for sequential or simultaneous solution. | MFPSIMUL |
|
| Specify the solution sequence. | MFSORDER |
|
Use the MFANALYSIS command to activate an ANSYS Multi-field solver analysis. Issue MFANALYSIS,OFF to deactivate the analysis (OFF is the default).
Use the MFPSIMUL command to specify groups of field solvers that you want to process simultaneously. For example, one group with both the ANSYS and CFX field solvers yields the following behavior: ANSYS requests its loads from CFX, CFX requests its loads from ANSYS, then both solvers execute simultaneously (see Figure 4.4: ANSYS and CFX Fields Solved Simultaneously). Two MFPSIMUL commands, each containing one field solver, are required to process and solve field solvers sequentially (see Figure 4.5: ANSYS and CFX Fields Solved Sequentially, ANSYS First).
Use the MFSORDER command to specify the order in which to process the groups of field solvers identified in the MFPSIMUL command(s).
Note: If you use the GUI to create the ANSYS input file, ANSYS will automatically use ANSYS as the ANSYS field solver name and CFX as the CFX field solver name.
If you are working interactively, ANSYS generates the MFPSIMUL and MFSORDER as shown in Figure 4.4: ANSYS and CFX Fields Solved Simultaneously and Figure 4.5: ANSYS and CFX Fields Solved Sequentially, ANSYS First, depending on whether you selected a simultaneous or sequential solution. You can specify the global relaxation factor (see MFRELAX,ALL,VALUE) at this point.
To set up a simultaneous solution, use the MFPSIMUL command once, with one group name and both field solver names. Again, use the MFSORDER command to specify the solution order.
To set up a sequential solution, use the MFPSIMUL command to set up two groups, each time with just one field. Then use the MFSORDER command to specify the solution order.
The MFPSIMUL and MFSORDER commands are used to optimize computing resource usage according to the nature of the physical coupling between the fields being solved.
Weakly coupled fields can often be solved simultaneously (i.e., via a single MFPSIMUL command). In this case, the overall simulation time may decrease because no field solver must wait for results/loads from another field solver. If the fields are too strongly coupled, however, this approach may also destabilize the solution process because less recent results/loads are applied in each field solver. Strongly coupled fields should be solved sequentially (i.e., via multiple MFPSIMUL commands), which ensures that the most recent results/loads from one field solver are applied to the other. Multiple stagger iterations are often required to obtain a fully implicit solution by the end of each multi-field time step (see MFITER).
In most simulations, the physical processes in one field solver will drive those in another field solver. In many FSI cases, for example, the forces generated by the fluid fields lead to strains in the solid field. In such cases, the MFSORDER command should specify that the 'driver' field solver (the fluid field solver in this case) be solved first.
MFX allows load transfer across flagged surfaces. Use the MFLCOMM command to set up the load transfer between the ANSYS and CFX codes. You must specify the load transfer information; there is no default setting.
| Step | Command/Option | GUI Path |
|---|---|---|
| Set up the load communication. | MFLCOMM |
|
Specify the names of field solvers sending and receiving quantities, the surface name or number, and the variable being transferred. The interpolation option -- Conservative or Profile Preserving (nonconservative) -- determines how loads are transferred across the field. Use (CPP) for heat flow and forces and use (NONC) for heat flux and force density. Use either method for mesh displacement and temperature. Interpolation must be consistent with the data transferred for the CFX code.
If you are working interactively, you can choose two pre-defined combinations, or , or you can choose a option. If you choose the load type, then the Total Force and Total Mesh Displacement data (corresponding to the ANSYS FORC and DISP labels, respectively) are transferred. If you choose the load type, then the Temperature and Wall Heat Flow data (corresponding to the ANSYS TEMP and HFLU labels, respectively) are transferred. If you choose , you can select any valid combination of label and option as described in the MFLCOMM command description. If you leave the as “default,” CFX will automatically find the corresponding multi-field interface name.
Note: You can specify multiple interface numbers or interface names (up to 50) in an MFX run by issuing multiple MFLCOMM commands.
The ANSYS Multi-field solver solver does not allow you to switch the load transfer direction for the same load quantity across the same interfaces for a restart run. For example, if Field1 sends temperature to and receives heat flow from Field2 across Interface 1 in a previous solution, then you cannot make Field1 send heat flow to and receive temperatures from Field2 across the same interface in a restart run, even if you cleared the corresponding load transfer command.
The following table lists the steps to set up the time controls.
| Step | Command | GUI Path |
|---|---|---|
| Set end time for ANSYS Multi-field solver analysis. | MFTIME |
|
| Set time step size for ANSYS Multi-field solver analysis. | MFDTIME |
|
| Restart the ANSYS Multi-field solver analysis (if necessary). | MFRSTART |
|
Use the MFTIME command to specify the end time of your
MFX analysis. Use the MFDTIME command to specify an
initial time step, minimum time step, maximum time step size, and time step
carryover key (for restarts). The time step size and end time default to 1. If
either DTMIN or DTMAX is
not equal to DTIME on the MFDTIME
command, auto time-stepping is turned on for the multi-field time loop. ANSYS
will automatically adjust the next multi-field time step size to occur between
DTMIN and DTMAX, based on
the status of the current convergence, the number of target stagger iterations
(specified by MFITER), and the actual number of iterations
needed to reach convergence at the current time step.
You must also specify the time step increment for each ANSYS field analysis. Auto time-stepping (AUTOTS) may be used within a field analysis. The time step increment for each ANSYS field analysis should be less than or equal to the time step increment for the overall analysis. The analysis allows sub-cycling over the ANSYS field, but load transfer across the field interface only occurs at multi-field time increments. CFX does not support sub-cycling, so the internal time step size for CFX should be the same as the multi-field time increments.
| Step | Command/Option | GUI Path |
|---|---|---|
| Specify a search option for interface mapping used by the profile preserving (NONC) interpolation scheme. | MFBUCKET |
|
| Activate normal distance checking used by the profile preserving (NONC) interpolation scheme. | MFTOL |
|
| Sets the control parameters used by the conservative (CPP) interpolation scheme. | MFCI |
|
When you use the profile preserving interpolation, you must use the bucket search method, which is set by default. If you turn off the bucket search option, you will get error messages and the solution will stop. This option partitions the interface into small, nearly equal-sized cells (buckets) for more efficient interface data mapping. You can specify a scaling factor for the search (the default is 50%). The number of buckets is equal to the scaling factor multiplied by the number of elements at the search interface. When normal distance checking (MFTOL) is activated, the mapping tool checks the normal distance from the node to the nearest element. The node is considered improperly mapped if the normal distance exceeds the tolerance value. The mapping tool creates a component to graphically display the improperly mapped nodes. See Mapping Diagnostics in the Coupled-Field Analysis Guide for more information. If the CFX mesh is the receiving side in a profile-preserving interpolation or the sending side in a conservative interpolation, and nodes are improperly mapped, the nodal component generated in ANSYS should be ignored because the CFX nodes do not exist in the ANSYS database.
When you use the conservative interpolation, MFX automatically selects an octree-based bisection search method to find all faces that intersect with the source face on the other side of the interface. For a dissimilar mesh interface, the nodes of one mesh are mapped to the local coordinates of an element in the other mesh. A relative separation factor handles the gaps between the two sides of the interface and can be adjusted via the MFCI command.
The following table lists the steps to set up the stagger solution.
| Step | Command | GUI Path |
|---|---|---|
| Set the maximum number of stagger iterations. | MFITER |
|
| Specify convergence values. | MFCONV |
|
| Specify relaxation values. | MFRELAX or MFFR (MFFR is GUI only) |
|
Use the MFITER command to set the maximum number of stagger iterations between the field solvers for each multi-field time step. At the end of each stagger iteration, the ANSYS master checks the convergence of the quantities transferred across the interface and the fields within each field solver. The analysis proceeds to the next time step if the interface quantities have converged. The stagger solution continues until the maximum number of stagger iterations has been reached or convergence occurs. The default is 10 stagger iterations. You can also specify a minimum stagger iteration (MFITER, ,MINITER) and a target stagger iteration (the desired number of stagger iterations) (MFITER,,,TARGET) for auto time stepping in MFX.
Use MFCONV to specify the convergence tolerance
(TOLER) for the quantities transferred across the
surface field interface. The default is 0.01 (1%).
By definition, convergence occurs when the changes of the interface loads are
smaller than the input tolerance TOLER. Convergence
is measured by:
where:
ε is the normalized change of the interface loads:
|| || = L2 norm of a vector
ϕnew = new load vector from other physics
ϕpre = applied load vector at the previous multifield iteration
The current applied load vector is given by:
where α is the relaxation factor specified by the MFRELAX command.
Convergence occurs when:
Note: Iteration controls and convergence criteria must also be set for the fields being solved in each of the coupled field solvers. Iteration controls are important for controlling the efficiency and stability of the coupled analysis. Convergence criteria are important for controlling the accuracy of the solutions provided by each field solver. General recommendations are summarized as:
Set the convergence criteria to obtain the desired level of solution accuracy.
Set the maximum stagger iterations to a value that is large enough to satisfy the convergence criteria during each multi-field time step.
Limit the work (e.g., iterations) done during the execution of each field solver to maintain a tighter coupling and promote efficiency and stability.
Use the MFRELAX command to specify the relaxation values
for the load transfer variables across the surface. The default relaxation value
is 0.75. Option = RELX will usually give you a more
stable and smooth load transfer and is suitable for strongly coupled problems
(such as FSI problems). If you are using a single stagger iteration for each
multi-field time step, you must use a relaxation value of 1.0 for all
quantities.
Use the MFFR command to relax the field solutions for an optimal convergence rate in coupled problems, especially cases that need dynamic relaxation. The ANSYS field that has the MFFR command applied will do only one nonlinear stagger iteration within each multi-field stagger; the convergence of the ANSYS field solver will be satisfied through multiple multi-field staggers. The CFX field solver can have multiple iterations within the field solver; see the CFX documentation for more details. ANSYS will not terminate the nonlinear field solution until the ANSYS field solver converges or reaches the maximum number of multi-field staggers as specified on MFITER.
If you are working interactively, use the commands shown in the following table to write the necessary input file.
| Step | Command | GUI Path |
|---|---|---|
| Write the MFX input file | MFWRITE |
|
You cannot initiate a solution interactively. You must issue MFWRITE to write out the input file containing all of the MFX data, and then submit that input file as a batch job, along with the necessary CFX input. When you write out the input file using MFWRITE, ANSYS will add /SOLU, SOLVE, and FINISH commands at the end of the input file.
The following table shows which commands are valid for multi-field analyses.
| Command | Valid for ANSYS Multi-field solver (MFS) | Valid for MFX |
|---|---|---|
| MFANALYSIS | yes | yes |
| MFBUCKET | yes | yes |
| MFCALC | yes | |
| MFCI | yes | |
| MFCLEAR | yes | yes |
| MFCMMAND | yes | |
| MFCONV | yes | yes |
| MFDTIME | yes | yes |
| MFELEM | yes | |
| MFEM | yes | |
| MFEXTER | yes | |
| MFFNAME | yes | |
| MFIMPORT | yes | |
| MFINTER | yes | |
| MFITER | yes | yes |
| MFLCOMM | yes | |
| MFLIST | yes | yes |
| MFMAP | yes | |
| MFPSIMUL | yes | |
| MFORDER | yes | |
| MFOUTPUT | yes | yes* |
| MFRELAX | yes | yes |
| MFRSTART | yes | yes |
| MFSORDER | yes | |
| MFSURFACE | yes | |
| MFTIME | yes | yes |
| MFTOL | yes | yes |
| MFVOLUME | yes | |
| MFWRITE | yes |
* Valid only for the ANSYS field in MFX.
For information on postprocessing, refer to An Overview of Postprocessing in the Basic Analysis Guide. To postprocess the fluid results, use CFD-Post.