The procedure for doing an MFS solution analysis consist of the following steps:
To perform an MFS analysis, you first create the field models in ANSYS. These models may be set up completely independently. The only criteria is that they share the same geometry (duplicate solid models). They may be created in a single ANSYS database, or in separate databases and imported (MFIMPORT command) to build a model. Each model consists of everything required to solve a particular field, including mesh, boundary conditions, analysis options, output options, etc. For information on how to set up a field analysis, refer to the Structural Analysis Guide, the Thermal Analysis Guide, and the Low-Frequency Electromagnetic Analysis Guide.
If you will be generating radiosity surface elements (RSURF), you must first mesh the different regions, and then generate the radiosity surface elements on each meshed region individually. Use RSURF,,,ETNUM to assign a separate element type number to each region. This procedure allow you to identify the individual regions later in the multi-field analysis. Also, include the radiosity surface element types in the field definition (MFELEM).
The next step is to flag field surface and volume interfaces for load transfer. Flagged surfaces sharing a common surface interface number will exchange surface load data; flagged volumes sharing a common volume interface number will exchange volume load data.
For surface load transfer across fields, use the SF family of commands (SF, SFA, SFE, or SFL) and the FSIN surface load label. Apply the field surface interface flag twice, once for each field surface where load transfer occurs. When issuing the SF, SFA, SFE, or SFL commands with the FSIN flag, apply the same interface number for both field interfaces. Load transfer occurs between fields with the same interface number. Also maintain unique interface numbers for load transfer across each pair of field surface interface, as these interface numbers are used in the MFSURFACE command for specifying the surface load transfer options.
For volumetric load transfer, use the BFE command and the FVIN volume load label. Apply the field volume interface flag twice: once for each field volume where load transfer occurs. When issuing the BFE command with the FVIN flag, apply the same interface number for both field interfaces where load transfer occurs. Load transfer occurs between fields with the same interface number. Also maintain unique interface numbers for load transfer across each pair of field volume interface, as these interface numbers are used in the MFVOLUME command for specifying the volume load transfer options.
The procedure for setting up the field solutions consists of the following main steps:
The following table lists the steps to define the fields and capture the field solutions.
| Step | Command | GUI Path |
|---|---|---|
| Define a field by grouping element types, add more element types to the field, or import a defined field into a current analysis. | MFELEM |
|
| MFEM |
| |
| MFIMPORT |
| |
| Specify a file name for each field. | MFFNAME |
|
| Capture solution options for each field. | MFCMMAND |
|
| Delete all solution options before setting options for a new field. | MFCLEAR |
|
Use the MFELEM command to define the fields for analysis. Use the MFEM command to add more element types to the field if it has more than 10 element types defined. It groups element types into different fields with a specified field number for the ANSYS Multi-field solver. Elements grouped into a field for analysis should belong to a single physics. More precisely, a single physics represents an ANSYS model using a single set of elements solving that physics. For instance, a coupled-field element type set for piezoelectric analysis will solve simultaneously electric and structural analysis within a single field loop. You may wish to couple this field model to a thermal field model to include thermal effects. The number of element types in a field must not be changed between restarts.
In addition to defining fields from models created in one ANSYS session, you can import fields defined in another ANSYS session and saved via a CDB file (CDWRITE command). Use the MFIMPORT command to import any number of new fields into a current analysis. With this option, you can prepare field models independently and then combine them to perform an MFS solution.
The import option makes use of the NUMOFF command capability to offset the current database numbering of entities to allow the model on the CDB file to be imported. Fields defined using the MFELEM or MFEM commands are updated based on the renumbered element type numbers. If no field is defined before the MFIMPORT command is issued, the program will automatically group the existing element types into a field (MFELEM or MFEM) and write any solution options to a command file (MFCMMAND). The field on the CDB file is assigned the field number that you specify, and it is read into the database accordingly. Exercise caution when using the MFIMPORT option since the NUMOFF command capability has some limitations.
Use the MFFNAME command to define file names for each field used in the MFS analysis. The field file name is used for all files during solution of the specified field. The field file name defaults to field"n" where n is the field number.
MFS analysis allows different solution options to be specified for each field analysis. Use the MFCMMAND command to capture solution options for each field number. The solution options are written to a file, and read when the field is solved. Issue the MFCLEAR, SOLU command to clear all existing solution options before setting options for a new field. The MFCLEAR, SOLU command sets all solutions options to defaults values in ANSYS. Specify solution options for each field analysis by issuing the ANSYS solution commands for analysis options, nonlinear options, load step options, etc. The solution options are written to a file that you specify for the given field number. The command file name defaults to field"n".cmd where n is the field number.
Note: If you need to model morphing, you must set that up before you issue the MFCMMAND command. For information on morphing, see Set up Morphing (if Necessary).
MFS analyses allow either stepped or ramped loading, but not both. The KBC command is globally used for all fields by the ANSYS Multi-field solver and therefore is not written to the field-specific command files. This restriction is due to the consistent load transfer issue between the fields. If the KBC command is not issued before the SOLVE command, ramped loading (KBC,0) is used. If the KBC command is issued more than once, the loading type specified by the last command is used.
The following table lists the steps to set up interface load transfers.
MFS analysis allows load transfer across flagged surface and volume interfaces. Use the MFSURFACE command to specify a surface load transfer across a field interface. Specify the variable being transferred, the send and receive field numbers, and the field surface interface number specified by the SF family of commands (SF, SFA, SFE, or SFL) and the FSIN surface load label. Use the MFVOLUME command to specify volume load transfer across a field interface. Specify the variable being transferred, the send and receive field numbers, and the field surface interface number specified by the BFE command and the FVIN volume load label.
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 global field solution.
| Step | Command | GUI Path |
|---|---|---|
| Turn the ANSYS Multi-field solver analysis on. | MFANALYSIS |
|
| Specify a globally conservative or profile preserving load transfer interpolation. | MFINTER |
|
| Specify a search option for load transfer interpolation. | MFBUCKET |
|
| Specify the field analysis order. | MFORDER |
|
| Define external fields (if necessary). | MFEXTER |
|
Use the MFANALYSIS command to activate an MFS analysis. MFANALYSIS,OFF deactivates an analysis (OFF is the default).
Use the MFINTER command to specify a globally conservative or profile preserving interpolation for the load transfer across the field interface. Globally conservative or profile preserving interpolation applies to forces, heat flux, and heat generation transferred across a field interface. Profile preserving interpolation transfers forces, heat flux, and heat generation across field interfaces as flux quantities, and globally conservative interpolation transfers these variables as forces and heat rates. The interpolation defaults to profile preserving.
A bucket search is the default option. This option partitions the interface into small cells (buckets) for more efficient interface data mapping. You can specify a scaling factor for the search algorithm (default is 50%). The number of buckets is equal to the scaling factor times the number of elements at the search interface. Use the MFBUCKET command if you want to switch to a global search.
Use the MFORDER command to specify the solution order for the defined fields. The MFORDER command specifies the order of the field solutions from the first field solution to the last field solution of the MFS analysis.
You can define an external field (MFEXTER) that predefines loads and exists only to transfer those loads to another field. It requires fully specified loads and does not perform a solution during an MFS analysis. It only transfers a load to another field. The external field should be set up in the following fashion:
If transferring displacements or temperature from an external field, specify the required displacements or temperature using the D command, on the external field mesh. Also specify the variable label to be transferred using MFSURFACE or MFVOLUME for surface or volumetric load transfer, respectively.
If transferring forces or heat flux from an external field, specify the forces or heat rates using the F command on the external mesh. Constrain the complete field mesh with a trivial displacement or temperature.
The External field capability allows an easy mechanism for transferring results from an external software code that can support writing a CDB file consisting of nodes, elements, and loads.
Use the MFEXTER command to define external fields during a analysis. Specify the loads to be transferred on the external field and use MFSURFACE or MFVOLUME to specify the load to be transferred to other fields across a field interface.
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 |
|
Use MFITER to set the maximum number of stagger iterations between the fields for an MFS analysis. At the end of each stagger loop, the coupling algorithm checks the convergence of the quantities transferred across the interface. 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.
Use MFCONV to specify the convergence tolerance
(TOLER) for the quantities transferred across the
surface and volume field interface. The default is 0.01 (1%). The interpolation
algorithm (globally conservative or profile preserving) determines the
quantities transferred across the field interface.
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:
Use MFRELAX to specify the relaxation values for the load transfer variables across the surface and volume field interface. If you are using a single stagger iteration for each time step of the MFS analysis, use a relaxation value of 1.0 for all quantities. The default relaxation value is 0.75.
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 field solver will be satisfied through multiple multi-field staggers. ANSYS will not terminate the nonlinear field solution until the field solver converges or reaches the maximum number of multi-field staggers as specified on MFITER.
The following table lists the steps to set up the time and frequency controls.
| Step | Command | GUI Path |
|---|---|---|
| Set end time for MFS analysis. | MFTIME |
|
| Set time step increment for MFS analysis. | MFDTIME |
|
| Set time step increment for each field analysis. | DELTIM |
|
| Specify a restart (if necessary). | MFRSTART |
|
| Specify a calculation frequency for a field (if necessary). | MFCALC |
|
| Specify the output frequency for MFS analysis. | MFOUTPUT |
|
Use the MFTIME command to specify the end time of your MFS analysis. The end time should be a multiple of the time step increment. Use the MFDTIME command to specify an initial time step, minimum time step, and maximum time step size. The solution only supports constant time stepping. The time step increment and end time default to 1.
You must also specify the time step increment for each field analysis. Use DELTIM for a structural, thermal or electromagnetic analysis. Auto time-stepping (AUTOTS) may be used within a field analysis as well. The time step increment for each field analyses should be less than or equal to the time step increment for the MFS analysis. The analysis sub-cycles over each field analyses so that load transfer across the field interface occurs at time increments specified by MFDTIME. The MFCMMAND command captures the time step size for each field analysis.
You can restart the MFS analysis from either the last time step or the last converged solution in the results file.
Use MFCALC to set the calculation frequency for a given
field within the analysis. The field solution for any given field can be
obtained at every time step or every Nth time step.
The calculation frequency option only applies to a field using a harmonic or
static analysis. This option is useful, for example, in skipping the harmonic
field solution (and load transfer updating) during a time step when the field
quantities transferred are not varying significantly over the specified time
increment (MFDTIME).
Use MFOUTPUT to set the output frequency for results from
your analysis with respect to the time step (MFDTIME). You
can write output at every time step or every Nth time
step. The output frequency applies to each field results file.
In an MFS analysis, the deflection of a structure may effect the solution of a surrounding non-structural field. A good example is electrostatic-structural interaction in MEMS structures where the structural deformation alters the electrostatic field which in turn alters the electrostatic forces and resulting deformation. To model this type of behavior, the field mesh surrounding a structure must be updated to coincide with the deflection of the structure. The process of updating the field mesh is called morphing. The structural field sends displacements to the non-structural field using the MFSURFACE command for a defined surface interface. The ANSYS Multi-field solver makes use of the MORPH command to invoke morphing within a given field model.
| Step | Command | GUI Path |
|---|---|---|
| Turn morphing on (if necessary). | MORPH |
|
The MORPH command is applicable to any non-structural field analysis (for example, air surrounding a solid). The command activates the UX, UY, and UZ degrees of freedom for non-structural elements so that boundary conditions may be placed on the field mesh to constrain the movement of the non-structural mesh during morphing. Morphing of a field mesh occurs during the non-structural field stagger prior to the field solution using displacements transferred at the surface interface between the structural field and the non-structural field.
The procedure for preparing a non-structural mesh for morphing is as follows. You must complete these steps before you issue the MFCMMAND command.
Create the non-structural model and mesh.
Set morphing and remeshing controls by issuing the morphing command (MORPH,ON). The MORPH command allows you to specify remeshing controls such as maximum allowable change in element size or aspect ratio, as well as other controls. Use MORPH,ON to turn on non-structural field morphing.
If morphing is activated during the solution, it will remain active until deactivated. To avoid unwanted morphing in structural fields, MORPH,OFF should be issued before issuing MFCMMAND. If morphing is ON for any field, the recommended practice is to explicitly define morphing (either ON or OFF) for all fields.
Apply appropriate structural boundary condition constraints to the boundary of the non-structural mesh (typically, you set normal components of displacement to zero).
After each remesh, new databases and results files are written with the
extensions .rth0n
and .db0n
, where n is the remesh file number
(FieldName.rth01, FieldName.rth02,
... and FieldName.db01,
FieldName.db02, etc.). The original database file is
FieldName.dbo. The FieldName.db01,
FieldName.db02, etc. files have elements that are
detached from the solid model.
Morphed fields must be in the global Cartesian system (CSYS = 0).
To obtain the solution or restart the MFS analysis from either the last time step or the last converged solution in the results file, use the commands shown in the following table.
To postprocess an analysis, the database must be available and the appropriate results file selected. To select the appropriate results file, use the FILE command in POST1 or POST26. The results file names are based on the settings used on the MFFNAME command. You can review results using standard ANSYS POST1 and POST26 commands. Be sure to select the appropriate field element types for the results file selected before you postprocess the results (ESEL). MFS analyses do not support simultaneous postprocessing of the field results.
For information on postprocessing, refer to An Overview of Postprocessing in the Basic Analysis Guide. To get the correct results, use the last database file which was saved right after the SOLVE command only, or read the results file only without the database.
The displacements of non-structural elements are mesh (or grid) displacements to avoid mesh distortion but have no physical meaning except at the interface between the structural field and the non-structural field.