Release 11.0 Documentation for ANSYS
www.kxcad.net Home > CAE Index > ANSYS Index > Release 11.0 Documentation for ANSYS
The ANSYS Multi-field solver is available in the ANSYS Multiphysics product. It provides you with the ability to solve coupled-field problems such as the following:
MEMS Actuation (electrostatic/structural without fluid coupling)
Electric Machines (magneto/thermal/structural coupling)
Joule Heating (thermal/electric/structural coupling)
Induction Heating (harmonic electromagnetic/thermal coupling)
Induction Stirring (harmonic electromagnetic/thermal/fluid coupling)
RF Heating (high-frequency electromagnetic/thermal/structural coupling)
Thermal/Stress Analysis (thermal/structural coupling)
Fluid Solid Interaction Analysis (fluid/structural coupling)
The following ANSYS Multi-field solver algorithm topics are available:
Load transfer is the process by which one field transmits mesh-based quantities to another field. The transfers occur from a surface to a surface or from a volume to a volume. Electrostatic Actuated Beam Analysis is an example of a surface load transfer problem. In that problem, forces are transmitted from the electrostatic field to the structural field and displacements are transmitted from the structural domain to the electrostatic field. Thermal-Stress Analysis of a Thick-walled Cylinder and Induction-heating Analysis of a Circular Billet are examples of volumetric load transfer problems. In the thick-walled cylinder problem, temperatures are transferred from the thermal field to the structural field. In the circular billet problem, heat generation is transferred from the magnetic field to the thermal field and temperatures are transferred from the thermal field to the magnetic field.
The ANSYS Multi-field solver automatically transfers coupled loads across dissimilar meshes. Two interpolation methods are available for a load transfer: profile preserving and globally conservative. In a profile preserving interpolation, each node on the receiver side maps onto an element on the sender side (αi). The transfer variable is then interpolated at αi. The transfer value is Ti = φ (αi). Thus, all nodes on the receiver side query the sender side.
Figure 3.1 Profile Preserving Interpolation
Figure 3.2 Globally Conservative Interpolation
Some important points to remember about the interpolation methods are:
For a profile preserving interpolation, the forces and heat rate will not balance on this interface. For a globally conservative interpolation, total force and total heat rate will balance on this interface. However, locally the distributions might not agree.
Figure 3.3 Profile Preserving Interpolation - Load Imbalances
Figure 3.4 Globally Conservative Interpolation - Load Balance
It makes physical sense to conserve quantities like heat flux and force at the surface interfaces. Similarly, heat generation should be conserved at volumetric interfaces. However, it does not make physical sense to conserve displacements or temperatures on a integral basis. However, displacement and temperature profiles should be adequately captured across interfaces.
As shown in the following figures, for a profile preserving interpolation, you should have a coarse mesh on the sending side and a fine mesh on the receiver side, rather than the converse. When the coarse mesh is on the sending side, the receiver adequately captures the normal heat flux profile. On the receiver side, a fine mesh ensures a sufficient number of nodes. When the coarse mesh is on the receiver side, the receiver does not adequately capture the normal heat flux profile due to an insufficient number of nodes on the receiver side.
Figure 3.5 Profile Preserving Interpolation - Coarse Mesh on the Sending Side
Figure 3.6 Profile Preserving Interpolation - Coarse Mesh on the Receiver Side
As shown in the following figures, for a globally conservative interpolation it is better to have a fine mesh on the sending side and a coarse mesh on the receiver side than the converse. When the fine mesh is on the sending side, the receiver adequately captures the forces. When the fine mesh is on the receiver side, the load distribution on the receiver might not be captured, even though the total force on the receiver is equal to the total force on the sender.
Figure 3.7 Globally Conservative Interpolation - Fine Mesh on Sending Side
Figure 3.8 Globally Conservative Interpolation - Fine Mesh on Receiver Side
The above two points hold true if either the sender or receiver mesh is made of higher order elements. Exercise care if you wish to produce a node-to-node mapping from higher order elements to lower order elements. For example, as shown in the following figure, a globally conservative load transfer across an interface that has the same number of elements on both sides will not produce the correct profile if the receiver is higher order.
Figure 3.9 Three Lower Order Elements
To get the right profile, you need to double the number of sending lower order elements as shown in the following figure. Also note you cannot drop mid-side nodes at a surface or volume interface.
Figure 3.10 Six Lower Order Elements
You can specify a globally conservative or a profile preserving interpolation method for forces, heat flux, and heat generation. Displacement and temperature transfers are always profile preserving.
In order to transfer loads across a dissimilar mesh interface, the nodes of one mesh must be mapped to the local coordinates of an element in the other mesh. The MFS solution algorithm must perform two mappings for every surface to surface and volume to volume interface. For example, in a fluid-solid interaction problem, fluid nodes must be mapped to the solid elements to transfer displacements. Likewise, solid nodes must be mapped to the fluid elements to transfer stresses.
Figure 3.11 Fluid-Solid Interaction Load Transfer
There are two mapping algorithms available: global and bucket search.
Global Method
As the name implies, the node in question loops over all the existing elements of the other mesh and tries to locate an element that it can be mapped to. Most nodes find a unique element and are mapped easily. However, occasionally a node is mapped to two or more elements. This occurs when a finite nonzero gap/penetration exists between the two meshes. The element that minimizes the distance is then selected. In the following figure, node N1 is found in elements e1 and e2, so it is mapped to the element which minimizes the gap distance (e1 because d1 < d2).
Figure 3.12 Node Mapped to Minimize Gap
Sometimes a node does not map to any element. This occurs when the interface edges are not aligned. In the following figure, node N1 does not map to any element, so it is mapped to the closest node (N1').
Figure 3.13 Node Mapped to Closest Node
The global method has a complexity of θ(n x m) where n is the number of nodes mapped onto m elements. If n and m are of the same order, the time required to compute the mapping grows quadratically and leads to computational inefficiency, especially for large models.
The same issues exist for 3-D models involving surface-to-surface mapping. They are also encountered for volumetric mapping in 2-D and 3-D models.
Bucket Search Method
The bucket search method is designed to alleviate the inefficiency problem that the global method has when the number of nodes increases. The underlying ideas for the bucket search method are presented in the book Computational Nonlinear Mechanics in Aerospace Engineering, American Institute of Aeronautics and Astronautics, edited by S. Atluri, ISBN 1563470446, Chapter 5, Fast Projection Algorithm for Unstructured Meshes by K. Jansen, F. Shakib, and T. Hughes, 1992.
For a given node, the bucket search method restricts the elements over which it loops. This is accomplished as follows:
All elements are distributed in Cartesian boxes (also referred to as buckets).
The node in question is then located in a box.
The global method is used for the node in question, but the elements are restricted to that box only.
For example, in the following figure, elements e1, e2, and e3 are in box 1, elements e3 and e4 are in box 2, and e4, e5, and e6 are in box 3. Node N1 searches only over the elements in box 3.
Figure 3.14 Node in Box 3 with Three Elements
When the node in question is in a box with elements, the mapping is identical to global mapping.
While this procedure appears straightforward, it is more complex when the node in question is in an empty box as shown in the following figure. This can occur when there are gap/penetration issues or the interface edges are misaligned.
Figure 3.15 Nine boxes and Node in Empty Box
The mapping is then different than global mapping. The mapping procedure requires locating the nearest boxes that have elements and choosing only one box for element looping.
The bucket search method has a complexity of θ(n) where n is the number of nodes to be mapped onto m elements. However, to achieve this increased efficiency, buckets must be created and the m elements must be placed in them, at an additional computational expense.
This same mapping process is used for 3-D models involving surface-to-surface mapping and 2-D and 3-D models involving volumetric mapping.
You can use the MFTOL command (Main Menu> Preprocessor> Multi-field Set Up> MFS-Single Code> Setup> Global) to turn normal distance checking on for surface mapping and to set a normal distance limit from a node to an element surface. The normal distance checking is a relative value by default, and defaults to 1.0e-6 (unit-independent). You can specify an absolute value (unit-dependent) via the MFTOL command.
When using relative gap tolerance (Toler = REL on the MFTOL command), the normal distance tolerance is derived from the product of the relative tolerance Value and the largest dimension of the Cartesian bounding box for a specific interface. Therefore, each interface will have a different normal distance tolerance, even though MFTOL is a global command.
As shown in the following figure, in surface mapping, improperly mapped nodes include nodes that exceed the normal distance limit specified (figure a) and nodes that are on misaligned surfaces (figure b). In volumetric mapping, improperly mapped nodes are nodes out of the target domain (figure c).
The mapping tool creates components to graphically display nodes that are improperly mapped. Component names for surface mapping are MFSU_interface number_field number_label_field number (for example, MFSU_1_1_TEMP_2). Component names for volumetric mapping are MFVO_interface number_field number_label_field number (for example, MFVO_2_1_HGEN_2). ANSYS cannot display improperly mapped nodes from CFX meshes.
You can use the MFMAP command (Main Menu> Preprocessor> Multi-field Set Up> MFS-Single Code> Interface> Mapping) to calculate, save, resume, or delete mapping data. By saving mapping data to a file and using resume, you might be able to significantly reduce computing time during a restart or another solve. If you wish to resume a mapping file, be sure to first delete any existing mapping data in memory. You can also use this command to check your mapping without performing a solution. See the Commands Reference for more information about this command.
The following tables show the loads that the ANSYS Multi-field solver can transfer in a coupled physics analysis.
Table 3.1 Load Transfer Between Fields
| Field | Structural | Thermal | Electric | Magnetic | Fluid |
|---|---|---|---|---|---|
| Structural | 1 | 2 | 3 | 4 | |
| Thermal | 5 | 6 | 7 | ||
| Electric | |||||
| Magnetic | 8 | ||||
| Fluid |
| Volumetric Load Transfer | Structural | Thermal |
|---|---|---|
| Send | Displacements | Temperature |
| Receive | Temperature | Displacements |
Electrostatic - Structural Coupling
| Surface Load Transfer | Structural | Electrostatic |
|---|---|---|
| Send | Displacements | Forces |
| Receive | Forces | Displacements |
Structural - Magnetic Coupling
| Surface or Volumetric Load Transfer | Structural | Magnetic |
|---|---|---|
| Send | Displacements | Forces |
| Receive | Forces | Displacements |
| Surface Load Transfer | Structural | Fluid |
|---|---|---|
| Send | Displacements | Forces |
| Receive | Forces | Displacements |
| Volumetric Load Transfer | Thermal | Electric |
|---|---|---|
| Send | Temperature | Heat Generation |
| Receive | Heat Generation | Temperature |
| Volumetric Load Transfer | Thermal | Magnetic |
|---|---|---|
| Send | Temperature | Heat Generation |
| Receive | Heat Generation | Temperature |
| Surface Load Transfer | Thermal | Fluid |
|---|---|---|
| Send | Temperature/Heat Flux | Temperature/Heat Flux |
| Receive | Heat Flux/Temperature | Heat Flux/Temperature |
| Volumetric Load Transfer | Magnetic | Fluid |
|---|---|---|
| Send | Forces | — |
| Receive | — | Forces |
The ANSYS Multi-field solver supports the elements shown in the following tables. These elements support the SF family of commands (SF, SFA, SFE, or SFL) for surface load transfer (field surface interface: FSIN flag) and the BFE command for volumetric load transfer (field volume interface: FVIN flag) during an analysis. You need to flag these elements at the surface (FSIN) and volume (FVIN) interface for load transfer to other fields during the analysis. Other elements types can be used in any of the field analyses, but they will not participate in load transfer.
Table 3.2 Structural and Thermal Elements
| Structural Elements | |||
| PLANE | SOLID | BEAM | SHELL |
| SOLID45 | BEAM3 | ||
| PLANE42 | SOLID92 | BEAM23 | SHELL63 |
| PLANE82 | SOLID95 | BEAM188 | SHELL93 |
| PLANE182 | SOLID185 | BEAM189 | SHELL181 |
| PLANE183 | SOLID186 | SOLSH190 | |
| SOLID187 | SHELL281 | ||
| Thermal Elements | |||
| PLANE | SOLID | SHELL | |
| PLANE35 | SOLID70 | SHELL57 | |
| PLANE55 | SOLID87 | ||
| PLANE77 | SOLID90 | ||
Table 3.3 Electromagnetic, Fluid, and Coupled-Field Elements
| Electromagnetic Elements | |||
|---|---|---|---|
| PLANE | SOLID | HF | |
| PLANE53 | SOLID96 | HF119 | |
| PLANE121 | SOLID97 | HF120 | |
| PLANE230 | SOLID117 | ||
| SOLID122 | |||
| SOLID123 | |||
| SOLID231 | |||
| SOLID232 | |||
| Fluid Elements | |||
| PLANE | SOLID | ||
| FLUID141 [1] | FLUID142 [1] | ||
| Coupled-Field Elements | |||
| PLANE | SOLID | SHELL | |
| PLANE13 | SOLID5 | SHELL157 | |
| PLANE67 | SOLID62 | ||
| PLANE223 | SOLID69 | ||
| SOLID98 | |||
| SOLID226 | |||
| SOLID227 | |||
You can use the FLOTRAN remeshing capability in a fluid-solid interaction analysis. See Remeshing in the Fluids Analysis Guide for additional information.
The solution algorithm for the ANSYS Multi-field solver is shown in the following figure. The MFANALYSIS command activates a solution. The solution loop consists of three loops: field loop, stagger loop, and time loop. The ANSYS Multi-field solver supports transient, static, and harmonic analysis of fields inside the field loop.
Figure 3.18 ANSYS Multi-field solver Algorithm
The time loop corresponds to the time step loop of the MFS problem and is set with the MFTIME command. A constant time step size may be set with the MFDTIME command. For a static analysis the time loop refers to the load step for each field analysis. For harmonic analysis the time loop refers to a harmonic solution within the time step. For a transient analysis, the time step represents the actual time-transient end time and time step. Load transfer between fields occur at the time loop time steps.
Within each time loop is the stagger loop. The stagger loop allows for implicit coupling of the fields in the MFS solution. Within each step in the time loop, the field solutions are repeated in the stagger loop until convergence. The number of iterations 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.
Within each stagger loop is the field loop. The field loop contains the analysis of each field solution. The field Loop is set up like any single ANSYS analysis. Each field can be set up by grouping a set of element types using the MFELEM command. Solution options for each field are set using the MFCMMAND command. Surface and volumetric load transfer between fields is specified using the MFSURFACE and MFVOLUME commands, respectively. Fields can share a dissimilar mesh across the interface and load transfer from a field occurs after the solution of the respective field. Load transfer to a particular field occurs before solution of the field. Morphing (MORPH command) of a non-structural field mesh occurs prior to the field solution. The morphing is based on displacements of a previous structural field solution.
