5.4. Performing a Load Transfer Coupled Physics Analysis with Multiple Physics Environments

This section outlines using a single database with multiple physics environments to run a load transfer coupled physics analysis.

  1. Build a model that meets the requirements of each physics discipline that will be addressed. Keep the following points in mind:

    • Each ANSYS solid model area or volume defined has its own particular needs with respect to element type, material properties, and real constants. All solid model entities should have element type numbers, real constant set numbers, material numbers, and element coordinate system numbers applied. (Their meaning will change according to the physics environment.)

    • Certain groups of areas or volumes will be used in two or more different physics environments. The mesh you use must be suitable for all environments.

  2. Create the physics environment. You perform this step for each physics discipline that is part of the load transfer coupled physics analysis.

    • Refer to various sections of the ANSYS Analysis Guides as necessary to determine what you should specify for a particular physics analysis.

    • Define the necessary element types to be used in a physics simulation (for example, ET,1,13 or ET,2,117 for a magnetic solution). Set the "null" element type (Type = 0, i.e. ET,3,0) for use in regions not associated with or needed for a given physics. Elements assigned to the null element type are ignored during solution.

    • Assign material properties, real constant set data, and element coordinate systems as needed, in accordance with the established attribute numbers defined earlier for the model.

    • Assign attribute numbers for element type, materials, real constants, and element coordinate systems to the solid model areas or volumes (using the AATT command (Main Menu> Preprocessor> Meshing> Mesh Attributes> All Areas or Picked Areas) or the VATT command (Main Menu> Preprocessor> Meshing> Mesh Attributes> All Volumes or Picked Volumes)).

    • Apply the nominal loads and boundary conditions. These conditions are those that are the same (for a steady state problem) for each execution of this physics analysis in the overall iterative procedure.

    • Set all the solution options.

    • Choose a title for the physics environment and issue the PHYSICS,WRITE command with that title. For example, in a thermal-magnetics analysis, you could use the following command to write out the thermal physics environment:

      Command(s): PHYSICS,WRITE,Thermal
      GUI: Main Menu> Preprocessor> Physics> Environment> Write
    • Clear the database of the present physics environment in order to create the next physics environment. This is done by issuing the PHYSICS,Clear option.

      Command(s): PHYSICS,Clear
      GUI: Main Menu> Preprocessor> Physics> Environment> Clear
    • Prepare the next physics environment as noted above.

    • Issue SAVE to save the database and physics file pointers.

      Assuming that the jobname for this multiphysics analysis is "Induct" and these are the first two physics environment files written, the files would be named Induct.PH1 and Induct.PH2. For more information about the PHYSICS command, see the Command Reference.

  3. Perform the load transfer coupled physics analysis, performing each physics analysis in turn.

    /SOLU                      ! Enter solution
    PHYSICS,READ,Magnetics     ! Contains magnetics environment
    SOLVE
    FINISH
    /SOLU
    PHYSICS,READ,Thermal
    LDREAD,FORCE,,,,2,,rmg     ! Magnetic Lorentz forces
    SOLVE

The extensions on the LDREAD command are associated with the results file which is being read in. Results from a thermal analysis would be read in from a Jobname.RTH file. All other results besides magnetics would come from a Jobname.RST file.

5.4.1. Mesh Updating

Many times a coupled-field analysis involving a field domain (electrostatic, magnetic) and a structural domain yields significant structural deflections. In this case, to obtain an overall converged coupled-field solution it is often necessary to update the finite element mesh in the non-structural region to coincide with the structural deflection and recursively cycle between the field solution and structural solution.

Figure 5.3: Beam Above Ground Plane illustrates a typical electrostatic-structural coupling problem requiring mesh updating. In this problem, a beam sits above a ground plane at zero potential. A voltage applied to the beam causes it to deflect (from electrostatic forces) toward the ground plane. As the beam deflects, the electrostatic field changes, resulting in an increasing force on the beam as it approaches the ground plane. At a displaced equilibrium, the electrostatic forces balance the restoring elastic forces of the beam.

Figure 5.3:  Beam Above Ground Plane

Beam Above Ground Plane

To run a simulation of this problem requires adjustment of the field mesh to coincide with the deformed structural mesh. In ANSYS, this adjustment is known as mesh morphing.

To accomplish mesh morphing, you issue the DAMORPH command (morphing elements attached to areas), DVMORPH command (morphing elements attached to volumes, or the DEMORPH command (morphing selected elements). You use the RMSHKY option to specify one of the following three ways of mesh morphing:

  • Morphing - The program moves nodes and elements of the "field" mesh to coincide with the deformed structural mesh. In this case, it does not create any new nodes or elements or remove any nodes or elements from the field region.

  • Remeshing - The program removes the field region mesh, and replaces it with a new mesh that coincides with the deformed structural mesh. Remeshing does not alter the structural mesh. It connects the new field mesh to the existing nodes and elements of the deformed structural mesh.

  • Morphing or Remeshing - The program attempts to morph the field mesh first. If it fails to morph, the program switches to remeshing the selected field region. This is the default.

Mesh morphing affects only nodes and elements. It does not alter solid model entity geometry locations (keypoints, lines, areas, volumes). It retains associativity of the nodes and elements with the solid modeling entities. Nodes and elements attached to keypoints, lines, and areas internal to a region selected for morphing may in fact move off these entities; however, the associativity will still remain.

You must exercise care when applying boundary conditions and loads to a region of the model undergoing mesh morphing. Boundary conditions and loads applied to nodes and elements are appropriate only for the morphing option. If boundary conditions and loads are applied directly to nodes and elements, the DAMORPH, DVMORPH, and DEMORPH commands require that these be removed before remeshing can take place. Boundary conditions and loads applied to solid modeling entities will correctly transfer to the new mesh. Since the default option may morph or remesh, you are better off assigning only solid model boundary conditions to your model.

You must also exercise care with initial conditions defined by the IC command. Before a structural analysis is performed, the DAMORPH, DVMORPH, and DEMORPH commands require that initial conditions be removed from all null element type nodes in the non-structural regions. Use ICDELE to delete the initial conditions.

The morphing algorithm uses the ANSYS shape checking logic to assess whether the element is suitable for subsequent solutions. It queries the element type in the morphing elements for shape checking parameters. In some instances, the elements in the morphing region may be the null element type (Type 0). In this case, the shape checking criteria may not be as rigorous as the shape checking criteria for a particular analysis element type. This may result in elements failing the shape checking test during the analysis phase of a subsequent solution in the field domain. To avoid this problem, reassign the element type from the null element type prior to issuing the morphing command.

Displacements results from a structural analysis must be in the database prior to issuing a morphing command. Results are in the database after a structural solution, or after reading in the results from the results file (SET command in POST1). The structural nodes of the model move to the deformed position from the computed displacements. If you are performing a subsequent structural analysis, you should always restore the structural nodes to their original position. You can accomplish this by selecting the structural nodes and issuing UPCOORD with a FACTOR of -1.0.

Command(s): UPCOORD,Factor
GUI: Main Menu> Solution> Load Step Opts> Other> Updt Node Coord

Mesh morphing supports all 2-D models meshed with quadrilateral and triangular lower and higher order elements. For 2-D models, all nodes and elements must be in the same plane. Arbitrary curved surfaces are not supported. In 3-D, only models with the following shape configurations and morphing options are supported.

  • All tetrahedral elements - (morphing and remeshing supported)

  • All brick elements - (morphing supported)

  • All wedge elements - (morphing supported)

  • Combination of pyramid-tetrahedral elements - (morphing supported)

  • Combination of brick-wedge elements - (morphing supported)

Mesh morphing will most likely succeed for meshes with uniform-sided elements (such as those created with the SMRTSIZE command option). Highly distorted elements may fail to morph.

Figure 5.4: Area Model of Beam and Air Region illustrates a beam region immersed within an electrostatic region. Area 1 represents the beam model and Area 2 represents the electrostatic region. In this scenario, you would select Area 2 for morphing.

Figure 5.4:  Area Model of Beam and Air Region

Area Model of Beam and Air Region

In many instances, only a portion of the model requires morphing (that is, the region in the immediate vicinity of the structural region). In this case, you should only select the areas or volumes in the immediate vicinity of the structural model. Figure 5.5: Area Model of Beam and Multiple Air Regions illustrates the beam example with multiple electrostatic areas. Only Area 3 requires mesh morphing. In order to maintain mesh compatibility with the nonmorphed region, the morphing algorithm does not alter the nodes and elements at the boundary of the selected morphing areas or volumes. In this example, it would not alter the nodes at the interface of Areas 2 and 3.

Figure 5.5:  Area Model of Beam and Multiple Air Regions

Area Model of Beam and Multiple Air Regions

To perform mesh morphing at the end of a structural analysis, issue the following:

Command(s): DAMORPH, DVMORPH, DEMORPH
GUI: Main Menu> Preprocessor> Meshing> Modify Mesh> Refine At> Areas
Main Menu> Preprocessor> Meshing> Modify Mesh> Refine At> Volumes
Main Menu> Preprocessor> Meshing> Modify Mesh> Refine At> Elements

An alternative command, MORPH, may be used for mesh morphing. It is generally more robust than the DAMORPH, DVMORPH, and DEMORPH commands and it can be used with all element types and shapes. To prepare a non-structural mesh for morphing with the MORPH command, perform the following steps:

  1. Create the non-structural model and mesh.

  2. Activate the morphing command (MORPH,ON).

  3. Apply appropriate structural boundary condition constraints to the boundary of the non-structural mesh (typically, you set normal components of displacement to zero).


Note:  Morphed fields must be in the global Cartesian system (CSYS = 0).


5.4.2. Restarting an Analysis Using Multiple Physics Environments

In many load transfer coupling applications, you may need to restart one of the physics solutions. For example, in induction heating, you need to restart the transient thermal analysis during the load transfer coupling cycles. For static nonlinear structural coupled-field analysis, it is advantageous to restart the structural solution rather than start all over. You can implement a restart procedure easily within a load transfer coupled-field analysis. A restart requires the EMAT, ESAV, and DB files of the particular physics. You can isolate EMAT and ESAV files for the particular physics by using the /ASSIGN command. If you use a single database with multiple physics files, the database file will be consistent with the physics. Following is a summary of the restart procedure:

  1. Use the /ASSIGN command to redirect the file assignment for the EMAT and ESAV files prior to solving the physics domain requiring a restart.

  2. Perform the restart analysis.

  3. Use the /ASSIGN command to redirect the file assignments for the EMAT and ESAV files to their default values for use by the other physics domains.

The induction heating example problem described later on in the chapter demonstrates the use of a transient restart thermal analysis.


Release 18.2 - © ANSYS, Inc. All rights reserved.