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 3.3: 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 3.3: 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 Mechanical APDL, this adjustment is known as mesh morphing.

To accomplish mesh morphing, issue DAMORPH (morphing elements attached to areas), DVMORPH (morphing elements attached to volumes, or DEMORPH (morphing selected elements). Specify RMSHKY for one of the following mesh-morphing methods:

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.

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

Use 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, DAMORPH, DVMORPH, and DEMORPH 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.

Also use care with initial conditions (IC). Before a structural analysis is performed, DAMORPH, DVMORPH, and DEMORPH require that initial conditions be removed from all null element type nodes in the non-structural regions. Issue ICDELE to delete the initial conditions.

The morphing algorithm determines whether the element is suitable for subsequent solutions. It queries the element type in the morphing elements for shape-checking parameters. In some cases, 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 in POST1). The structural nodes of the model move to the deformed position from the computed displacements. If performing a subsequent structural analysis, always restore the structural nodes to their original position by selecting the structural nodes and issuing UPCOORD with a FACTOR of -1.0:

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

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

Figure 3.4: 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 3.4: 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 3.5: 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 3.5: Area Model of Beam and Multiple Air Regions

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

An alternative mesh-morphing command, MORPH, is also available. It is generally more robust than DAMORPH, DVMORPH, and DEMORPH and can be used with all element types and shapes. To prepare a non-structural mesh for morphing via MORPH: