The program automatically generates the target/contact elements and supported surface-effect elements if the underlying solid elements are remeshed, then transfers all applied boundary conditions (BCs) and loads to the new mesh. Use plot or list commands to verify that the newly generated target/contact elements, surface-effect elements, and the transferred BCs and loads, are complete and correct.
For further information, the following topics are available:
After the contact boundaries, surface-effect elements, loads, and boundary conditions have been applied and verified, proceed to Step 6: Map Variables and Balance Residuals.
Rigid target elements cannot be remeshed. They are automatically transferred from the original mesh to the new mesh.
Deformable target elements and all contact elements are always attached to solid elements; therefore, provided that the underlying solid elements are remeshed, the program creates the target/contact elements automatically after exiting remeshing (REMESH,FINISH). the program passes all specified element options, real constants, and materials from the old target/contact elements to the new ones automatically.
Verify that the new elements on the contact boundary are complete and correct.
Surface-effect elements (SURF153 and SURF154) are always attached to solid elements; therefore, provided that the underlying solid elements are remeshed, the program creates the surface-effect elements automatically after exiting remeshing (REMESH,FINISH). The program passes all specified element options from the old surface-effect elements to the new ones automatically.
Verify that the new surface-effect elements on the boundary, and the transferred BCs and loads, are complete and correct.
Only normal and tangential pressures applied on SURF153 and SURF154 are supported. (That is, rezoning support is available only for pressure on faces 1 and 2 for SURF153 and pressure on faces 1, 2 and 3 for SURF154.)
During remeshing, if you are using a program-generated new mesh, the program maintains the nodes on the boundary of the region where pressures or contiguous displacements are applied. If you are using a generic new mesh created by another application, you must maintain the nodes manually.
In 2D problems, the boundary consists of only the starting and ending points. In 3D problems, the boundary can be a line of ordered nodes representing a line bounding a set of facets.
You can redistribute nodes inside the region (between starting and ending points). If you do so, the program uses linear interpolation to apply the pressures and displacements at the new node locations. If the starting and ending points are rotated, the new nodes are also rotated with the angle determined by linear interpolation of the angles of the old nodes. If the original distribution is not linear, the interpolation may introduce a small degree of error, although the error should not be significant if both the original mesh and the new mesh are sufficiently dense.
The following illustration shows how the displacements are applied before and after remeshing.
If a force or isolated (applied only at one node) displacement is applied at a node, the program maintains that node, its rotation angle (if any), and the applied forces and displacements, during rezoning.
The program transfers only nodal temperatures applied via the BF command to the new nodes (by interpolation with shape functions) from the old nodes.
If the remeshed region crosses the boundary where one side has old nodes with applied temperatures and the other side does not, the interpolation may cause different temperature distributions at the new nodes close to the boundary. Therefore, avoid remeshing the region crossing the boundary and use horizontal rezoning instead.
When higher-order elements are used, the interpolated temperatures can exceed the maximum value or fall below the minimum value. The behavior is due to the nature of the shape functions of the higher-order elements. The effects of this limitation are minimized when both the old and new meshes are sufficiently refined.
Any other loads and boundary conditions (such as coupling and constraint equations) are not valid in the remeshed region and are lost during rezoning, which may result in a solution that does not converge or a solution that is very different from the one expected.