If you decide that the generated mesh is not appropriate, you can easily change the mesh by one of the following methods:
Remesh with new element size specifications.
Use the accept/reject prompt to discard the mesh, then remesh.
Clear the mesh, redefine mesh controls, and remesh.
Refine the mesh locally.
Improve the mesh (for tetrahedral element meshes only).
Details of these methods are discussed below.
You can remesh a meshed model by resetting element size controls and initiating the meshing operation (AMESH or VMESH). This is the simplest way to change your mesh. The accept/reject prompt is not required, and the mesh does not need to be cleared in order to remesh it.
However, there are some restrictions to using this method. You can change element size specifications controlled by the KESIZE, ESIZE, SMRTSIZE, and DESIZE commands, but you cannot change size specifications assigned directly to lines (LESIZE). If you want the option of changing LESIZE settings before remeshing, use the mesh accept/reject prompt instead of this method.
This remesh option is available only when meshing is performed interactively through the GUI. If you are using command input, you must first clear the mesh before remeshing (see Clearing the Mesh for more information).
As mentioned earlier, you can activate the mesh accept/reject prompt in the GUI by picking before meshing. (The prompt is turned off by default.) When activated, the prompt appears after each meshing operation and allows you to either accept or reject the generated mesh. If the mesh is rejected, all nodes and elements will be cleared from the meshed entities. You can then reset any of the meshing controls and remesh the model.
The accept/reject prompt is available for area and volume meshing. The advantage of using the prompt is that you do not have to manually clear the mesh (ACLEAR and VCLEAR).
Clearing the mesh of nodes and elements is not always required before remeshing. However, you do have to clear the mesh in order to respecify LESIZE settings. You also have to clear the mesh if you want to change the underlying solid model.
For more information on the clearing operation, see Clearing a Mesh of this manual.
If you are generally satisfied with a mesh but would like to have more elements in a particular region, you can refine the mesh locally around selected nodes (NREFINE), elements (EREFINE), keypoints (KREFINE), lines (LREFINE), or areas (AREFINE). The elements surrounding the chosen entities will be split to create new elements. You control the refinement process by specifying:
The level of refinement to be done (in other words, the desired size of the elements in the refinement region, relative to the size of the original elements)
The depth of surrounding elements that will be remeshed, in terms of the number of elements outward from the selected entity
The type of postprocessing to be done after the original elements are split (smoothing and cleaning, smoothing only, or neither)
Whether triangles can be introduced into the mesh during the refinement of an otherwise all-quadrilateral mesh
You can access local mesh refinement in the GUI by picking . You can also do overall refinement by using the command ESEL,ALL or by picking the menu path . See Revising Your Model of this manual for details on refining a mesh locally.
The tetrahedral mesh improvement feature enables you to improve a given tetrahedral mesh. The program performs this improvement through face swapping, node smoothing, and other techniques that it uses to reduce the number of poorly-shaped tetrahedral elements (in particular, the number of sliver tetrahedral elements) - as well as the overall number of elements - in the mesh. It also improves the overall quality of the mesh.
In many cases, you won't need to take any action to obtain the benefits offered by the tetrahedral mesh improvement feature. As described earlier in Controlling Tetrahedral Element Improvement, the program invokes the feature automatically as a postprocessing step of its volume meshers. Tetrahedral mesh improvement also occurs automatically during the creation of transitional pyramid elements (described in Creating Transitional Pyramid Elements) and the refinement of tetrahedral element meshes (described in Revising Your Model).
Although tetrahedral mesh improvement often occurs automatically, there are certain situations in which you'll find it useful to request additional improvement for a given tetrahedral mesh:
When tetrahedra improvement is invoked automatically during a volume meshing operation (VMESH), the program uses a linear tetrahedral shape metric for improvement. This means that the program ignores midside nodes that may be present within the elements. However, when you request tetrahedra improvement of a given mesh as documented below, the program takes the midside nodes into account. Thus, for meshes of quadratic (midside-node) tetrahedral elements, requesting additional tetrahedra improvement (VIMP) after the mesh is created (VMESH) can help to remove, or at least reduce, the number of element shape test warning messages that are produced and to improve the overall quality of the mesh.
Since imported tetrahedral meshes have not received the benefits of the tetrahedral mesh improvement that the program often performs automatically, imported tetrahedral meshes are likely candidates for user-invoked improvement.
Tetrahedral mesh improvement is an iterative process. Each time that processing completes, a special window appears to report the improvement statistics from that iteration, along with diagnostic messages. If you want to try to improve the mesh further, you can reissue your request repeatedly, until either the statistics indicate a satisfactory mesh, or until it converges and no more noticeable improvement is made.
You can request improvement of two types of tetrahedral elements:
Use the TIMP command to improve tetrahedral elements that are not associated with a volume. Typically, this option is useful for an imported tetrahedral mesh for which no geometry information is attached.
Use the VIMP command to improve tetrahedral elements that are in a selected volume or volumes. You might want to use this option to further improve a volume mesh created with the VMESH command.
The following restrictions apply to tetrahedral mesh improvement:
The mesh must consist of either all linear elements or all quadratic elements.
For all of the elements in the mesh to be eligible for tetrahedral mesh improvement, they must all have the same attributes, including element type. (The element type must be tetrahedral, but the tetrahedral elements may be the degenerated form of hexahedral elements.) After tetrahedral mesh improvement, the program reassigns the attributes from the old set of elements to the new set of elements.
Note: Tetrahedral mesh improvement is possible in a mesh of mixed element shapes (as opposed to types). For example, as stated earlier, improvement occurs automatically during the creation of transitional pyramid elements at the interface between hexahedral and tetrahedral element types. However, in a mixed mesh, only the tetrahedral elements are improved.
Loading has an effect on whether tetrahedral mesh improvement is possible. Tetrahedral mesh improvement is possible when loading occurs in either of these ways:
When loads have been applied to the element faces or nodes on the boundary of the volume only
When loads have been applied to the solid model (and have been transferred to the finite element mesh)
Tetrahedral mesh improvement is not possible when loading occurs in either of these ways:
When loads have been applied to the element faces or nodes within the interior of a volume
When loads have been applied to the solid model (and have been transferred to the finite element mesh), but have also been applied to the element faces or nodes within the interior of a volume
Note: In the last two loading situations, the program issues a warning message to notify you that you must remove the loads if you want tetrahedral mesh improvement to occur.
If node or element components are defined, you are prompted whether you want to proceed with mesh improvement. If you choose to proceed, you must update any affected components.
Other characteristics of tetrahedral mesh improvement include:
Element numbering and node numbering are modified.
Generally, if the program encounters an error or a user abort occurs, it leaves the mesh unchanged. However, the program may save a partially improved mesh after an abort if you verify the save when the program prompts you. If you have requested improvement for multiple volumes (VIMP), the abort applies only to the current volume mesh that is being improved. All previously improved volume meshes are already saved. (The same applies when an error occurs after the first of multiple volumes is improved.)
See the TIMP and VIMP command descriptions for more information.