Basic Concepts and Definitions

XXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXX''">XXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXX''">

Following are several topics that include basic concepts and definitions related to the Finite
Elements application.

Finite elements themselves are defined by both their topology (i.e., their shape) and their properties. For example, the elements used to create a mesh for a surface may be composed of quadrilaterals or triangles. Similarly, one element may be a steel plate modeling structural effects such as displacement and rotation, while another may represent an air mass in an acoustic analysis. Both the shapes and properties supported depend upon the analysis program you are using with Patran, as defined in your Analysis Preferences.

At this stage of using Patran, where you are creating a finite element mesh using the Finite Elements application form, elements are defined purely in terms of their topology. Other properties such as materials, thickness and behavior types are then defined for these elements in subsequent applications, and discussed in later chapters of this guide.

The table below describes the element topologies supported by Patran. The columns in the table provide the following information:

• The left-hand column lists seven element shapes and illustrates each with a common node configuration.

• The Structural Uses column describes typical usage conditions for the element shapes. For example, use Bar-shaped elements if you plan to define the element properties as bars, springs, or gap elements.

• The Mesher Support column indicates which mesher-node configuration combinations are supported for each element shape.

A complete description of the Patran element library, including numbering conventions and parametric coordinates, is available in Part 4 of the Patran Reference Manual.

There are four basic mesh generation techniques available in Patran: IsoMesh, Paver Mesh, Auto TetMesh, and 2-1/2D Meshing. This section describes each meshing technique. Selecting the right technique for a particular model must be based on geometry, model topology, analysis objectives, and engineering judgment.

This approach creates elements within a regularly shaped region of geometry via simple subdivision.

Some key features of the Isomesh approach are as follows:

Element Shape	Node Configurations and Mesh Techniques Supported	Structural Uses
Point			Use Point for a concentrated mass, spring, or damper to ground.
Bar		Isomesh supports Bar1, Bar2, and Bar4 elements.	Use Bar when the stress state varies in one dimension, and when properties of the element are defined along a curve or straight line.
Tria		Isomesh and Paver support Tria3, 4, 6, 7, 9, and 13 elements.	Use Tria and Quad when the stress state varies in two dimensions and is constant in the third. You can also use Tria and Quad when one dimension of the area to be modeled is very small in comparison to the other two.
Quad		Isomesh and Paver support Quad4, 5, 8, 9, 12, and 16 elements.
Tet		Isomesh supports Tet4, 5, 10, 11, 14, 15, 16, and 40 elements. Tet Mesh - Tet4, 10, and 16.	Use Tet, Wedge and Hex when the stress state varies in all three dimensions, and all three dimensions of the area to be modeled are comparable. Patran supports a variety of node configurations for each of these elements.
Wedge		Isomesh supports Wedge6, 7, 15, 16, 20, 21, 24, and 52 elements.
Hex		Isomesh supports Hex8, 9, 20, 21, 26, 27, 32, and 64 elements.

• It requires regular regions of surface or solid geometry. Surface regions must have three or four sides, while solid regions may contain five or six faces.

• By default, it creates a consistent number of elements in each direction, based on a parameter known as the Global Edge Length. Element density and spacing can be controlled via the use of mesh seeds, which can also be used to create a different element densities on opposing edges or faces of a region.

• For so-called "degenerate" regions, such as triangular surfaces or wedge-shaped solids, where one edge or face is collapsed, appropriate degenerate Tria or Wedge elements are created at the degenerate point or edge.

The Paver is an automated surface meshing technique that you can use with any arbitrary surface region, including trimmed surfaces, composite surfaces, and irregular surface regions. Unlike the IsoMesh approach, the Paver technique creates a mesh by first subdividing the surface boundaries into mesh points, and then operates on these boundaries to construct interior elements.

Some of its key features are:

• It can be used to create Quad or Tria element meshes. Quad meshes can contain some triangles, due to the nature of the approach.

• Either mesh seeds or the Global Edge Length parameter on its meshing form are used to control element density.

• The Paver method accommodates associated geometry, such as a curve lying on a surface which has been associated with that surface using the Associate/Curve/Surface option of the Geometry application form. If such a curve has mesh seeds assigned to it, the Paver ensures that the mesh passes through these mesh seed points.

• Adjacent regions can be meshed with either the Paver or IsoMesh approach. The mesh density along a common edge becomes a default mesh density for that edge of the adjacent region.

The Auto TetMesh approach is a highly automated technique for meshing arbitrary solid regions of geometry. It creates a mesh of tetrahedral (4-noded solid) elements for any closed solid, including boundary representation (B- rep) solids, as well as regular solid regions.

Some key features are:

• Tetmeshing is a valid technique for meshing boundary representation solids, such as solid models imported from most CAD systems.

• Curvature-based meshing creates high quality meshes in curved regions. You can specify the density of the mesh in curved regions relative to the global element size.

A planar 2D mesh can also be transformed to produce a 3D mesh of solid elements, using sweep and extrude operations.

Important points to note are:

• The direction and element density in the sweep or extrude direction can be specified with this 2D to 3D transformation approach.

• This technique produces elements that maintain no associativity with any parent geometry. This prevents subsequent loads, boundary conditions and properties from being assigned via geometric entities for these elements.

To generate a mesh, Patran must know what size of elements to use for each region of the geometry. Moreover, you may wish to adjust the number of elements upward or downward for a specific area of the model. For example, you may want to increase the number of elements in an area of high stress or temperature to get a more accurate result, or decrease the number of elements in a less critical region to improve the analysis run time.

There are several tools available in Patran for controlling your mesh size and density, including mesh seeds, mesh density, and mesh density of adjacent regions. These tools combine to allow rapid meshing of geometric model, while providing a high degree of control over the nature of your finite element mesh.

When you create a mesh in Patran, the mesh density along each edge of a region is chosen according to the following order of precedence:

Mesh seeds are points explicitly defined along an edge of your model to specify where node locations will be along that edge. These seeds can be uniform, or vary linearly towards either end, both ends, or the center of the edge. You can even specify specific individual locations for mesh seeds along an edge.

These mesh seeds are created using the Create/Mesh Seeds option on the Finite Elements application form, with methods including Uniform, Bias, Curve Based, and Tabular. Like other Patran entities, these mesh seeds can also be redefined using a subsequent Create option, or deleted using Delete/Mesh Seeds.

When you create a mesh in a geometry region, the mesh density created along an edge will normally be used in the meshing of any adjacent regions sharing that edge. In addition, Patran uses a concept of mesh paths to guide the subdivision of geometry regions when using the IsoMesh approach.

Simply put, Patran projects a specified mesh density to the opposing edge of a region, and then to an adjacent region, until it reaches the end of a "path." The figure shown here displays the path of the specified mesh densities, and how they affect the meshing of the overall model.

Each variation of the Create/Mesh form contains a parameter called Global Edge Length that defines the approximate length of each element edge. Patran uses this parameter to subdivide each boundary edge of your model into an integer number of elements yielding elements closest to this edge value, using
the relationship:

When there are no other constraints on mesh size, such as mesh seeds or adjacent meshes, the Global Edge Length is used to define the mesh size.

Many geometry models in Patran consist of multiple regions sharing common boundaries. Finite element meshing in Patran is always performed one region at a time, even when multiple geometric regions are selected in the meshing form.

This means that by default, the elements of one region are not connected to the elements of another region, and would not share behavior across their nodes. To quickly correct this, Patran provides a feature known as equivalencing to join together nodes at common locations. This feature can be accessed via the Equivalence action on the Finite Elements application form.

The equivalencing operation itself is very straightforward; each node is checked for neighboring nodes within a specified tolerance value. If two or more nodes are within this tolerance, they are combined as one node containing the lowest numbered node number. The following figure shows the equivalencing process.

Important:	Set this value explicitly whenever you perform a meshing operation. The default value found upon entering this form can result in an extremely dense mesh, if it is very small relative to the dimensions of your geometry.

Important:	Equivalencing must be explicitly performed by you prior to analysis. Failure to equivalence generally produces invalid analysis results: for example, unconnected regions which are free to fly off into space in a structural analysis. Patran does not automatically inform you that regions have not been equivalenced prior to an analysis.

You have the option of equivalencing all nodes in a region, or just those nodes corresponding to a specified group or list, as discussed in Chapter 2 of this guide. Once the requested nodes are equivalenced, all references to the original higher numbered nodes (such as element definitions, loads, and boundary conditions) are automatically changed within Patran to reflect the new equivalenced
node numbers.

The equivalencing option allows you to select nodes to exclude from equivalencing. This is useful for cases where there are coincident nodes that you wish to keep physically separate. In addition, the value and measurement technique for the equivalencing tolerance value can be set using the
Equivalence action.

No matter how your finite element model is created--either by meshing or by direct finite element modeling operations--there is one short, painless operation that can speed up your analysis substantially. This operation, known as optimization, simply renumbers your nodes or elements to decrease the run time of the problem.

In an analysis, terms from each finite element combine to form a symmetric matrix that is sparse, containing many zero terms. As part of solving this matrix equation, by essentially inverting the matrix, many finite element solvers have a solution time that varies with the bandwidth of the matrix. The bandwidth is the maximum width of non-zero terms from the matrix diagonal. The figure below shows what this bandwidth looks like physically within the matrix equation.

Other solvers are based on a similar criteria of wavefront, based on the number of active columns in a matrix row. By renumbering nodes or elements, the rows and columns of the matrix can be rearranged to reduce this bandwidth or wavefront, optimizing your run time. In Patran, the Optimize action from the Finite Elements application form performs this optimization, based on analysis-specific criteria documented in Part 4 of the Patran Reference Manual.