Creating a Finite Element Model

Patran Users Guide > Finite Element Meshing > Creating a Finite Element Model

XXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXX''">XXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXX''">

To create the finite elements mesh, Patran supports a variety of element shapes and node configurations, and its mesh creation tools include several automated meshing techniques.

The Finite Element Application Form

The Finite Elements application form provides numerous Action/Object/Type combinations that create, modify, and qualify the finite elements model to facilitate valid analysis results.

To use the Finite Element Application form:

1. Click the FE (Elements) application button on the Patran Main form.

The Finite Elements application form appears in your viewport.

2. Select an Action, Object, and Type using the drop-down menus at the top of the form.

The rest of the form varies depending on what you select for these menus.

Actions

The actions create, modify, and qualify all of your mesh related objects. The table that follows describes the action choices for the Finite Element application.


	Action Descriptions
	Create Actions
Create	Creates a variety of new mesh-related entities: a mesh generated by one of the automated mesh techniques, mesh seeds to vary the density of the mesh, individually designed elements and nodes, and additional objects.
Transform	Creates nodes and elements by translating, rotating, or mirroring existing ones.
Sweep	Creates new mesh elements by sweeping a set of existing elements along one of ten path types, such as Arc, Extrude, Glide, Glide-Guide, and Normal. Sweep can convert a surface (2D) mesh into a solid (3D) mesh by sweeping it along a normal perpendicular to the surface.
	Modify Actions
Modify	Modifies one or more attributes of entities such as nodes, elements, and multipoint constraints. This can include renumbering nodes and elements, splitting one into two or more elements, and more. Modify can also be used to optimize element shapes and modify the arrangement of mesh seeding.
Delete	Removes entities from the model, such as nodes, elements, and mesh seed definitions.
Renumber	Modifies the ID numbering of elements or nodes.
Associate/ Disassociate	Modifies nodes and elements so that they are either associated with or disassociated from geometric structures. To apply loads, boundary conditions, and properties directly to the geometry, mesh entities must be associated with geometric entities.
	Qualify Actions
Verify	Provides numerous quality tests for the finite element model, including checks of element distortion, element duplication, and node/element ID numbering.
Equivalence	Improves the finite element model by eliminating duplicate nodes, either at the same location or within the Equivalencing Tolerance distance.
Optimize	Minimizes the CPU time, memory, and disk space needed to solve the stiffness matrix portion of the analysis, by renumbering the nodes or elements in the model. The optimization method varies, depending on the analysis model, type, and code in use.
Show	Displays a variety of information about finite element objects. For example, for selected groups of elements, shows coordinate systems, IDs, load and boundary conditions, material property ID number, element properties, and associated results.

Objects

The Objects are your mesh related entities. These include items such as a mesh, individual nodes, and elements. The table that follows describes the Objects you may choose on the Finite Elements application form.


	Object Descriptions
Mesh	The finite element method requires that you divide the analysis model into interconnected pieces called elements, to which separate analysis equations are assigned. A set of these interconnected elements is referred to as a mesh.
Mesh Seed	Mesh seeds are points that can be explicitly defined along an edge of your model, to specify where node locations will be along that edge. These seeds can be uniform, specified at individual locations, or vary linearly towards either end, both ends, or the center of the edge.
Mesh Control	Mesh control allows you to specify a particular global edge length for selected surfaces for use with any of the auto meshers. This option allows you to create meshes with transition without having to do so one surface at a time.
Node	A node is the finite element model equivalent of a vertex in geometry. Nodes are the connection points between adjacent elements.
Element	An element is one discrete piece of a mesh; it may be one of several standard shapes such as quad and tetrahedral, and can have different numbers of node points along its edges.
MPC (multipoint constraint)	MPCs are a substitute for finite elements that you can use more easily to model certain physical phenomena, such as rigid links, joints (revolutes, universal, etc.), and sliders, to name a few. MPCs are treated as elements in Patran; they display as lines between nodes.
Superelement	This object is currently available only for the MD Nastran analysis preference. It groups several elements as one large element.

Types

Type specifies how the mesh action is carried out. The choices for Type vary according to the Object you selected. A few examples are shown in the following sections. For a complete listing, please refer to the Patran Reference Manual, Volume 2, Part 4: Finite Element Modeling.

Sample Finite Element Forms and Subforms

Three sample Finite Element Modeling forms are shown on the following pages:

• The form for the selection Create/Mesh/Solid.

• The Isomesh Parameters subform.

• The form for Create/Mesh Seed/Two-Way Bias.

Create/Mesh/Solid Form

Meshing is the process of automatically creating finite elements from geometry or other element data in Patran. It is controlled using the FEM Create/Mesh form, shown in the following illustration.


Node ID List and Element ID List	Assigns an optional list of ID numbers for a new set of nodes and elements. If not specified, ID values will be assigned consecutively starting with the node and element ID shown.
Global Edge Length	Specifies a real value to assign the default element edge length for a given mesh. This value does not override any predefined mesh seeded edges. Global edge lengths will only be applied where mesh seeds have not been defined.
Mesher	Specifies which mesh technique to use.
Isomesh Parameters...	Brings up the Isomesh Parameters form that enables you specify the Isomesh application parameters.
Node Coordinate Frames...	This allows an Analysis and a Reference Coordinate system to be defined for the next mesh of nodes.
Element Topology	Choose the type of element to create from the given list. Available elements to choose from here are Hex6, Hex9, and Hex20.
Solid List	Specifies solids to mesh by either cursor selecting existing solids, or by specifying the solid IDs.

IsoMesh Parameters Subordinate Form

This form appears when the IsoMesh Parameters button is selected on the Finite Elements application form.


Isomesh on Triangular Surfaces	Defines the mesh patterns for degenerate surfaces or solids.
Tri Pattern on Retang Surfaces	Defines the mesh patterns for surfaces or solids with 90 degree corners only.
Isomesh Smoothing Parameters	Controls how the Isomesher handles transitions between regions with different numbers of elements.

Sample Create/Mesh Seed/Two Way Bias

Create mesh seed definition for a given curve, or an edge of a surface or solid, with a symmetric nonuniform element edge length, specified either by a total number of elements with a length ratio, or by actual edge lengths. The mesh seed is represented by small yellow circles displayed only when the Finite Element applications form is set to creating a Mesh, or creating or deleting a Mesh Seed.


Display Existing Seeds	Plots all defined mesh seeds associated with the visible geometry
Element Edge Length Data	Patran calculates the nonuniform mesh seed node spacing through a geometric progression based on the given L2⁄L1 ratio.
• Num Elems and L2⁄L1	Specifies that you will enter an integer value for the desired number of elements and an edge length ratio as indicated by the diagram.
• L1 and L2	Specifies that you will enter edge lengths for the end and middle elements.
Curve List	Specifies a list of edges by either cursor selecting existing curves or surface or solid edges, or specifying curve IDs or surface or solid edge IDs. For example, Curve 10, Surface 12.1, Solid 22.5.2.)

Direct Finite Element Modeling

The vast majority of finite element modeling performed today is via operations on geometric modeling, one or more pieces of geometry are created, and then a mesh and properties are generated. In other cases, however, it may be easier to work directly with the nodes and elements themselves.
Such cases might include:

• Modifying a mesh read in from an analysis program, such as an MD Nastran bulk data file.

• Finite element models whose meshes are created via an external software application, without an underlying geometry model.

• Changing specific elements that fail verification tests.

It is preferable to mesh a geometric model where possible, from a standpoint of both modeling time and assignment of properties. When properties are assigned directly to geometry, the mesh can later be modified without needing to re-assign these properties. Conversely, properties assigned directly to nodes and elements may need to be re-entered if the underlying mesh is changed.

Direct finite element modeling tools in Patran include the following:

• Create actions that create nodes, elements, MPCs (Multi-Point Constraints), and superelements.

• Transform actions that create nodes and elements via Transform, Rotate and Mirror operations on existing nodes and elements.

• Sweep actions that create higher order elements by sweeping lower order elements through a path, as described above under 2-1/2D mesh generation.

• Modify actions that smooth an existing mesh, edit element and node ID or attribute values, split existing Bar, Quad or Tria elements, or modify MPC attributes.