Finite Elements

MSC Nastran > Building A Model > 2.5 Finite Elements

XXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXX''">XXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXX''">

2.5 Finite Elements

The Finite Elements Application in Patran allows the definition of basic finite element construction. Created under Finite Elements are the nodes, element topology, multi-point constraints, and Superelement.

For more information on how to create finite element meshes, see Mesh Seed and Mesh Forms (p. 25) in the Reference Manual - Part III.

Nodes

Nodes in Patran will generate unique GRID Bulk Data entries in MD Nastran. Nodes can be created either directly using the Node object, or indirectly using the Mesh object. Each node has associated Reference (CP) and Analysis (CD) coordinate frames. The ID is taken directly from the assigned node ID. The X1, X2, and X3 fields are defined in the specified CP coordinate frame. If no reference frame is assigned, the global system is used. The PS and SEID fields on the GRID entry are left blank.

Elements

The Finite Elements Application in Patran assigns element connectivity, such as Quad4, for standard finite elements. The type of MD Nastran element to be created is not determined until the element properties are assigned (for example, shell or 2D solid). See the Element Properties Form, 79 for details concerning the MD Nastran element types. Elements can be created either directly using the Element object, or indirectly using the Mesh object

Multi-point Constraints

Multi-point constraints (MPCs) can also be created from the Finite Elements Application. These are special element types that define a rigorous behavior between several specified nodes. The forms for creating MPCs are found by selecting MPC as the Object on the Finite Elements form. The full functionality of the MPC forms are defined in Create Action (FEM Entities).

MPC Types

To create an MPC, first select the type of MPC to be created from the option menu. The MPC types that appear in the option menu are dependent on the current settings of the Analysis Code and Analysis Type preferences. The following table describes the MPC types which are supported for MD Nastran.


MPC Type	Analysis Type	Description
Explicit	Structural	Creates an explicit MPC between a dependent degree of freedom and one or more independent degrees of freedom. The dependent term consists of a node ID and a degree of freedom, while an independent term consists of a coefficient, a node ID, and a degree of freedom. An unlimited number of independent terms can be specified, while only one dependent term can be specified. The constant term is not allowed in MD Nastran.
RSSCON Surf-Vol	Structural	Creates an RSSCON type MPC between a dependent node on a linear 2D plate element and two independent nodes on a linear 3D solid element to connect the plate element to the solid element. One dependent and two independent terms can be specified. Each term consists of a single node.
Rigid (Fixed)	Structural and Explicit Nonlinear	Creates a rigid MPC between one independent node and one or more dependent nodes in which all six structural degrees of freedom are rigidly attached to each other. An unlimited number of dependent terms can be specified, while only one independent term can be specified. Each term consists of a single node. There is no constant term for this MPC type.
RBAR	Structural and Explicit Nonlinear	Creates an RBAR element, which defines a rigid bar between two nodes. Up to two dependent and two independent terms can be specified. Each term consists of a node and a list of degrees of freedom. The nodes specified in the two dependent terms must be the same as the nodes specified in the two independent terms. Any combination of the degrees of freedom of the two nodes can be specified as independent as long as the total number of independent degrees of freedom adds up to six. There is no constant term for this MPC type.
RBE1	Structural	Creates an RBE1 element, which defines a rigid body connected to an arbitrary number of nodes. An arbitrary number of dependent terms can be specified. Each term consists of a node and a list of degrees of freedom. Any number of independent terms can be specified as long as the total number of degrees of freedom specified in all of the independent terms adds up to six. Since at least one degree of freedom must be specified for each term there is no way the user can create more that six independent terms. There is no constant term for this MPC type.
RBE2	Structuraland Explicit Nonlinear	Creates an RBE2 element, which defines a rigid body between an arbitrary number of nodes. Although the user can only specify one dependent term, an arbitrary number of nodes can be associated to this term. The user is also prompted to associate a list of degrees of freedom to this term. A single independent term can be specified, which consists of a single node. There is no constant term for this MPC type.
RBE3	Structuraland Explicit Nonlinear	Creates an RBE3 element, which defines the motion of a reference node as the weighted average of the motions of a set of nodes. An arbitrary number of dependent terms can be specified, each term consisting of a node and a list of degrees of freedom. The first dependent term is used to define the reference node. The other dependent terms define additional node/degrees of freedom, which are added to the m-set. An arbitrary number of independent terms can also be specified. Each independent term consists of a constant coefficient (weighting factor), a node, and a list of degrees of freedom. There is no constant term for this MPC type.
RROD	Structural	Creates an RROD element, which defines a pinned rod between two nodes that is rigid in extension. One dependent term is specified, which consists of a node and a single translational degree of freedom. One independent term is specified, which consists of a single node. There is no constant term for this MPC type.
RSPLINE	Structural	Creates an RSPLINE element, which interpolates the displacements of a set of independent nodes to define the displacements at a set of dependent nodes using elastic beam equations. An arbitrary number of dependent terms can be specified. Each dependent term consists of a node, a list of degrees of freedom, and a sequence number. An arbitrary number of independent nodes (minimum of two) can be specified. Each independent term consists of a node and a sequence number. The sequence number is used to order the dependent and independent terms with respect to each other. The only restriction is that the first and the last terms in the sequence must be independent terms. A constant term, called D/L Ratio, must also be specified.
RTRPLT	Structural	Creates an RTRPLT element, which defines a rigid triangular plate between three nodes. Up to three dependent and three independent terms can be specified. Each term consists of a node and a list of degrees of freedom. The nodes specified in the three dependent terms must be the same as the nodes specified in the three independent terms. Any combination of the degrees of freedom of the three nodes can be specified as independent as long as the total number of independent degrees of freedom adds up to six. There is no constant term for this MPC type.
Cyclic Symmetry	Structural	Describes cyclic symmetry boundary conditions for a segment of the model. If a cyclic symmetry solution sequence is chosen, such as “SOL 114,” then CYJOIN, CYAX and CYSYM entries are created. If a solution sequence that is not explicitly cyclic symmetric is chosen, such as “SOL 101,” MPC and SPC entries are created. Be careful, for this option automatically alters the analysis coordinate references of the nodes involved. This could erroneously change the meaning of previously applied load and boundary conditions, as well as element properties.
Sliding Surface	Structural	Describes the boundary conditions of sliding surfaces, such as pipe sleeves. These boundary conditions are written to the NASTRAN input file as explicit MPCs. Be careful, for this option automatically redefines the analysis coordinate references of all affected nodes. This could erroneously alter the meaning of previously applied load and boundary conditions, as well as element properties.
RBAR1	Structural	This is an alternate (simplified) form for RBAR. Creates an RBAR1 element, which defines a rigid bar between two nodes, with six degrees of freedom at each end. Each dependent term consists of a node and a list of degrees of freedom, while the independent term consists only of a node (with all six degrees of freedom implied). The constant term is the thermal expansion coefficient, ALPHA.
RTRPLT1	Structural	Alternative format to define a rigid triangular plate element connecting three grid points. Creates an RTRPLT1 element, which defines a rigid triangular plate between three nodes. Each dependent term consists of a node and a list of degrees of freedom, while the independent term consists only of the node (with all six degrees of freedom implied). The constant term is the thermal expansion coefficient, ALPHA.
RJOINT	Structural	Creates an RJOINT element, which defines a rigid joint element connecting two coinciding grid points. Each dependent term consists of a node and a list of degrees of freedom, while the independent term consists only of a node (with all six degrees of freedom implied). There is no constant term for this MPC type.

Degrees of Freedom

Whenever a list of degrees of freedom is expected for an MPC term, a listbox containing the valid degrees of freedom is displayed on the form.

The following degrees of freedom are supported by the Patran MD Nastran MPCs for the various analysis types:


Degree of freedom	Analysis Type
UX	Structural
UY	Structural
UZ	Structural
RX	Structural
RY	Structural
RZ	Structural


Note:	Care must be taken to make sure that a degree of freedom that is selected for an MPC actually exists at the nodes. For example, a node that is attached only to solid structural elements will not have any rotational degrees of freedom. However, Patran will allow you to select rotational degrees of freedom at this node when defining an MPC.

Explicit MPCs

This subordinate MPC form appears when the Define Terms button is selected on the Finite Elements form and Explicit is the selected type. This form is used to create an MD Nastran MPC Bulk Data entry. The difference in explicit MPC equations between Patran and MD Nastran will result in the A1 field of the MD Nastran entry being set to -1.0.

Rigid (Fixed)

This subordinate MPC form appears when the Define Terms button is selected on the Finite Elements form and Rigid (Fixed) is the selected type. This form is used to create an MD Nastran RBE2 Bulk Data entry. The CM field on the RBE2 entry will always be 123456.

RBAR MPCs

This subordinate MPC form appears when the Define Terms button is selected on the Finite Elements form and RBAR is the selected type. This form is used to create an MD Nastran RBAR Bulk Data entry and defines a rigid bar with six degrees of freedom at each end. Both the Dependent Terms and the Independent Terms lists can have either 1 or 2 node references. The total number of referenced nodes, however, must be 2. If either or both of these lists references 2 nodes, then there must be an overlap in the list of referenced nodes.

RBE1 MPCs

This subordinate MPC form appears when the Define Terms button is selected on the Finite Elements form and RBE1 is the selected type. This form is used to create an MD Nastran RBE1 Bulk Data entry.

RBE2 MPCs

This subordinate MPC form appears when the Define Terms button is selected on the Finite Elements form and RBE2 is the selected type. This form is used to create an MD Nastran RBE2 Bulk Data entry.

RBE3 MPCs

This subordinate MPC form appears when the Define Terms button is selected on the Finite Elements form and RBE3 is the selected type. This form is used to create a MD Nastran RBE3 Bulk Data entry.

RROD MPCs

This subordinate MPC form appears when the Define Terms button is selected on the Finite Elements form and RROD is the selected type. This form is used to create an MD Nastran RROD Bulk Data entry.

RSPLINE MPCs

This subordinate MPC form appears when the Define Terms button is selected on the Finite Elements form and RSPLINE is the selected type. This form is used to create an MD Nastran RSPLINE Bulk Data entry. The D/L field for this entry is defined on the main MPC form. This MPC type is typically used to tie together two dissimilar meshes.

RTRPLT MPCs

This subordinate MPC form appears when the Define Terms button is selected on the Finite Elements form and RTRPLT is the selected type. This form is used to create an MD Nastran RTRPLT Bulk Data entry.

Cyclic Symmetry MPCs

The Cyclic Symmetry MPC created by this form will be translated into CYJOIN, CYAX, and CYSYM entries if cyclic symmetric is the selected type, see Solution Parameters, 268, or into SPC and MPC entries if the requested type is not explicitly cyclic symmetric.

Sliding Surface MPCs

The Sliding Surface MPC created by this form will be translated into explicit MPCs in the NASTRAN input file.

RBAR1 MPCs

This subordinate MPC form appears when the Define Terms button is selected on the Finite Elements form and RBAR1 is the selected type. This form is used to create an MD Nastran RBAR1 Bulk Data entry..

RTRPLT1 MPCs

This subordinate MPC form appears when the Define Terms button is selected on the Finite Elements form and RTRPLT1 is the selected type. This form is used to create an MD Nastran RTRPLT1 Bulk Data entry..

RJOINT MPCs

This subordinate MPC form appears when the Define Terms button is selected on the Finite Elements form and RJOINT is the selected type. This form is used to create an MD Nastran RJOINT Bulk Data entry..

Superelements

In superelement analysis, the model is partitioned into separate collections of elements. These smaller pieces of structure, called Superelement, are first solved as separate structures by reducing their stiffness matrix, mass matrix, damping matrix, loads and constraints to the boundary nodes and then combined to solve for the whole structure. The first step in creating a superelement is to create a Patran group (using Group/Create) that contains the elements in the superelement. This group is then selected in the Finite Elements application on the Create/ Superelement form.

Select Boundary Nodes