Line Meshing

Bar Elements

1D elements created in a space between two or three nodes of a model where beam properties are desired.

The nodes are related to each other based on the properties of the bar or beam element connecting them. Properties associated with bar elements include vector orientation, offset vectors that end at A and B, or at A, B, and C, and pin flags to tell it what degree of freedom should carry through the beam.

Bar elements are displayed as a line between two nodes with BAR2 or BAR3 written at the centroid of the element.

Bar2: Configuration 60 - 1D (1st order) elements with 2 nodes used to model axial, bending, and torsion behavior. Bar2 elements have a property reference, an orientation vector, offset vectors and ends A and B, and pin flags at ends A and B.
Bar3: Configuration 63 - 1D (2nd order) elements with 3 nodes used to model axial, bending, and torsion behavior. Bar3 elements have a property reference, an orientation vector, offset vectors and ends A and B, and pin flags at ends A and B.

Gap Elements

Configuration 70 - 1D elements created in a space between two nodes, or between a node and an element, of a model where contact may occur.

Create a gap element when you want to impose a nonlinear constraint on a model; this constraint will limit the amount of movement possible during analysis.

Gap elements have a property reference and an orientation vector.

Gap elements are displayed as a line between two nodes with GAP written at the centroid of the element.

Gap elements can translate to CGAP or CGAPG elements in OptiStruct, CGAP element in Nastran or *GAP option in Abaqus.

Joint Elements

Configuration 22 - 1D elements with 2, 4, or 6 nodes which have a property and orientation systems or nodes.

Joint element is a definition of a connection between two rigid bodies. Joint elements store a property and orientation information.

Joint elements are displayed with lines between the appropriate nodes and the letter J between nodes 1 and 3 of the element.

Only certain types of elements can be used to create joint elements. The type of the element controls the number of nodes used in the element and the permissible orientations of the element.

Table 1. Types of Joint Elements
Type	Type Name	Number of Nodes	Orientation	Solver Interface
1	Spherical joint	2	None Systems Nodes	LS-DYNA PAM-CRASH
2	Revolute joint	4	None Systems	LS-DYNA
3	Cylindrical joint	4	None Systems	LS-DYNA
4	Planar joint	4	None Systems	LS-DYNA
5	Universal joint	4	None Systems	LS-DYNA
6	Translational joint	6	None Systems	LS-DYNA
7	Locking joint	6	None Systems	LS-DYNA
8	Ball joint	2	None	OptiStruct
9	Fixed joint	2	None	OptiStruct
10	Revolute joint	2	Node Vector Coordinates	OptiStruct
11	Translational1 joint	2	Node Vector Coordinates	OptiStruct
12	Cylindercal 1 joint	2	Node Vector Coordinates	OptiStruct
13	Universal joint	2	Node Vector Coordinates	OptiStruct
14	Constant_velocity joint	2	Node Vector Coordinates	OptiStruct
15	Planar joint	2	Node Vector Coordinates	OptiStruct
16	Inline joint	2	Node Vector Coordinates	OptiStruct
17	Perpendicular joint	2	Node Vector Coordinates	OptiStruct
18	Parallel axes joint	2	Node Vector Coordinates	OptiStruct
19	Inplane joint	2	Node Vector Coordinates	OptiStruct
20	Orient joint	2	Node Vector Coordinates	OptiStruct
21	Point_to_curve joint	2	Node Vector Coordinates	OptiStruct
22	Curve_to_curve joint	2	Node Vector Coordinates	OptiStruct
23	Point_to_deformable_curve joint	2	Node Vector Coordinates	OptiStruct
24	Point_to_deformable_surface joint	2	Node Vector Coordinates	OptiStruct
25	Translational_2N joint	2	None Systems	PAM-CRASH
26	Revolute_2N joint	2	None Systems	PAM-CRASH
27	Cylindrical_2N joint	2	None Systems	PAM-CRASH
28	Universal_2N joint	2	None Systems	PAM-CRASH
29	Flexion-Torsion joint	2	None Systems	PAM-CRASH
30	Planar_2N joint	2	None Systems	PAM-CRASH
31	General joint	2	None Systems	PAM-CRASH
32	Bracket joint	2	None Systems	PAM-CRASH
33	Free joint	2	None Systems	PAM-CRASH

Plot Elements

Configuration 2 - 1D elements with 2 nodes used for display purposes.

Plot elements are displayed as a line between two nodes.

RBE3 Elements

Configuration 56 - Rigid elements with one dependent node and variable independent nodes typically used to define the motion at the dependent node as a weighted average of the motions at the independent nodes.

Both the dependent node and independent nodes contain a coefficient (weighting factor) and user-defined degrees of freedom. The dependent degrees of freedom and weighting factors can be specified or automatically calculated based on the geometry.

RBE3 elements are displayed as lines between the dependent node and the independent node(s) with RBE3 displayed at the dependent node of the element.

RBE3’s are typically used to distribute loads applied on the dependent node amongst the selected independent nodes.

Note: The dependent node cannot be directly constrained, as this would lead to a double-dependency for that node.

Rigidlink Elements

Configuration 55 - Rigid elements with one independent node and variable dependent nodes typically used to model rigid bodies.

Rigidlink elements have user-defined degrees of freedom which apply to all dependent nodes.

Rigidlink elements can be created with dependent nodes attached to an element as a SET. If a rigid link with a dependent node set is deleted, the associated node set is also deleted. If the dependent node set is deleted, the connected rigid link element is also deleted. Dependent node sets are automatically created when rigid link elements are created. A node set can be connected as a set of dependent nodes to a rigid link element independent node.

Note: Two-node rigids with a dependent node set attached are always created as rigid link elements

Rigidlink elements are displayed as lines between the independent node and the dependent node(s) with RL displayed at the independent node of the element.

Rigid Elements

Configuration 5 - Rigid 1D elements with 2 nodes used to model rigid connections.

Rigid elements are displayed as a line between two nodes with the letter R written at the centroid of the element.

Rigids can translate to RBE2 in Nastran or *MPC in Abaqus.

Rod Elements

Configuration 61 - 1D elements with 2 nodes used to model axial behavior only.

The two nodes are related to each other based on the properties of the rod element connecting them. Rod elements have property pointers.

Rod elements are displayed as a line between two nodes with ROD written at the centroid of the element.

Rods can translate to CTUBES in Nastran or a C1D2 element in Abaqus.

Spring Elements

Configuration 21 - 1D elements used to model spring connections.

Spring elements have user-defined degrees of freedom, an orientation vector, and a property reference.

Spring elements are displayed as a line between two nodes with the letter K written at the centroid of the element.

Spring: 1D elements with 2 nodes used to model spring connections.
Spring2N: 1D elements with 2 nodes used to model spring connections.
Spring3N: 1D elements with 3 nodes used to model spring connections.; The third node serves as the direction node.
Spring4N: 1D elements with 4 nodes used to model spring connections.; This type of element will mostly be considered as joints, based on the property it is assigned.

Springs can translate to CELAS2 in Nastran or *SPRING in Abaqus.

Weld Elements

Configuration 3 - Rigid 1D elements with 2 nodes used to model welded connections.

Weld elements are displayed as a line between two nodes with the letter W written at the centroid of the element.