1D Meshing
1D mesh that allows accurate testing of connectors, such as bolts, and similar rodlike or barlike objects that can be modeled as a simple line for FEA purposes.
1D Elements
Supported 1D elements.
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.
Type  Type Name  Number of Nodes  Orientation  Solver Interface 

1  Spherical joint  2 


2  Revolute joint  4 

LSDYNA 
3  Cylindrical joint  4 

LSDYNA 
4  Planar joint  4 

LSDYNA 
5  Universal joint  4 

LSDYNA 
6  Translational joint  6 

LSDYNA 
7  Locking joint  6 

LSDYNA 
8  Ball joint  2  None  OptiStruct 
9  Fixed joint  2  None  OptiStruct 
10  Revolute joint  2 

OptiStruct 
11  Translational1 joint  2 

OptiStruct 
12  Cylindercal 1 joint  2 

OptiStruct 
13  Universal joint  2 

OptiStruct 
14  Constant_velocity joint  2 

OptiStruct 
15  Planar joint  2 

OptiStruct 
16  Inline joint  2 

OptiStruct 
17  Perpendicular joint  2 

OptiStruct 
18  Parallel axes joint  2 

OptiStruct 
19  Inplane joint  2 

OptiStruct 
20  Orient joint  2 

OptiStruct 
21  Point_to_curve joint  2 

OptiStruct 
22  Curve_to_curve joint  2 

OptiStruct 
23  Point_to_deformable_curve joint  2 

OptiStruct 
24  Point_to_deformable_surface joint  2 

OptiStruct 
25  Translational_2N joint  2 

PAMCRASH 
26  Revolute_2N joint  2 

PAMCRASH 
27  Cylindrical_2N joint  2 

PAMCRASH 
28  Universal_2N joint  2 

PAMCRASH 
29  FlexionTorsion joint  2 

PAMCRASH 
30  Planar_2N joint  2 

PAMCRASH 
31  General joint  2 

PAMCRASH 
32  Bracket joint  2 

PAMCRASH 
33  Free joint  2 

PAMCRASH 
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 userdefined 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.
Rigidlink Elements
Configuration 55  Rigid elements with one independent node and variable dependent nodes typically used to model rigid bodies.
Rigidlink elements have userdefined degrees of freedom which apply to all dependent nodes.
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 userdefined degrees of freedom, an orientation vector, and a property reference.
 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.
 Spring4N
 1D elements with 4 nodes used to model spring connections.
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.