Hexahedral Elements

The preferred element for solid bodies in Explicit Dynamics systems is the eight node reduced integration hexahedral. These elements are well suited to transient dynamic applications including large deformations, large strains, large rotations and complex contact conditions. The basic element characteristics are

Connectivity	8 Node
Nodal Quantities	Position, Velocity, Acceleration, Force
	Mass (lumped mass matrix)
Element Quantities	Volume, Density, Strain, Stress, Energy
	Other material state variables
Material Support	All available materials
Points to Note	Preferred element for Explicit Dynamics
	Reduced integration, constant strain element
	Requires hourglass damping to stabilize zero energy "hourglass" modes (see section Damping Controls, Hourglass Damping)

The default Integration Type for hexahedral elements is the Exact option. Here the element formulation based upon the work of Wilkins [8] results in an exact volume calculation even for distorted elements. This formulation is therefore the most accurate option, especially if the faces of the hex elements become warped. This is also computationally the most expensive formulation.

It is possible to speed-up simulations by using the 1pt Gaussian quadrature integrated hexahedral element. This uses the element formulation described by Hallquist [9]. There will be some loss in accuracy when using this formulation with warped element faces which are common place in large deformation analysis.

Tetrahedral Elements

Linear 4 noded tetrahedron elements are available for use in Explicit Dynamic analysis.

Connectivity	4 Node
Nodal Quantities	Position, Velocity, Acceleration, Force
	Mass (lumped mass matrix)
	Additionally ANP formulation: Volume, Pressure, Energy
	Additionally NBS: Volume, Density, Strain, Stress, Energy, Pressure and other material state variables
Element Quantities	Volume, Density, Strain, Stress, Energy
	Other material state variables
	Additionally NBS: If PUSO stability coefficient is set to a non-zero value, there is an additional variable set for all variables for the PUSO solver
Material Support	SCP: All available materials
	Only Isotropic materials can be used with the ANP formulation
	Only ductile materials can be used with the NBS formulation
Points to Note	Only the ANP and NBS are recommended for use in majority tetrahedral meshes
	For NBS models exhibiting zero energy modes, the Puso coefficient can be set to a non-zero value. A value of 0.1 is recommended.
	Reduced integration, constant strain element

The four noded linear tetrahedron is available with three forms of Pressure Integration

The SCP tetrahedral element is a basic, constant strain element and can be used with all the material models. The element is intended as a "filler" element in meshes dominated by hexahedral elements. The element is known to exhibit locking behavior under both bending and constant volumetric straining (that is, plastic flow). If possible the element should therefore not be used in such cases.

The ANP tetrahedral formulation used here is an extension of the advanced tetrahedral element (Burton [11]) and can be used as a majority element in the mesh. The ANP tetrahedral overcomes problems of volumetric locking.

The NBS tetrahedral formulation based on the work of (Bonet [21] and Puso [22]) is a further extension of the ANP tetrahedral element and can also be used as a majority element in the mesh. The NBS tetrahedral overcomes both problems of volumetric and shear locking, therefore is recommended over the other two tetrahedral formulations for models involving bending.

Supported material types in the NBS tetrahedral element are currently limited to ductile materials. The following is a list of supported material properties for NBS tetrahedral elements:

If a model containing NBS tetrahedral elements exhibits zero-energy modes (Puso, 2006 [22]), the PUSO stability coefficient can be set to a non-zero value. The recommended value is 0.1. Stabilization is achieved by taking a contribution to the nodal stresses from the SCP solution. Therefore, for models with a non-zero Puso stability coefficient, the solution is computed on both the nodes and the elements.

NBS tetrahedral elements cannot share nodes with ANP tetrahedral elements, SCP tetrahedral elements, shell elements, or beam elements. Also note that the use of NBS tetrahedral elements with joins or spotwelds is not supported.

Figure 10.7: Comparison of results of a Taylor test solved using SCP, ANP and NBS Tetrahedral elements. Results using NBS and ANP tetrahedral elements compare more favorably with experimental results than results using SCP (see table below).

Tet-SCP	Tet-ANP	Tet-NBS

Figure 10.8: Example bending test using SCP (1), ANP (2), NBS tetrahedral (3), and hex (4) elements. The displacement of the beam with NBS tetrahedral elements is the most similar to the beam meshed with hexahedral elements as it does not exhibit shear locking.

Figure 10.9: Taylor test: Iron cylinder impacting rigid wall at 221m/s. Good correlation between ANP and Hex element results is obtained

Figure 10.10: Example pull out test simulated using both hexahedral elements and ANP tetrahedral elements. Similar plastic strains and material fracture are predicted for both element formulations used.

Pentahedral Elements

Linear 6 noded pentahedral elements are available for use in Explicit Dynamics analysis.

Connectivity	6 Node
Nodal Quantities	Position, Velocity, Acceleration, Force
	Mass (lumped mass matrix)
Element Quantities	All available materials
	Other material state variables
Material Support	All available materials
Points to Note	Reduced integration, constant strain element

The pentahedral element is a basic constant strain element and is intended as a filler element in meshes dominated by hexahedral elements.

Pyramid Elements

Pyramid elements are not recommended for Explicit Dynamics simulations. Any pyramid elements present in the mesh will be converted to 2 tetrahedral elements in the solver initialization phase. Results are mapped back onto the Pyramid element for postprocessing purposes.

Shell Quad Elements

Bilinear 4 noded quadrilateral shell elements are available for use in Explicit Dynamics analysis.

Connectivity	4 Node
Nodal Quantities	Position, Velocity, Angular Velocity, Acceleration, Force, Moment
	Mass (lumped mass matrix)
Element Quantities	Strain, Stress, Energy
	Other material state variables
	Data stored per layer
Material Support	Linear elasticity must be used
	Equations of state and porosity are not applicable to shell elements
	Pressure dependant material strength is not applicable to shell elements
Points to Note	Reduced integration, constant strain element
	Based on Mindlin plate theory, transverse shear deformable
	Shells have zero through thickness stress and are therefore not suitable for modelling wave propagation through the thickness of the surface body

The bilinear 4 noded quadrilateral shell element is based on the corotational formulation presented by Belytschko-Tsay [13]. The element has one quadrature point per layer and is stabilized using hourglass control. By default, additional curvature terms are added for warped elements in accordance with Belytschko [14]. This option is deactivated using the Shell BWC Warp Correction setting in the Solver Controls.

The number of through thickness integration points (sublayers) is controlled through the analysis settings option Solver Controls, Shell Sublayers. The default value is 3.

The thickness of the shell element is updated during the simulation in accordance with the material response. The update is carried out at the shell nodes by default.

The principal inertia of the shell nodes is recalculated every time increment (cycle) by default. This is the most robust method. It is more efficient to rotate the principal inertias rather than recalculate (although less robust for certain applications). The Shell Thickness Update option can be used to select this more efficient inertial update method.

Shell Tri Elements

Linear 3 noded triangular shell elements are available for use in Explicit Dynamics analysis.

Connectivity	3 Node
Nodal Quantities	Position, Velocity, Angular Velocity, Acceleration, Force, Moment
	Mass (lumped mass matrix)
Element Quantities	Volume, Density, Stress, Energy
	Other material state variables
	Data stored per layer
Material Support	Linear elasticity must be used
	Equations of state and porosity are not applicable to shell elements
	Pressure dependant material strength is not applicable to shell elements
Points to Note	Reduced integration, constant strain element
	This element is only recommended for use as a "filler" element in quad dominant shell meshes
	Shells have zero through thickness stress and are therefore not suitable for modelling wave propagation through the thickness of the surface body

The bilinear 3 noded, C0, triangular shell element is based on the formulation presented by Belytschko et al. [15]. The number of through thickness integration points (sublayers) is controlled through the analysis settings option Solver Controls, Shell Sublayers. The default value is 3.

The thickness of the shell element is updated during the simulation in accordance with the material response. The update is carried out at the element irrespective of the global settings for Shell Thickness update in Mechanical.

Beam Elements

Linear 2 noded beam elements are available for use in Explicit Dynamics analysis.

Connectivity	2 Node
Nodal Quantities	Position, Velocity, Angular Velocity, Acceleration, Force, Moment
	Mass (lumped mass matrix)
Element Quantities	Resultant Strain/Stress, Energy
	Other material state variables
Material Support	Linear elasticity must be used
	Equations of state and porosity are not applicable to beam elements
	Pressure dependant material strength is not applicable to beam elements
Points to Note	Supports symmetrical circular, square, rectangular, I-Beam and general cross sections
	Beams have zero transverse stress and are therefore not suitable for modeling wave propagation across the cross section

The 2 noded beam element is based on the resultant beam formulation of Belytschko [16] and allows for large displacements and resultant elasto-plastic response.

SPH Elements

Bodies meshed with the particle method are solved using the Smoothed Particle Hydrodynamics (SPH) method. SPH characteristics are summarized in the table below:

The default values for the SPH options in the analysis settings should be sufficient for most examples, but it may be necessary to change them to improve the accuracy of solutions for certain types of applications.