Explicit Dynamic Analysis

This newly developed OptiStruct Explicit solution type (ANALSIS=NLEXPL) has been developed solely in OptiStruct, in the same way as the OptiStruct implicit solution. The input data (elements, material, property, loading, etc…) for explicit solution is the same as implicit solution and the output data structure is also the same as implicit solution.

Attention: This functionality is different from the existing explicit dynamic analysis through an integration with Altair Radioss (ANALYSIS=EXPDYN).

This solution sequence performs Nonlinear Explicit Finite Element Analysis. The predominant difference between Nonlinear Explicit Finite Element Analysis and Nonlinear Implicit Transient Analysis is the time integration scheme. In Nonlinear Explicit Finite Element Analysis, time step is usually smaller, and no matrix assembly and inversion is required in explicit analysis as compared to implicit approaches. The OptiStruct Nonlinear Explicit solution sequence generally supports all major nonlinear features, for instance, NLSTAT (LGDISP), including Geometric Large Displacement Nonlinearity, Material Nonlinearity, and Contact. Subcase continuation, is currently not supported. Optimization is also currently not supported.

SMP and MPI (DDM) parallelization are supported for OptiStruct Nonlinear Explicit Analysis.

Nonlinearity Sources

Geometric Nonlinearity

In analyses involving geometric nonlinearity, changes in geometry as the structure deforms are considered in formulating the constitutive and equilibrium equations. Many engineering applications require the use of large deformation analysis based on geometric nonlinearity. Applications such as metal forming, tire analysis, and medical device analysis.

Material Nonlinearity

Material nonlinearity involves the nonlinear behavior of a material based on current deformation, deformation history, rate of deformation, temperature, pressure, and so on.

Constraint and Contact Nonlinearity

Constraint nonlinearity in a system can occur if kinematic constraints are present in the model. The kinematic degrees-of-freedom of a model can be constrained by imposing restrictions on its movement. In OptiStruct explicit and MPCs are not supported. For RBE2 and TIE contact, constraints are enforced in a kinematic way.

In the case of contact, the constraint condition is enforced by penalty method.

Auto-contact is available by setting the TYPE field to AUTO on the CONTACT Bulk Data Entry.

Follower Load

Applied loads can depend upon the deformation of the structure when large deformations are involved. Geometrically, the applied loads (Forces or Pressure) can deviate from their initial direction based on how the model deforms at the location of application of load. In OptiStruct, if the applied load is treated as follower load, the orientation and/or the integrated magnitude of the load will be updated with changing geometry throughout the analysis.

Applied loads can be indicated as follower loads using the FLLWER Bulk and Subcase Entries, and/or with the PARAM,FLLWER entry.

Note: Follower loading is currently supported for loads specified via DLOAD/TLOAD#, for all pressure loads, FORCE1, FORCE2, MOMENT1 and MOMENT2.

Explicit Finite Element Analysis Method

In explicit finite element method, the time-discretized equation is solved using explicit time integration method. The explicit time integration method is based on the central difference scheme.

Central Difference Method

In the Central Difference method, the equilibrium equation takes the following form:(1)

M a^{n} = f_{e} (u^{n}, t^{n}) + f_{d} (v^{n}, t^{n}) + f_{c} (u^{n}, t^{n}) + f_{h} (u^{n}, t^{n}) - f_{i} (u^{n}, t^{n})

Where,

$M$: Lumped mass matrix
$f_{e}$ , $f_{d}$ , $f_{c}$ , $f_{h}$ and $f_{i}$: Are the external force, damping force, contact force, hourglass force and element internal force vectors, respectively.
$a^{n}$: Computed directly from the equilibrium equation.

From

a^{n}

velocity and displacement vectors can be updated as:(2)

v^{n + \frac{1}{2}} = v^{n - \frac{1}{2}} + \frac{1}{2} (t^{n + \frac{1}{2}} - t^{n - \frac{1}{2}}) a^{n}

(3)

d^{n + 1} = d^{n} + (t^{n + 1} - t^{n}) v^{n + \frac{1}{2}}

Where,

$t^{n}$: Current time
$t^{n + 1}$: Next time

The following time increments are defined:(4)

Δ t^{n} = t^{n + 1} - t^{n}

(5)

Δ t^{n - 1} = t^{n} - t^{n - 1}

Then,(6)

v^{n + \frac{1}{2}} = v^{n - \frac{1}{2}} + \frac{1}{2} (Δ t^{n - 1} + Δ t^{n}) a^{n}

(7)

d^{n + 1} = d^{n} + Δ t^{n} v^{n + \frac{1}{2}}

Critical Time Step

Unlike implicit nonlinear transient analysis, explicit time integration scheme is conditionally stable.

The explicit solution marches forward in time. The time-step at each time increment is calculated automatically by default (elemental time step is the default), and can be switched between elemental and nodal time step using the TYPE field of the TSTEPE Bulk Data Entry. The DTMIN field on TSTEPE Bulk Data Entry can be used to specify a minimum allowed nodal time increment. The top ten smallest critical timesteps (elemental/nodal) are printed in the .out file by default for Explicit Dynamic Analysis. This can be controlled using PARAM, CRTELEM.

Elemental Time Step

This is the default time step control type for Nonlinear Explicit Analysis. The TYPE field on TSTEPE entry is set to ELEM by default.

Solid Elements
The time step size should satisfy:(8) $Δ t \leq \frac{2}{ω_{\max}}$

Where, $ω_{\max}$ denotes the maximum natural frequency of the system.

For solid elements, a critical time step size is computed from:(9) $Δ t_{e} = \frac{l_{e}}{Q + {(Q^{2} + c^{2})}^{\frac{1}{2}}}$

Where,

$c$

Adiabatic sound speed

$Q$

Afunction of the bulk viscosity coefficients $C_{0}$ and $C_{1}$

(10) $Q = C_{1} c + C_{0} l_{e} \max (0, - {\dot{ε}}_{k k})$

Where,

$C_{0}$ and $C_{1}$

Bulk viscosity coefficients, are dimensionless constants with default values of 1.5 and 0.06, respectively.

$l_{e}$

Element characteristic length.

8 node hexahedron

(11) $l_{e} = \frac{V_{e}}{A_{e_{\max}}}$

10 node tetrahedron

(12) $l_{e} = \frac{1}{{(B_{i j} B_{i j})}^{\frac{1}{2}}}$

6 node pentahedron

(13) $l_{e} = \frac{1}{{(B_{i j} B_{i j})}^{\frac{1}{2}}}$

4 node tetrahedron

(14) $l_{e} = \frac{3 V_{e}}{A_{e_{\max}}}$

Where,

$B_{i j}$

Symmetric gradient of shape function

$V_{e}$

Volume of the hexahedron element

$A_{e_{\max}}$

Maximum area among all the six faces of the hexahedron element
Shell Elements
For shell elements, the time step size is determined by:(15) $Δ t = \frac{L}{c}$

Where, $c$ is the speed of sounds, which is calculated as:(16) $c = \sqrt{\frac{E}{ρ (1 - ν^{2})}}$

Where,

$E$

Young's modulus

$ρ$

Density

$ν$

Poisson's ratio

$L$

Characteristic length, which is calculated as for quadrilateral elements:

$L = \frac{A}{\max (L_{1}, L_{2}, L_{3}, L_{4})}$

Where,

$A$

Area

$L_{1}, L_{2}, L_{3}, L_{4}$

Lengths of the sides of the trianagle elements:

$L = \frac{2 * A}{\max (L_{1}, L_{2}, L_{3})}$

Where,

$A$

Area

$L_{1}, L_{2}, L_{3}$

Lengths of the sides of the element
Elemental Mass Scaling
The elemental mass can be scaled to increase $Δ t_{e}$ , if the scaled elemental critical time step (scaled by DTFAC), falls below DTMIN. This is possible since the elemental time step equation contains the speed of sound term ( $c$ ), which is dependent on material density ( $ρ$ ).
Spring Elements
For spring elements (lumped spring-mass system) there is no wave propagation speed to calculate the critical time-step size.

The eigenvalue problem for the free-vibration of a spring with nodal masses, $m_{1}$ and $m_{2}$ , and stiffness, $k$ , is:(17) $[\begin{matrix} k & - k \\ - k & k \end{matrix}] [\begin{matrix} u_{1} \\ u_{2} \end{matrix}] - ω [\begin{matrix} m_{1} \\ m_{2} \end{matrix}] [\begin{matrix} u_{1} \\ u_{2} \end{matrix}] = [\begin{matrix} 0 \\ 0 \end{matrix}]$

Since the determinant of the characteristic equation should equal zero, the maximum eigenvalue can be solved for:(18) $| \begin{matrix} k - ω^{2} m_{1} & - k \\ - k & k - ω^{2} m_{2} \end{matrix} | = 0$ Where, $ω_{\max}^{2} = \frac{k (m_{1} + m_{2})}{m_{1} \cdot m_{2}}$ .

Based on the critical time-step of a truss element:

$Δ t \leq \frac{l}{c}$ and $ω_{\max} = \frac{2 c}{l}$ , you can write:(19) $Δ t \leq \frac{2}{ω_{\max}}$

Approximating the spring masses by using half of the actual modal mass, you obtain:(20) $Δ t = 2 \sqrt{\frac{m_{1} m_{2}}{m_{1} + m_{2}} \frac{1}{k}}$

Therefore, in terms of the nodal mass, the critical time step size can be written:(21) $Δ t_{e} = \sqrt{\frac{2 m_{n 1} m_{n 2}}{m_{n 1} + m_{n 2}} \frac{1}{k}}$

This does not take damping into consideration. If damping is defined, the time step is scaled by:(22) $Δ t_{e} = \sqrt{\frac{2 m_{n 1} m_{n 2}}{m_{n 1} + m_{n 2}} \frac{1}{k}} (\sqrt{1 - ξ^{2}} - ξ)$

Where,

$m_{n 1}$ and $m_{n 2}$

Nodal masses.

$k$

Stiffness in the corresponding degree of freedom.

$ξ = \frac{c}{c_{c r}} = \frac{c}{2 m ω}$

$c$

Damping coefficient (for CBUSH elements, it is defined via the Bi fields of the PBUSH Bulk Data Entry).

Nodal Time Step

The time step control can be switched from the default elemental time step to nodal time step by setting the TYPE field on TSTEPE Bulk Entry to NODA.

The nodal time step is calculated as:(23)

Δ t_{n} = \sqrt{\frac{2 m_{n}}{k_{n}}}

Where,

$m_{n}$: Nodal mass
$k_{n}$: Nodal stiffness (which is calculated from the elemental stiffness)

Nodal stiffness is calculated as:

For each element, the critical time step,

Δ t_{e}

is calculated first, and each node is assumed to have the same time step,

Δ t_{e}

, then for each node, you can estimate the nodal stiffness from this equation.(24)

Δ t_{e} = \sqrt{\frac{2 m_{e_{i}}}{k_{e_{i}}}}

Where,

$i$: The i-th node of the element
$m_{e_{i}}$: Nodal mass of the i-th node
$k_{e_{i}}$: Nodal stiffness of the i-th node of this element

Therefore, the nodal stiffness of the i-th node is:(25)

k_{e_{i}} = \frac{2 m_{e_{i}}}{Δ t_{e}^{2}}

The final nodal stiffness is:(26)

k_{n} = \sum_{e} k_{e_{i}}

Using $k_{n}$ , the nodal critical time step $Δ t_{n}$ can be calculated.

Nodal Mass Scaling

The nodal mass $m_{n}$ can be scaled to increase $Δ t_{n}$ , if the scaled nodal critical time step (scaled by DTFAC), falls below DTMIN.

Hourglass Control

Hourglass control can be activated using PARAM,HOURGLS or HOURGLS entries. These entries also provide access to adjust hourglass control parameters (HGTYP and HGFAC).

If the HOURGLS entry is input, then it should be chosen via HGID field on the corresponding Property entry to be activated. HOURGLS entry via HGID field overwrites the settings defined via PARAM,HOURGLS.

For Solid Elements

For solid elements with MAT1/MATS1 material, two types of hourglass control are provided:

Type 1 (Flanagan and Belytschko, 1981) resists undesirable hourglass modes with viscous damping.
Type 2 (Puso, 2000), uses an enhanced assumed strain physical stabilization to provide coarse mesh accuracy with computational efficiency. Type 2 is chosen as the default hourglass type for MAT1/MATS1 material for 1st order CHEXA elements.

The implementations of Type 1 and Type 2 hourglass controls are very similar, except that the hourglass forces are calculated in a different manner.

Note: Type 2 is more computationally intensive; however, performs better in eliminating Hourglass modes, when compared to Type 1. The only limitation of Type 2 is that it may lead to an overly stiff response in bending problems with large plastic deformation.

For MATHE entry, the default hourglass control is Type 4 (Reese, 2005). Type 2 is also available for MATHE entries.

In case of reduced integration for solid elements (ISOPE=URI/AURI), hourglass control is turned on by default.

	Hourglass Control (Solid Element-based)
Elements	Regular Elements (`ISOPE`=FULL)	Regular Elements (`ISOPE`=URI)	Regular Elements (`ISOPE`=AURI)	Regular Elements (`ISOPE`=SRI)
CHEXA (1st order)	Hourglass control is not required	Hourglass Control is turned ON by default. ¹ For MAT1/MATS1 Hourglass Type 2 For MATHE Hourglass Type 4	Hourglass Control is turned ON by default. ¹ The defaults are: For MAT1/MATS1 Hourglass Type 2 For MATHE Hourglass Type 4	Hourglass control is not required
CPENTA (1st order)	NA	NA	NA	NA

For Shell Elements

For shell elements, only two types of hourglass control are provided:

Type 1 (Flanagan and Belytschko – viscous form)
Type 2 (Flanagan and Belytschko – stiffness form). Type 2 is chosen as the default hourglass type for MAT1/MATS1 material for CQUAD4.

	Hourglass Control (Shell Element-based)
Elements	Belytschko-Tsay (`ISOPE`=BT)	Belytschko-Wong-Chiang with full projection (`ISOPE`=BWC)
CQUAD4	Hourglass Control is turned ON by default. ¹ For MAT1/MATS1 Hourglass Type 2	Hourglass Control is turned ON by default. ¹ For MAT1/MATS1 Hourglass Type 2

Materials

The following table shows the various Hourglass control types and defaults for supported materials.

	Hourglass Control (Material-based)
Materials	Type 1 Solids and Shells: Flanagan-Belytschko Viscous Form	Type 2 Solids: Puso Enhanced Assumed Strain Stiffness Form Shells: Flanagan-Belytschko Stiffness Form	Type 4 Solids: Reese Hourglass Control Shells: Type 4 is not supported for shells
MAT1/MAT2/MAT8/MATS1	Available ²	Default ⁶	NA
MATHE	NA	Available ²	Default ⁶
MATVE	NA	Available ²	Default ⁶

Adaptive Dynamic Relaxation

Dynamic relaxation can be used to solve static or quasi-static problems using an Explicit Dynamic Analysis, by avoiding dynamic oscillations. Compared to an implicit analysis, it could be more efficient and robust in some cases with high nonlinearities (e.g. with many complicated contacts). Examples of typical applications include 3-point bending simulations of phone structures and spring back simulation in sheet metal forming.

Unlike conventional dynamic relaxation which requires at least one input, OptiStruct supports adaptive dynamic relaxation via the DYREL entry, for which no input parameters are needed. The damping factor is automatically determined based on the system’s highest natural frequency.

Problem Setup

Input

Activation:
A Nonlinear Explicit Subcase can be identified via ANALYSIS=NLEXPL. The TTERM Subcase Entry is mandatory to define the termination time. Additionally, a TSTEPE Subcase entry which points to the corresponding TSTEPE Bulk Data Entry is also available for Nonlinear Explicit Analysis. If TSTEPE Subcase Entry is not defined, then ANALYSIS=NLEXPL is mandatory in conjunction with TTERM. Otherwise, TTERM and TSTEPE together is sufficient to identify the Explicit Nonlinear subcase. Nonlinear Explicit Analysis is always large displacement analysis.
Initial Conditions:
The initial conditions can be defined using IC Subcase Entry and in conjunction with the TIC Bulk Data Entry.
Loading:
Loads can be defined using LOAD, DLOAD, and TLOAD# Bulk Data Entries which should be referenced in the subcase using DLOAD Subcase Entry. For reference via LOAD Subcase Entry or TLOAD# Bulk Entry, only the FORCE, FORCE1, FORCE2, MOMENT, MOMENT1, MOMENT2, PLOAD2, PLOAD4, GRAV, ACCEL2, and SPCD entries are supported for loading.
Boundary Conditions:
Boundary Conditions can be applied via SPC Bulk Data which are referenced by a corresponding SPC subcase entry. MPCs are not supported currently.
Supported Elements:

Solid Elements

4-noded CTETRA, 10-noded CTETRA, 8-noded CHEXA, and 6-noded CPENTA elements are supported.

Shell Elements

CTRIA3 and CQUAD4 are supported.

One-dimensional Elements

CBUSH, CBEAM, and CBAR elements are supported.

Currently, only Belytschko-Schwer Beam formulation is supported for CBAR/CBEAM 1D elements in Explicit Analysis.

Mass Elements

CONM2 is supported.
Note:
- Offset, on elements or property for Shell elements is supported for Explicit Analysis.
- In case of CBUSH elements, Mi fields in PBUSH definition will be used for mass and inertia calculations. Refer to PBUSH in the Reference Guide for more details.
- For CBEAM, CBAR elements,
  - The continuation lines on PBEAM/PBAR are not supported with Explicit Analysis.
  - Pin flags (PA and PB) are supported with Explicit Analysis.
Supported Materials:
MAT1, MAT2, MAT8, MATS1, MATHE, and MATVE materials are supported. The MATVE entry should be defined under MATHE entry.
Integration Schemes:
For explicit analysis, the element integration scheme can be changed using the ISOPE field on the PSOLID, PLSOLID, PSHELL, PCOMP, PCOMPG, PCOMPP entries, or via PARAM,EXPISOP. The settings on the ISOPE field will overwrite the settings on PARAM,EXPISOP.

Example:

SUBCASE 10
   ANALYSIS=NLEXPL
   SPC = 1
   DLOAD = 2
   TSTEPE = 2
   NLOUT = 23
   IC = 12
   TTERM = 2.0
.
.
BEGIN BULK
TSTEPE,2,ELEM,0.8
NLOUT,23,NINT,12
IC,12,33,3,0.2
SPC,1,45,123,0.0
TLOAD1,2,3,,0,8
TABLED1,8
+,0.0,0.0,2.0,8.0,ENDT,ENDT

Output

The typical output entries (DISPLACEMENT, VELOCITY, and ACCELERATION) can be used to request corresponding output for Nonlinear Explicit Analysis. The NLOUT Subcase and Bulk Data Entries can be used to request intermediate results, only with NINT parameter support.

The NLOUT Bulk Data Entry and NLOUT Subcase Information Entry can be used to control incremental output. For Nonlinear Explicit Analysis, only the NINT field is supported for NLOUT. The NLADAPT entry is not supported for Nonlinear Explicit Analysis, and no other TSTEP# entries are supported, except TSTEPE entry.

Currently, only Hyper3D (_expl.h3d) and HyperGraph presentation format (_expl.mvw) files are supported. Nonlinear Explicit Analysis results are not output to the regular .h3d and .mvw files, but instead are output to _expl.h3d and _expl.mvw files, respectively.

_expl.h3d: Contours for Displacement, Rotation, Velocity, Acceleration, Strain, Strain rate (in case of rate dependent plasticity), Stress, Plastic Strain, CBUSH element force, Composite stress, Composite Strain and Composite failure index are output.
_expl.mvw: This session file automatically loads the corresponding _expl.h3d file and allows you to plot the results output in the _expl.h3d file.
_s<ID>_e.expl: Curves for Internal energy, Elastic Contact energy, Plastic Contact energy, Kinetic energy, Hourglass energy, and Plastic Dissipation energy are output
_expl_energy.mvw: This session file automatically loads the corresponding _s<ID>_e.expl file and allows you to plot the various energy output.
.out: For explicit, the .out file contains Time Cycle information (based on PARAM,NOUTCYC), Current time, Current Time Step, Maximum Strain Energy, Element ID for which the information is printed, Kinetic Energy, Contact Work, Total Energy, Maximum Penetration, Node ID associated with this maximum penetration, Maximum Normal Work, Node ID associated with this Maximum Normal Work, Mass Change Ratio. which is the information regarding the scaled mass change after mass scaling – this is calculated as: (current mass-original mass)/(original mass).
_expl.cntf: An ASCII file that contains the contact force output results on the main surface and is activated when the OPTI format is specified in the CONTF I/O Options Entry. The output includes Normal/Tangential Force, Magnitude and Area of contact. This output is available for each explicit time-step.; The frequency of output in this file can be controlled using the NINT field in the NLOUT entry.
_TH.h5: Time history output for Explicit Dynamic analysis is available in a _TH.h5 file HDF5 format file. In some situations, a subset of results (for example, energy) is required to be output at a high output frequency. But increasing output frequency in NLOUT would affect all results, leading to enormous file size and this may be undesired. Time history output is a useful and effective solution for such cases.; For more details regarding supported results, kindly refer to the THIST bulk data entry.

Table 1. Nonlinear Explicit Analysis Quick Summary
Nonlinear Explicit Analysis	Subcase or I/O	Bulk Data	Comments
Activation:
Subcase Type	ANALYSIS=`NLEXPL` (optional)	NA	If TSTEPE is not specified, then ANALYSIS=`NLEXPL` is mandatory.
Nonlinear Explicit Activation	TTERM (mandatory) TSTEPE (optional)	TSTEPE (optional)	If TSTEPE is not specified, then ANALYSIS=`NLEXPL` is mandatory.
Loads:
Nodal Loads	LOAD, DLOAD	If LOAD in subcase is used: FORCE, FORCE1, FORCE2, MOMENT, MOMENT1, and MOMENT2. If DLOAD in subcase is used: TLOAD1 or TLOAD2. DLOAD can be used to combine multiple TLOADi data. For nodal loads, `EXCITEID` on TLOADi data can be FORCE, FORCE1, FORCE2, MOMENT, MOMENT1, and MOMENT2.	`TYPE` field on TLOADi data can be set to 0 or LOAD for this case.
Surface Loads	LOAD, DLOAD	If LOAD in subcase is used: PLOAD2 and PLOAD4. If DLOAD in subcase is used: TLOAD1 or TLOAD2. DLOAD can be used to combine multiple TLOADi data. For Surface loads, `EXCITEID` on TLOADi data can be PLOAD1 and PLOAD4.	`TYPE` field on TLOADi data can be set to 0 or LOAD for this case.
Body Loads	LOAD, DLOAD	If LOAD in subcase is used: GRAV and ACCEL2. If DLOAD in subcase is used: TLOAD1 or TLOAD2. DLOAD can be used to combine multiple TLOADi data. For Body loads, `EXCITEID` on TLOADi data can be GRAV and ACCEL2.	`TYPE` field on TLOADi data can be set to 0 or LOAD for this case.
Enforced Displacement, Velocity, Acceleration	LOAD, DLOAD	If LOAD in subcase is used: Enforced displacement, velocity, or acceleration using SPCD or SPCD. If DLOAD in subcase is used: TLOAD1 or TLOAD2. DLOAD can be used to combine multiple TLOADi data. For Enforced loading, `EXCITEID` on TLOADi data can be SPC or SPCD.	`TYPE` field on TLOADi data can be set to: 1 or DISP For enforced displacement, 2 or VELO For enforced velocity, 3 or ACCE For enforced acceleration.
Follower Loading	FLLWER	FLLWER PARAM,FLLWER	Loads can be chosen as follower loads, similar to implicit nonlinear analysis. Follower loading is currently supported for loads specified via DLOAD/TLOAD#, for all pressure loads, FORCE1, FORCE2, MOMENT1 and MOMENT2.
Boundary Conditions:
Single Point Constraints	SPC	SPC
Initial Conditions:
Initial Displacement	TIC	IC
Initial Velocity	TIC	IC
Time Step Control:
Basic time controls	TSTEPE	TSTEPE	`TYPE` field on TSTEPE entry to choose between elemental and nodal time step controls. `DTMIN` field can define minimum time step below which nodal/elemental mass scaling is activated. `DTFAC` field can define scale factor for stable time increments.
Mass Elements:
Mass Elements Support		CONM2 is supported
Structural Elements:
Supported Structural Elements	NA	One-dimensional elements: CBUSH, CBEAM, and CBAR are supported; Shells CTRIA3 and CQUAD4 elements. Solids 4-noded CTETRA, 10-noded CTETRA, 8-noded CHEXA, and 6-noded CPENTA elements.
Integration Schemes	NA	`ISOPE` field on PSOLID, PLSOLID, or PSHELL. PARAM,EXPISOP (parameter is only supported for solid elements).	`ISOPE` field will overwrite settings defined on PARAM,EXPISOP. Refer to Elements in the User Guide for more details regarding Integration Schemes.
Constraints:
Support for Rigids	NA	RBE2, RBE3 and RBODY are supported.
Materials:
Supported Materials	NA	Shells: MAT1, MAT2, MAT8 and MATS1. Solids: MAT1, MATS1, MATVE, and MATHE.	For MATS1: In addition to materials on MATS1 supported for implicit, we also support Johnson-Cook and crushable foam materials. For MATHE: All material models listed in MATHE are supported with solid elements.
Properties:
Supported Properties	NA	PSHELL, PSOLID, PLSOLID, PCOMP, PCOMPG, PCOMPP	PLY, STACK and DRAPE entries are supported.
Contact:
Supported Contact Types	NA	CONTACT and TIE	N2S and S2S contact discretization are supported. SMALL, FINITE, and CONSLI contacts are supported. Auto-Contact is supported by setting the `TYPE` field to AUTO on CONTACT Bulk Data Entry. For TIE in explicit: 1 Only kinematic TIE is supported. That is, the kinematic condition is precisely constrained instead of using the penalty-based method. 2 Hierarchy in kinematic TIE is not supported (that is, secondary node of a TIE cannot be the main node in another TIE). 3 Overconstrained TIEs are ignored (only the first constraint for such cases, based on the order of input in the .fem file, is retained). 4 All such hierarchy and over constrained TIE nodes are printed into grid SET in the *_badtied.fem file.
Coordinate Systems:
Supported User-defined Coordinate Systems	NA	CORD2R, CORD1C, CORD2C, CORD1S, and CORD2S
Output:
ASCII Output	NA	PARAM,NOUTCYC	Only explicit time cycle summary and corresponding information like Time steps, Energy, Maximum Penetration, Mass Change Ratio, and so on are printed to the .out file.PARAM,NOUTCYC can be used to choose the frequency of summary output in the .out file.
Binary File Output	DISP, VELOCITY, ACCELERATION, STRESS, STRAIN (includes Plastic Strain), Strain rate for rate dependent plasticity problems, CBUSH, FORCE, CSTRESS, CSTRAIN, CFAILURE, ESE	NA	Results are output only to the _expl.h3d and _expl.mvw files. _expl.h3d The displacement, rotation, velocity, acceleration, stress, strain, strain rate (for rate dependent plasticity problems), CBUSH force, plastic strain composite stress, composite strain and composite failure index results output. _expl.mvw Automatically loads the corresponding _expl.h3d file and allows you to plot the results output in the _expl.h3d file. _s<ID>_e.expl Contains curves for Internal energy, Elastic Contact energy, Plastic Contact energy, Kinetic energy, Hourglass energy, and Plastic Dissipation energy output. _expl_energy.mvw Automatically loads the corresponding _s<ID>_e.expl file and allows you to plot the various energy output. ESE output is available with COMP and OCOMP group options, only in the .h3d format. THIST can be used to generate time history output for certain results in a _TH.h5 file.
Output Control	NLOUT, THIST	NLOUT, THIST	Only the `NINT` field is supported for Explicit Analysis. The NLADAPT entry is not supported for Nonlinear Explicit Analysis.
Miscellaneous:
Large Displacement	NA	NA	Explicit Nonlinear Analysis is large displacement nonlinear analysis by default.
Adaptive Dynamic Relaxation	DYREL	NA
Hourglass Control		HOURGLS (`HGID` field references this card on PSOLID/PLSOLID/PSHELL) PARAM,HOURGLS	The default hourglassing values are overwritten by HOURGLS entry referenced on PSOLID/PLSOLID/PSHELL entry or PARAM,HOURGLS. `HGID` via HOURGLS entry overwrites PARAM,HOURGLS. For more information, refer to Hourglass Control.
Optimization:
Optimization Support	Not Supported	Not Supported		Not Supported

¹ The defaults can be overwritten by user-defined PARAM,HOURGLS or HOURGLS entry (referenced by HGID on property entry)

² Users can turn on hourglass control using PARAM,HOURGLS or HOURGLS entry (referenced by HGID on property entry)

³ For solid elements, ISOPE field on PSOLID/PLSOLID entries can be used to switch between integration schemes

⁴ Hourglass control is not applicable for CTETRA (1st and 2nd order)

⁵ For shell elements, ISOPE field on PSHELL entry can be used to switch between integration schemes

⁶ The defaults can be overwritten by user-defined PARAM,HOURGLS or HOURGLS entry (referenced by HGID on property entry). Note that for MAT1/MATS1/MATHE, the defaults only apply in the case of 1st order CHEXA elements. For CPENTA elements, the user should turn ON hourglass control, if required.

⁷ Some materials listed here are not supported for shells (for instance, MATHE and MATVE)