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, and so on) for explicit solution is the same as implicit solution and the output data structure is also the same as implicit solution.
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, Geometric Large Displacement Nonlinearity, Material Nonlinearity, and Contact. Subcase continuation, is currently not supported.
SMP, MPI (DDM), and hybrid parallelization are supported for OptiStruct Nonlinear Explicit Analysis. Single precision and double precision executables are both supported for OptiStruct 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 degreesoffreedom of a model can be constrained by imposing restrictions on its movement. For RBE2, RBE3, MPC, and TIE contact, constraints are enforced in a kinematic way by default. RBE3, MPC and TIE switch to penalty approach if overconstraints are detected.
In the case of contact, the constraint condition is enforced by penalty method.
Autocontact 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.
Explicit Finite Element Analysis Method
In explicit finite element method, the timediscretized 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:
 $M$
 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:
 ${t}^{n}$
 Current time
 ${t}^{n+1}$
 Next time
The following time increments are defined:
Then,
Critical Time Step
Unlike implicit nonlinear transient analysis, explicit time integration scheme is conditionally stable.
The explicit solution marches forward in time. The timestep 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
 Solid Elements
The time step size should satisfy:
$$\text{\Delta}t\le \frac{2}{{\omega}_{\mathrm{max}}}$$Where, ${\omega}_{\mathrm{max}}$ denotes the maximum natural frequency of the system.
For solid elements, a critical time step size is computed from:
$$\text{\Delta}{t}_{e}=\frac{{l}_{e}}{Q+{\left({Q}^{2}+{c}^{2}\right)}^{\raisebox{1ex}{$1$}\!\left/ \!\raisebox{1ex}{$2$}\right.}}$$Where, $c$
 Adiabatic sound speed
 $Q$
 A function of the bulk viscosity coefficients ${C}_{0}$ and ${C}_{1}$
$$Q={C}_{1}c+{C}_{0}{l}_{e}\mathrm{max}\left(0,{\dot{\epsilon}}_{kk}\right)$$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

$${l}_{e}=\frac{{V}_{e}}{{A}_{{e}_{\mathrm{max}}}}$$
 10 node tetrahedron

$${l}_{e}=\frac{1}{{\left({B}_{ij}{B}_{ij}\right)}^{{\scriptscriptstyle \frac{1}{2}}}}$$
 6 node pentahedron

$${l}_{e}=\frac{1}{{\left({B}_{ij}{B}_{ij}\right)}^{{\scriptscriptstyle \frac{1}{2}}}}$$
 4 node tetrahedron

$${l}_{e}=\frac{3{V}_{e}}{{A}_{{e}_{\mathrm{max}}}}$$
Where, ${B}_{ij}$
 Symmetric gradient of shape function
 ${V}_{e}$
 Volume of the hexahedron element
 ${A}_{{e}_{\mathrm{max}}}$
 Maximum area among all the six faces of the hexahedron element
 Shell Elements
For shell elements, the time step size is determined by:
$$\text{\Delta}t=\frac{L}{c}$$Where, $c$ is the speed of sounds, which is calculated as:
$$c=\sqrt{\frac{E}{\rho \left(1{\nu}^{2}\right)}}$$Where, $E$
 Young's modulus
 $\rho $
 Density
 $\nu $
 Poisson's ratio
 $L$
 Characteristic length, which is calculated as for quadrilateral elements:
Where, $A$
 Area
 ${L}_{1},{L}_{2},{L}_{3},{L}_{4}$
 Lengths of the sides of the triangle elements:
 Spring Elements
For spring elements (lumped springmass system) there is no wave propagation speed to calculate the critical timestep size.
The eigenvalue problem for the freevibration of a spring with nodal masses, ${m}_{1}$ and ${m}_{2}$ , and stiffness, $k$ , is:
$$\left[\begin{array}{cc}k& k\\ k& k\end{array}\right]\left[\begin{array}{c}{u}_{1}\\ {u}_{2}\end{array}\right]\omega \left[\begin{array}{cc}{m}_{1}& \\ & {m}_{2}\end{array}\right]\left[\begin{array}{c}{u}_{1}\\ {u}_{2}\end{array}\right]=\left[\begin{array}{c}0\\ 0\end{array}\right]$$Since the determinant of the characteristic equation should equal zero, the maximum eigenvalue can be solved for:
$$\left\begin{array}{cc}k{\omega}^{2}{m}_{1}& k\\ k& k{\omega}^{2}{m}_{2}\end{array}\right=0$$Where, ${\omega}_{\mathrm{max}}^{2}=\frac{k\left({m}_{1}+{m}_{2}\right)}{{m}_{1}\cdot {m}_{2}}$ .Based on the critical timestep of a truss element:
$\text{\Delta}t\le \frac{l}{c}$ and ${\omega}_{\mathrm{max}}=\frac{2c}{l}$ , you can write:
$$\text{\Delta}t\le \frac{2}{{\omega}_{\mathrm{max}}}$$Approximating the spring masses by using half of the actual modal mass, you obtain:
$$\text{\Delta}t=2\sqrt{\frac{{m}_{1}{m}_{2}}{{m}_{1}+{m}_{2}}\frac{1}{k}}$$Therefore, in terms of the nodal mass, the critical time step size can be written:
$$\text{\Delta}{t}_{e}=\sqrt{\frac{2{m}_{n1}{m}_{n2}}{{m}_{n1}+{m}_{n2}}\frac{1}{k}}$$This does not take damping into consideration. If damping is defined, the time step is scaled by:
$$\text{\Delta}{t}_{e}=\sqrt{\frac{2{m}_{n1}{m}_{n2}}{{m}_{n1}+{m}_{n2}}\frac{1}{k}}\left(\sqrt{1{\xi}^{2}}\xi \right)$$Where, ${m}_{n1}$ and ${m}_{n2}$
 Nodal masses.
 $k$
 Stiffness in the corresponding degree of freedom.
 $\xi =\frac{c}{{c}_{cr}}=\frac{c}{2m\omega}$
 $c$
 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:
 ${m}_{n}$
 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, $\text{\Delta}{t}_{e}$ is calculated first, and each node is assumed to have the same time step, $\text{\Delta}{t}_{e}$ , then for each node, you can estimate the nodal stiffness from this equation.
 $i$
 The ith node of the element
 ${m}_{{e}_{i}}$
 Nodal mass of the ith node
 ${k}_{{e}_{i}}$
 Nodal stiffness of the ith node of this element
Therefore, the nodal stiffness of the ith node is:
The final nodal stiffness is:
Using ${k}_{n}$ , the nodal critical time step $\text{\Delta}{t}_{n}$ can be calculated.
Mass Scaling
 Elemental Mass Scaling
The elemental mass can be scaled to increase $\text{\Delta}{t}_{e}$ , 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 ( $\rho $ ).
 Nodal Mass Scaling
The nodal mass ${m}_{n}$ can be scaled to increase $\text{\Delta}{t}_{n}$ , if the scaled nodal critical time step (scaled by DTFAC), falls below DTMIN.
 Mass Scaling Controls
Mass scaling in a succeeding Explicit Dynamic Analysis subcase can be controlled through the MSCALE Subcase Information Entry. When MSCALE is not defined, the mass scaling will continue from the preceding Explicit Dynamic Analysis subcase.
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
 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.
For MATHE entry, the default hourglass control is Type 4 (Reese, 2005). Type 2 is also available for MATHE entries.
Hourglass Control (Solid Elementbased)  

Elements  Regular Elements (ISOPE=FULL)  Regular Elements (ISOPE=URI)  Regular Elements (ISOPE=SRI) 
CHEXA
(1st order) 
Hourglass control is not required  Hourglass Control is turned ON by default. ^{1}

Hourglass control is not required 
CPENTA
(1st order) 
Hourglass control is not required  Hourglass control is not required  Hourglass control is not required 
For Shell Elements
 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.
Materials
Hourglass Control (Materialbased)  

Materials  Type 1 Solids and Shells: FlanaganBelytschko Viscous Form 
Type 2 Solids: Puso Enhanced Assumed Strain Stiffness Form Shells: FlanaganBelytschko 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 quasistatic 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 (for example, with many complicated contacts). Examples of typical applications include 3point 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.
Material Failure Criterion
Material failure criterion can be defined using the MATF Bulk Data Entry or the MATS1 Bulk Data Entry (for damage initiation/evolution criteria only). Failure of materials is strongly influenced by the loading conditions and thus, the stress state. Hence, several criteria available refer to the notions of stress triaxiality and optionally to the Lode parameter to describe the loading conditions (uniaxial tension, pure shear, plane strain etc).
To describe a failure criterion based on plasticity and stress states, the value stress triaxiality, $\eta $ , and the lode parameter, $\xi $ , are needed. For shells only, stress triaxiality is needed.
Stress Triaxiality
Loading condition  Solids  Shells 

Confined compression  1  
Biaxial compression  2/3  2/3 
Uniaxial compression  1/3  1/3 
Pure shear  0.0  0.0 
Uniaxial tension  1/3  1/3 
Plane strain  0.5751  0.5751 
Biaxial tension  2/3  2/3 
Confined tension  1 
Lode Angle
To describe 3D loading conditions, another important quantity is the lode angle ( $\theta $ ) given by:
Under plane stress hypothesis (for shell elements), the lode angle and the stress triaxiality are linked and thus one for them can be used to recover the other:
As it is much easier to deal with normalized value instead of radians, the lode angle is usually switched by the Lode parameter denoted $\xi $ , given by:
 1.0 in compression
 In pure shear or plane strain
 In tension
Supported Failure Criteria
 BIQUAD
 The BIQUAD criterion is a stress triaxiality based failure criterion
mostly used for ductile metals. Its double quadratic curve shape
describes the evolution of plastic strain,
${\epsilon}_{p}^{f}$
, at failure with respect to stress
triaxiality,
$\eta $
, as shown in the below image.It then requires five parameters called c1, c2, c3, c4 and c5
respectively corresponding to V1,
V2, V3, V4
and V5 value in the MATF Bulk Data
Entry. These five values correspond to plastic strain at failure for
five different stress states:
 Uniaxial compression
 Pure shear
 Uniaxial tension
 Plane strain
 Biaxial tension
Note: The parabolic curve computation at high stress triaxiality is made so that c4 is always the minimum value.For shell elements, strain localization and necking occurring at high strain rate might not be correctly detected as the thickness variation is purely numerical. Thus, failure can be delayed in comparison to an equivalent sized solid element. To avoid that, an additional curve (see the blue curve in the below figure) can be defined for shells using INST parameter (V6), replacing c4 in the high stress triaxiality parabolic curve computation.If enough experimental data is unavailable to identify all the c1, c2, c3, c4 and c5 parameters, a material selector input is also available for BIQUAD criterion. Depending on the keyword MATER value chosen in the list presented above, the c1, c2, c4 and c5 parameters will be automatically computed with respect to c3 value, as shown below.$$c1=r1\cdot c3$$ $$c2=r2\cdot c3$$ $$c3=c3$$ $$c4=r4\cdot c3$$ $$c5=r5\cdot c3$$The value c3 is then the only expected parameter when using material input for BIQUAD criterion. However if no c3 value is specified, a default value of c3 will automatically be set.For each timestep, the plastic strain at failure, ${\epsilon}_{p}^{f}(\eta )$ , is estimated according to the stress triaxiality and the parabolic curves. This allows increases to the damage variable accounting for the stress state history:Table 2. Automatic parameters settings for MATER keyword Keyword c3 (Default) r1 r2 r4 r5 MILD 0.60 3.5 1.6 0.6 1.5 HSS 0.50 4.3 1.4 0.6 1.6 UHSS 0.12 5.2 3.1 0.8 3.5 AA5182 0.30 5.0 1.0 0.4 0.8 AA6082 0.17 7.8 3.5 0.6 2.8 PA6GF30 0.10 3.6 0.6 0.5 0.6 PP T40 0.11 10.0 2.7 0.6 0.7 $$D={\displaystyle \sum _{t=0}^{\infty}\frac{\text{\Delta}{\epsilon}_{p}}{{\epsilon}_{p}^{f}(\eta )}}$$  TSTRN
 The TSTRN failure criterion is a strain based damage model and is
supposed to be fully coupled (DAMAGE keyword
activated and
${D}_{C}=0$
). However, you have the freedom to use
it as a failure criterion or a pure output damage variable. It considers
a linear evolution of the damage variable between two starting and
ending strain values, in tensile loading conditions (
$\eta >0$
):$$D=\frac{\epsilon {\epsilon}_{start}}{{\epsilon}_{end}{\epsilon}_{start}}$$A couple of values ${\epsilon}_{start}$ and ${\epsilon}_{end}$ are then needed in the card. V1 and V2 values corresponds to starting and ending von Mises equivalent strain. The von Mises equivalent strain is computed as follows:$$\epsilon =\sqrt{\frac{2}{3}\left({\epsilon}_{xx}^{2}{}^{\text{'}}+{\epsilon}_{yy}^{2}{}^{\text{'}}+{\epsilon}_{zz}^{2}{}^{\text{'}}+2{\epsilon}_{xy}^{2}+2{\epsilon}_{yz}^{2}+2{\epsilon}_{zx}^{2}\right)}$$Where ${\epsilon}^{\text{'}}$ is the deviatoric strain tensor.If V3 and V4 values are specified, they correspond to starting and ending major principal strain.$$\epsilon =\mathrm{max}({\epsilon}_{1},{\epsilon}_{2},{\epsilon}_{3})>0$$Note: V3 and V4 values are always prioritized when both V1/V2 and V3/V4 pairs are specified.
 Tabulated failure criteria
 The TAB failure criterion is used to give as much freedom as possible to
describe a plastic strain based tabulated criterion. The
TABLEMD entry defined by EPS_TID describes the
map showing the evolution of plastic strain at failure,
${\epsilon}_{p}^{f}$
, with respect to stress triaxiality and,
optionally for solid elements, with lode parameter,
$\xi $
, as shown in Figure 5.For solid elements, the entire map with all possible couple of
values,
$(\eta ,\xi )$
, is considered. However, for shells
stress triaxiality and lode parameter are linked due to plane stress
conditions. Hence, only the plane stress (blue line in Figure 5) is considered.
The V1 value is a scale factor that allows you to quickly increase or decrease in entire map.
The damage variable evolution is given by a specific formula using the parameter in defined in V2 value:$$D={\displaystyle \sum _{t=0}^{\infty}\frac{\text{\Delta}{\epsilon}_{p}}{{\epsilon}_{p}^{f}(\eta ,\xi )}}\cdot n\cdot {D}^{\left(1\frac{1}{n}\right)}$$Thus, including its own current value, the damage variable evolution is taking into account the stress state history but also the damage history. The exponent $n$ allows to indirectly change the shape of the damage evolution with respect to plastic strain as presented in Figure 6. The increase of the $n$ exponent parameter tends to delay the stress softening effect as shown.You can use the TAB criterion defining only the first line of parameters (EPS_TID, V1 and V2). In this case, like any other criterion available, you can activate the element deletion using DAMAGE, chose the beginning of stress softening with the constant value for critical damage DC and the shape of the stress softening using EXP.Another approach of stress softening approach with TAB criterion is called the neckingcontrolled approach.
To use this new approach, the two first parameters of the second line INST_TID and V6 must be defined. INST_TID defines the ID of a TABLEMD entry defining a map showing the evolution of the plastic strain value (denoted ${\epsilon}_{p}^{loc}$ ) for which necking instability and thus strain localization starts, with respect to stress triaxiality and, optionally, lode parameter. It is an instability limit curve or map mostly defined at high stress triaxiality as the one described above for BIQUAD criterion in Figure 3 and is supposed to be lower than the failure curve/map to have an effect. It can be used with solids or shells.
This INST second map allows to compute the evolution of a new variable called neckingtriggering variable and denoted $f$ . Its evolution is very similar to the damage variable one:
$$f={\displaystyle \sum _{t=0}^{\infty}\frac{\text{\Delta}{\epsilon}_{p}}{{\epsilon}_{p}^{loc}(\eta ,\xi )}}\cdot n\cdot {f}^{\left(1\frac{1}{n}\right)}$$Once this variable reaches the value 1, a stress softening is triggered (defined by Comment 12 in the MATF Bulk Data Entry). However, instead of using the constant value, ${D}_{C}$ , in the MATF entry, the parameter, ${D}_{C}$ , becomes an integration point. Thus ${D}_{C}$ can be very different from one element to another depending on the history of the element stress state.
Thus, when INST_TID is used, the ${D}_{C}$ value corresponds to the value taken by the damage variable $D$ at the exact moment when $f$ reaches or overtakes the value 1. In other words, ${D}_{C}$ is the $D$ value when the necking criterion is reached the first time. Then, ${D}_{C}$ remains untouched until the end of the simulation.
$$\begin{array}{l}D={\displaystyle \int \text{\Delta}D}\\ f={\displaystyle \int \text{\Delta}f}\\ {D}_{C}=\left\{\begin{array}{c}\begin{array}{ccc}1& \text{while}& f<1\end{array}\\ \begin{array}{ccc}D& \text{when}& f\ge 1\end{array}\end{array}\right.\\ \sigma ={\sigma}_{eff}\left(1{\left(\frac{D{D}_{c}}{1{D}_{c}}\right)}^{\mathrm{exp}}\right)\end{array}$$Unlike the ${D}_{C}$ parameter, the exponent (EXP) is a constant parameter over all elements.This neckingcontrolled approach can offer a higher predictivity for a large range of stress state but needs to define an instability map especially at high stress triaxiality when necking is more likely to happen.
Finally, parameters V7 and V8 values are stress triaxiality boundaries for element size scaling defined below. If this pair of values are defined, the size scaling only occurs when:
$$V7<\eta <V8$$  Damage initiation and evolution (INIEVO)
 INIEVO failure criterion is very specific and provides the ability to
define a failure approach based on the use of a DMGINI Bulk Data Entry and, optionally a DMGEVO Bulk Data Entry.
For the DMGINI Bulk Data Entry, only DUCTILE criterion is available. For the DMGEVO Bulk Data Entry, only DISP and ENERGY evolution are available.
This criterion can be defined using two methods: The DAMAGE continuation line in the MATS1 Bulk Data Entry. This method is supported both for Implicit and Explicit Dynamic Analysis.
 CRI=INIEVO in the MATF Bulk Data Entry. This method is supported only for Explicit Dynamic Analysis.
Note: For INIEVO, strain rate dependency and element size dependency are not available.
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. The initial temperature field can be defined using TEMP(INIT) which uses the referenced temperature field to lookup the TABLEMD entry for the initial material data on the corresponding MATS1 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
 4noded CTETRA, 10noded CTETRA, 8noded CHEXA, and 6noded CPENTA elements are supported.
 Shell Elements
 CTRIA3 and CQUAD4 are supported.
 Onedimensional Elements
 CBUSH, CBEAM, and CBAR elements are supported.
 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:
The following materials are currently supported for Explicit Analysis:
MAT1, MAT2, MAT8, MATS1, MATHE, and MATVE materials are supported. The MATVE entry should be defined under MATHE entry.
 Linear Materials
 Isotropic Materials
 MAT1
 Anisotropic Materials
 MAT2, MAT9
 Orthotropic Materials
 MAT8, MAT9OR
 Nonlinear Materials
 Elastoplasticity (MATS1)
 JohnsonCook
 Hyperelasticity (MATHE)
 MOONEY
 Viscoelasticity (MATVE)
 Prony
 Cohesive Zone Modeling (CZM)
 MCOHED (TractionOpening)
 Failure Models:
 Failure (MATF)
 BIQUAD
 Damage Initiation and Evolution
 MATS1 (via DAMAGE continuation line – DMGINI and DMGEVO)
 Brittle Damage
 MATBRT
 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.
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
The NLDEBUG, CONT2TIE and NLDEBUG, RMNLMAT are available to simplify the model in certain ways to aid in debugging.
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.
 _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 massoriginal 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 timestep.
 _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.
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:


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  Onedimensional elements: CBUSH,
CBEAM, and CBAR are supported;


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, MAT9OR, MCOHED, and MATHE. 
See analysis_nonlinear_explicit_r.htm#analysis_nonlinear_explicit_problem_setup_r_reference_ywr_2hb_shb__analysis_nonlinear_explicit_problem_setup_r_ph_tll_hfp_xbc for more information.  
Properties:  
Supported Properties  NA  PSHELL, PSOLID, PLSOLID, PCOMP, PCOMPG, PCOMPP, PCOMPLS  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. AutoContact is supported by setting the TYPE field to AUTO on CONTACT Bulk Data Entry. For TIE in
explicit:


Coordinate Systems:  
Supported Userdefined 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.
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. When a monitor volume is defined via the MONVOL Bulk Data Entry, the following output results are available by default – Pressure, Temperature, Volume, Area, Mass, Internal Energy, Mass flow rate, Vent Area and Leaked Mass. 

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  
Monitor Volume  NA  MONVOL  Defines a onechamber gas filled structure with hybrid input of inflated gas.  
Material Failure Criterion  NA  MATF or MATS1 (for damage initiation and evolution criteria only).  
Mass scaling control  MSCALE  NA  
Hourglass Control  HOURGLS (HGID field
references this card on
PSOLID/PLSOLID/PSHELL) PARAM,HOURGLS 
The default hourglass 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 