Explicit Dynamic Analysis (Beta Release)

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, General contact 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, RBE3s 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.

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 ( $ρ$ ).

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:(17)

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.(18)

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:(19)

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

The final nodal stiffness is:(20)

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`=URI)	Regular Elements (`ISOPE`=AURI)	Regular Elements (`ISOPE`=SRI)
CHEXA (1st order)	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 turned on by default. ²
CTETRA (2nd order)	Hourglass control not required	Hourglass control not required	Hourglass control not required
CPENTA (1st order)	NA	NA	Hourglass Control is not turned on by default. ²
CTETRA (1st order)	Hourglass control not required	Hourglass control not required	Hourglass control not required

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/MATS1	Available ²	Default ⁶	NA
MATHE	NA	Available ²	Default ⁶
MATVE	NA	Available ²	Default ⁶

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.

Mass Elements

CONM2 is supported.
Supported Materials:
MAT1, MATS1, MATHE, MATVE materials supported. FOAM material in MATHE is supported for Explicit analysis; however, it is not supported for nonlinear implicit analysis. 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, or PSHELL 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, Velocity, Acceleration, Strain, Stress, and Plastic Strain are output.
_expl.mvw: Curves for Strain Energy, Elastic Contact Energy, Plastic Contact Energy, Kinetic Energy, Hourglass Energy, and Plastic Dissipation Energy are 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).

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	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.
Rigids:
Support for Rigids	NA	RBE2 and RBODY are supported.
Materials:
Supported Materials	NA	Shells: MAT1 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 supported for implicit are also supported for Explicit, and in addition, Foam material is supported on MATHE for Explicit.
Properties:
Supported Properties	NA	PSHELL, PSOLID, and PLSOLID
Contact:
Supported Contact Types	NA	CONTACT and TIE	N2S and S2S contact discretization are supported. SMALL, FINITE, and CONSLI contacts are supported. General Contact is not currently supported. 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, slave node of a TIE cannot be the master 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)	NA	Results are output only to the _expl.h3d and _expl.mvw files. _expl.h3d The displacement, velocity, acceleration, stress, strain, and plastic strain results are output. _expl.mvw The curves for Strain energy, Elastic Contact energy, Plastic Contact energy, Kinetic energy, Hourglass energy, and Plastic Dissipation energy are output.
Output Control	NLOUT	NLOUT	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.
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 ,PARAMHOURGLS 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 CTRIA3 elements do not require hourglass control

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)