Explicit Dynamic Analysis (Radioss Integration)

Explicit Dynamic Analysis in OptiStruct is provided through an integration of the Radioss Starter and Radioss Engine via a translator. Explicit integration schemes, are available via Radioss Integration.

Transparent to you, OptiStruct input data is directly translated into Radioss input data. The Radioss Starter and Radioss Engine are then executed, and the results are brought back into the OptiStruct output module to export the different output formats.

Solution Method

The basic concepts of the solution methods to highlight the characteristics of the solution methods and to identify the use of certain parameters to control convergence. The solution utilizes a general Newmark integration scheme.

The following equation of motion shall be solved.(1)

M \ddot{u} + C \dot{u} + K u = f

$M$: Mass matrix
$C$: Damping matrix
$K$: Stiffness matrix; These matrices are derived using finite elements.
$f$: The vector describes the external loads
$u$: Displacement vector; The dots describe the derivatives with respect to time.

The equation of motion can be solved using a general Newmark integration scheme. Newmark is a one-step time integration method. All solutions can be derived from it and are formulated in terms of a Time History (Figure 1).

Figure 1. Time History

In general Newmark, the state vector is computed:(2)

{\dot{u}}_{t + 1} = {\dot{u}}_{t} + Δ t [(1 - γ) {\ddot{u}}_{t} + γ {\ddot{u}}_{t + 1}]

(3)

u_{t + 1} = u_{t} + Δ t {\dot{u}}_{t} + (\frac{1}{2} - β) Δ t^{2} {\ddot{u}}_{t} + β Δ t^{2} {\ddot{u}}_{t + 1}

Then the equation of motion yields:(4)

[M + γ Δ t C + β Δ t^{2} K] {\ddot{u}}_{t + 1} = f - C [{\dot{u}}_{t} + (1 - γ) Δ t {\ddot{u}}_{t}] - K [u_{t} + Δ t {\dot{u}}_{t} + (\frac{1}{2} - β) Δ t^{2} {\ddot{u}}_{t}]

This can be rewritten into:(5)

[\frac{1}{β Δ t^{2}} M + \frac{γ}{β Δ t} C + K] Δ u_{t} = Δ {\tilde{f}}_{t}

using:(6)

u_{t + 1} = u_{t} + Δ u_{t}

In short:(7)

A Δ u = \tilde{f}

The matrix $A$ is the dynamic stiffness. In nonlinear time-dependent problems, this system becomes nonlinear and its solution requires an additional iteration loop at each time step using a Newton-type method.

A conditionally stable explicit integration scheme can be derived from the Newmark scheme by setting:(8)

γ = \frac{1}{2}, β = 0

(9)

{\dot{u}}_{t + 1} = {\dot{u}}_{t} + \frac{1}{2} Δ t [{\ddot{u}}_{t} + {\ddot{u}}_{t + 1}]

(10)

u_{t + 1} = u_{t} + Δ t {\dot{u}}_{t} + \frac{1}{2} Δ t^{2} {\ddot{u}}_{t}

From these relationships the central differences explicit integration scheme can be derived.(11)

{\dot{u}}_{t + 1 / 2} = {\dot{u}}_{t - 1 / 2} + Δ t_{12} {\ddot{u}}_{t}

(12)

u_{t + 1} = u_{t} + Δ t_{2} {\dot{u}}_{t + 1 / 2}

(13)

M {\ddot{u}}_{t + 1} = f - C {\dot{u}}_{t + 1 / 2} - K u_{t + 1}

Figure 2 illustrates the relationships.

Figure 2. Explicit Integration

Assuming that(14)

C {\dot{u}}_{t + 1} \approx C {\dot{u}}_{t + 1 / 2}

The equation of motion for the central differences scheme simplifies to:(15)

M {\ddot{u}}_{t + 1} = f - C {\dot{u}}_{t + 1} - K u_{t + 1}

(16)

M {\ddot{u}}_{t + 1} = f - \int B_{t + 1}^{t} σ_{t + 1} d V

These central differences scheme is used for explicit analysis. The time step must always be smaller than the critical time step to ensure stability of the solution. The critical time step depends on the highest frequency in the system and is computed from the corresponding angular frequency

ω_{\max}

as:(17)

Δ t_{c r} = \frac{2}{ω_{\max}}

For a discrete system, the time step must be small enough to excite all frequencies in the finite element mesh. This requires such a short time step that a shock wave does not miss any node when traveling the mesh. Therefore, (18)

Δ t \leq \frac{l_{c}}{c}

With $l_{c}$ being the critical length of an element and $c$ is the speed of sound in the given material.

Different ways of time step control are available. The default method is the nodal time step which is computed from the nodal mass

m

and the equivalent nodal stiffness

k

such that:(19)

Δ t_{c m} = \min_{n} \sqrt{\frac{2 m}{k}}

The element time step based on the critical length of each element is also available. The choice can be made on the XSTEP Bulk Data Entry.

Problem Setup

Explicit Dynamic Analysis is defined through a SUBCASE.

An XSTEP statement as well as ANALYSIS=EXPDYN must be present in the subcase. To define the termination time a TTERM Subcase Information Entry is mandatory. XSTEP references an XSTEP Bulk Data Entry. Time step control can be defined on the XSTEP Bulk Data Entry.

The definition of a unit system through the DTI, UNITS or UNITS Bulk Data Entry statement is required.

The Explicit Dynamic Analysis loads and boundary conditions are defined in the Bulk Data Entry section of the input deck. They need to be referenced under the SUBCASE using an SPC, NLOAD, LOAD, IC and RWALL statements in a SUBCASE. Each SUBCASE defines one loading condition that is executed separately.

Subcase continuation is available through the use of CNTNLSUB. Any number of explicit and implicit analyses can be linked. However, explicit (ANALYSIS=EXPDYN) analysis subcases cannot yet be linked with small displacement quasi-static nonlinear (ANALYSIS=NLSTAT) analysis subcases and vice versa.

Example: Explicit Analysis

SUBCASE       3
  ANALYSIS = EXPDYN
  SPC = 1
  NLOAD = 2
  XSTEP = 3
  TTERM = 1.0
  DISP = ALL
  STRESS = ALL
BEGIN BULK
XSTEP,3
NLOAD1,2,2,,L,88
TABLED1,88,
+,0.0,0.0,1.0,1.0,ENDT
DTI,UNITS,1,kg,N,m,s

Example: Subcase Continuation

DISP = ALL
  STRESS = ALL
SUBCASE       1
  ANALYSIS = EXPDYN
  IC = 5
  XSTEP = 4
  TTERM = 1.0
SUBCASE       2
  ANALYSIS = EXPDYN
  IC = 5
  XSTEP = 4
  TTERM = 1.1
  CNTNLSUB = 1

User's Considerations

Explicit Dynamic Analysis Properties and Materials

Special element types and nonlinear materials are available for Explicit Dynamic Analysis. As a general rule, property and material definitions that are only applicable in Explicit Dynamic Analysis are defined on extensions to the original property and to a MAT1 material, respectively. The extensions are grouped with the base entry by sharing the same PID or MID. In the case of a subcase that is not an Explicit Dynamic Analysis, these extensions are ignored. Property defaults can be set for shells (XSHLPRM) and solids (XSOLPRM) that may replace the use of property extensions.

Property Example:

PSHELL, 3, 7, 1.0, 7, , 7
PSHELLX, 3, 24, , , 5

Material Example:

MAT1, 102, 60.4, , 0.33, 2.70e-6
MATX02, 102, 0.09026, 0.22313, 0.3746, 100.0, 0.175

Coordinate Systems

In Explicit Dynamic Analysis there are moving and fixed coordinate systems. Rectangular coordinate systems that are defined through grid points (CORD1R, CORD3R) are moving with the deformations of the model. Systems defined in terms of point coordinates (CORD2R, CORD4R) are fixed.

The behavior of loads depends on the coordinate system referenced. If the loads FORCE and MOMENT are desired to be follower forces, a CID that references a moving coordinate system (CORD1R, CORD3R) must be defined. Otherwise these loads are not following the deformation. PLOAD always follows the deformations.

Characteristics

Explicit Dynamic Analysis has the following characteristics:

In general, a diagonal mass matrix is used
No matrix factorization necessary
Equilibrium is always guaranteed
Maximum stable time step needs to be respected
Small time steps
Short-term events

Limitations

The solution will be terminated if unsupported Bulk Data Entries are encountered.

The following Bulk Data properties and elements are currently not translated:
- PBUSHT (partially, KN is translated)
- PDAMP, CDAMPi
- PGAP, CGAP, CGAPG (partially, friction is not allowed)
- PMASS, CMASSi
- PSHEAR, CSHEAR
- PVISC, CVISC
Additional relevant Bulk Data Entries (except loads) that are currently not translated:
- CORD1C, CORD1S, CORD2S
- DMIG
- MAT2, MAT4, MAT5, MAT8, MAT9, MAT10
- MATTi, TABLEST
- MPC, MPCADD
- RBE1, RROD
Relevant loads that are currently not translated:
- PLOAD1, PLOAD2
- PLOAD4 (partially, N1, N2, N3 cannot be used)
- RFORCE (partially, RACC is not supported)
- TLOAD1, TLOAD2