Implicit Features and Compatibility

Not all explicit features are available for implicit analyses; actual available features are presented in this section.

Element Formulations

In Radioss implicit, the element formulations are used in two main computations.

  1. Stiffness Matrix will determine the displacements:

    Available element formulations for this computation are outlined in the table below.

  2. Strains, Stress and Internal Nodal Forces:
    Implicit and explicit analyses share the same coding and all formulations are available for this computation.
    /BRICK /TETRA4 /TETRA10 /BRIC20 Thick Shell

    /BRICK, /PENTA6
    Isolid=24

    Isolid=14 (recommended)

    		 Itetra4=0 Itetra10=0 Isolid=16 Isolid=14, 15
    /SHELL /SH3N /SPRING /BEAM /TRUSS
    Ishell=24 (QEPH)

    Ishell=12 (QBAT)

    		 Ish3n=1

    Ish3n=2 (default)

    		 /PROP/TYPE4, /PROP/TYPE8, /PROP/TYPE12, /PROP/TYPE13 /PROP/TYPE3 (BEAM) /PROP/TYPE2 (TRUSS)

Monitored Volume TYPE3, Orthotropic shell (TYPE9, 10, 11 and 17) are also available.

Orthotropic solid (TYPE6) is also available from version 11. However, the elements in the above table are strongly recommended, especially in a nonlinear analysis.

Material Compatibility

Radioss uses only the elastic part of material parameters to build the stiffness matrix (or Jacobian matrix for nonlinear analyses) for most of the material laws.

For the hyper-elastic type laws (42, 62, 69, and 82), special treatments have been done to avoid the divergence. The use of elastic matrix (called initial stress method) results out slow convergence (consisting tangent matrix development is ongoing); two Nonlinear Solution methods are recommended in this case, Modified Newton and Quasi-Newton (BFGS). For the viscous type laws used for quasi-static analysis, a long duration time is recommended for the simulation (as there is no physical sense for time in this case). In this way, there is no compatibility issue with any Radioss material, but converging issues might be experienced, especially for the high nonlinear materials.

Kinematic Conditions

Several kinematic conditions are supported.

The following available kinematic conditions are supported in Radioss Implicit:
  • Boundary conditions /BCS
  • Imposed displacement /IMPDISP (velocity /IMPVEL, and acceleration /IMPACC)
  • Rigid bodies /RBODY
  • Interface TYPE2 /INTER/TYPE2 (not available with rupture or penalty methods)
  • Rigid walls /RWALL (not recommended, due to performance reasons. Use contact interface, if possible.)
  • Adaptive meshing link /ADMESH
  • Interpolation constraint element /RBE3
  • Rigid element /RBE2

Contact Interfaces

Only contact interface types 5, 7, 10 and 11 are available and supported in Radioss Implicit.

Note: Some options of interface TYPE7, such as Ifric > 0, Iadm are currently not available. Only the SMP version is available with interface TYPE24 in implicit.

Contact interfaces are treated through a penalty method (with fictitious springs) and the contact stiffness will be stored in an independent stiffness matrix. Information regarding this second stiffness matrix can be printed out (if /IMPL/PRINT/NONLIN/n is defined) once contacts have been detected.

Loads

Concentrated load /CLOAD, pressure /PLOAD, and gravity load /GRAV are available. The loading definition is the same as in an explicit simulation.

Note: Additional attention should be brought to time-based loading functions in nonlinear implicit computations as this might influence the iteration convergence. In such computations, the use of increasing time versus load function, instead of a constant function is recommended even for the gravity load and the imposed displacements.

Thermal Analysis

In Radioss not all thermal options are currently available for implicit analysis.

Implicit Analysis Types

The following analysis modules (types) are available:
  • Model Check: with /IMPL/CHECK
  • Static or Quasi-static linear
  • Buckling mode analysis
  • Static or Quasi-static nonlinear
  • Dynamic nonlinear
  • Modal analysis