**Next:***SUBMODEL

**Up:**Input deck format

**Previous:***STEADY STATE DYNAMICS

**Contents**

##

*STEP

Keyword type: step

This card describes the start of a new STEP. PERTURBATION, NLGEOM, INC, INCF and TURBULENCE MODEL are the optional parameters.

The parameter PERTURBATION is allowed for *FREQUENCY and *BUCKLE steps only. If it is specified, the last *STATIC step is taken as reference state and used to calculate the stiffness matrix. This means the inclusion of previous deformations (large deformation stiffness) and the inclusion of previous loads as preloads (stress stiffness), taking the temperatures into account to determine the material properties. The loads active (mechanical and thermal) are those specified in the perturbation step. The displacements and stresses are those corresponding to the eigenmodes. At the end of the step the perturbation load is reset to zero.

The loading active in a non-perturbative step is the accumulation of the loading in all previous steps since but not including the last perturbation step (or, if none has occurred, since the start of the calculation), unless OP=NEW has been specified since.

If NLGEOM is specified, the calculation takes geometrically nonlinear effects into account. To this end a nonlinear strain tensor is used (Lagrangian strain for hyperelastic materials, Eulerian strain for deformation plasticity and the deviatoric elastic left Cauchy-Green tensor for incremental plasticity), the step is divided into increments and a Newton iteration is performed within each increment. Although the internally used stresses are the Piola stresses of the second kind, they are transformed into Cauchy (true) stresses before being printed. In the present version of the program geometrically nonlinear calculations only apply to static calculations, and consequently the *STATIC or *DYNAMIC keyword card should be used within the step. The latter card also allows for the specification of the step size and increment size. The maximum number of increments in the step (for automatic incrementation) can be specified by using the parameter INC (default is 100) for thermomechanical calculations and INCF (default is 10000) for 3D fluid calculations. In coupled fluid-structure calculations INC applies to the thermomechanical part of the computations and INCF to the 3D fluid part. Once the NLGEOM parameter has been selected, it remains active in all subsequent static calculations. Some analyses involving nonlinear materials (*HYPERELASTIC, *HYPERFOAM, *DEFORMATION PLASTICITY, *PLASTIC, *CREEP) automatically trigger the NLGEOM option. Thus, for these types of analysis nonlinear geometric effects are always taken into account. This also applies to analyses with 1d or 2d elements in the presence of knots and calculations with *GAP, *MPC or *RIGID BODY definitions.

For 3D fluid calculations the parameter TURBULENCE MODEL defines the turbulence model to be used. The user can choose among NONE (laminar calculations; this is default), K-EPSILON, K-OMEGA and SST [42].

First and only line:

- *STEP
- Enter any needed parameters and their values

Example: *STEP,INC=1000,INCF=20000,TURBULENCE MODEL=SST

starts a step and increases the maximum number of thermomechanical increments to complete the step to 1000. The maximum number of 3D fluid increments is set to 20000 and for the turbulence model the SST model was chosen.

Example files: beamnlp.

**Next:***SUBMODEL

**Up:**Input deck format

**Previous:***STEADY STATE DYNAMICS

**Contents**guido dhondt 2012-10-06