!STEP¶

Analysis step settings

Required for nonlinear static and nonlinear dynamic analysis

If you omit this definition for any analysis other than the above, all boundary conditions are in effect and the calculation is done in one step

In static analysis, if the material properties are visco-elasticity and creep, specify TYPE=VISCO and set the calculation time condition.

Note that TYPE (STATIC/VISCO) is the step type that controls whether a time increment is passed to the material, and is an axis independent of the analysis type (STATIC/DYNAMIC etc.) specified by !SOLUTION (see Note below).

Parameter¶

TYPE     = STATIC (default)/VISCO (quasi-static analysis)
SUBSTEPS = Number of substeps of the boundary conditions (Default: 1)
CONVERG  = Convergence threshold (Default: 1.0e-6)
MAXITER  = Maximum number of iterations in nonlinear analysis (Default: 50)
AMP      = Time function name (specified in !AMPLITUDE)
INC_TYPE = FIXED (fixed increment, default) / AUTO (automatic increment)
MAXRES   = Setting of maximum allowable residuals (default: 1.0e+10)
TIMEPOINTS = Name of the time list (specified by `!TIME_POINTS, NAME`)
AUTOINCPARAM = auto-incremental parameter set name (specified by `!AUTOINC_PARAM, NAME`)
MAXCONTITER = Maximum number of contact iterations in contact analysis (default: 10)

** 2nd line or later **

In case of INC_TYPE=FIXED (If TYPE=STATIC, it can be omitted.)

(2nd line) DTIME, ETIME

Parameter Name	Attribution	Contents
DTIME	R	Time increment value (Default: 1/SUBSTEPS)
ETIME	R	End value of time increment in this step (Default: 1)

In case of INC_TYPE=AUTO (regardless of TYPE)

(2nd line) DTIME_INIT, ETIME, MINDT, MAXDT

Parameter Name	Attribution	Contents
DTIME_INIT	R	Initial time increment
ETIME	R	Step time width
MINDT	R	Lower limit of time increments
MAXDT	R	Maximum limit of time increments

** 3rd line or later **

BOUNDARY, id          GRPID defined in id=!BOUNDARY
LOAD, id              GRPID defined in id=!CLOAD, !DLOAD, !SPRING, !TEMPERATURE
CONTACT, id           GRPID defined in id=!CONTACT

example¶

Examples of fixed time increment usage¶

!STEP, CONVERG=1.E-8
0.1, 1.0
BOUNDARY, 1
LOAD, 1
CONTACT, 1

Enable automatic incremental adjustment, set the initial time increment to 0.01, step time width to 2.5, lower time increment 1E-5, upper time increment 0.3, and maximum number of sub-steps to 200.

!STEP, INC_TYPE=AUTO, SUBSTEPS=200
0.01, 2.5, 1E-5, 0.3

Enable automatic incremental adjustment and specify time list TP1 as the calculated and resulting output time

!STEP, INC_TYPE=AUTO, TIMEPOINTS=TP1
0.1, 2.0, 1E-3, 0.2

Note¶

TYPE (STATIC/VISCO) is a switch for whether a time increment is passed to the material constitutive law in that step, and is an axis independent of the analysis type specified by !SOLUTION. With STATIC the material does not see the time increment (rate-independent); with VISCO visco-elasticity and creep refer to the actual time increment. This distinction is effective only in static analysis; in dynamic analysis (!SOLUTION, TYPE=DYNAMIC) TYPE is not referenced and the time increment is always treated as actual time.
In dynamic analysis, the fixed time increment and step time width should be specified with DTIME, ETIME on the 2nd line of !STEP. The n_step and t_delta of !DYNAMIC are treated as defaults used only when !STEP is omitted (legacy single-step input) or for backward compatibility.
In the case of automatic incremental adjustment, SUBSTEPS is treated as the maximum number of substeps
Time-list name TIMEPOINTS and automatic contact parameter set AUTOINCPARAM are valid only when INC_TYPE=AUTO.
if TIMEPOINTS is specified, the destination !TIME_POINTS must be defined before the !STEP card.
if AUTOINCPARAM is specified, the destination !AUTOINC_PARAM must be defined prior to the !STEP card. If this parameter is omitted, the default auto-incremental parameter set is used.