5.1 Create a Step

To create a step, do this

Module:	Step
Menu:	Step, Create, OK

This opens a window (see screenshots below) where you give a name, like ApplyStrain, to the step. Also, you select the Procedure type, which could be:

General.

Is used for linear and nonlinear incremental analysis.

Linear perturbation.

One step linear analysis, or two-step for buckling eigenvalue/eigenmode extraction, vibration frequencies/modes, etc. See screenshot below.

\includegraphics[width=.5\textwidth ]{./AbqImages/CreateStep.PNG} \includegraphics[width=.5\textwidth ]{./AbqImages/CreateStepLinearPerturbation.PNG}

Among the General procedures you choose one of these:

Coupled temp-displacement.
Coupled thermal-electrical-structural.
Direct cyclic.
Dynamic implicit.
Geostatic.
Soils.
Static, General.

This is the most common. Static analysis that can be linear or nonlinear. The nonlinear algorithm is Newton-Raphson.

Static, Riks

Nonlinear static analysis with Riks The nonlinear algorithm is Newton-Raphson.

Visco.

Among the Linear Perturbation procedures you choose one of these:

Buckle.

Finds buckling load-multipliers (eigenvalues) and buckling mode shapes (eigenvectors).

Frequency

Finds vibration frequencies and modes of vibration.

Static, linear perturbation

Static linear with several load cases possible.

Steady-state dynamics, Direct.
Substructure generation.

Once you hit Continue, you get to Edit Step where you have 3 tabs (see screnshots) below.

\includegraphics[width=.5\textwidth ]{./AbqImages/EditStepBasic.PNG} \includegraphics[width=.5\textwidth ]{./AbqImages/EditStepIncrementation.PNG}

and

\includegraphics[width=.5\textwidth ]{./AbqImages/EditStepOther.PNG}

It is important to understand these concepts:

Time period.

(timePeriod). In a time dependent analysis such as viscoelastic analysis, it is the time in whatever units you are using for time, say seconds. In a nonlinear analysis without real time scale, such as plasticity, it is pseudo-time (no units). The time period is divided into increments.

Increment

Inc

Initial increment.

initialInc It is the first increment. Must satisfy initialInc$<$maxInc

Minimum increment.

minInc

Maximum increment.

maxInc

If a load $P_ F$ (or specified displacement $U_ F$) is defined in Module: Load, each increment increments the load by

  $\displaystyle  \Delta P = \frac{P_ F}{{timePeriod}}\times {Inc}  $   (5.1)

Say you apply $U_ F$=0.30 mm to a bar of length L=15 mm, and you want to apply it gradually, during pseudo-time 0 to 2, with increments of 0.001 mm each, then

  $\displaystyle  \Delta U = \frac{U_ F}{{2}}\times {0.001}=15\times 10^{-5}\frac{\text {mm}}{\text {increment}}  $   (5.2)

and the volume-average strain in the bar is

  $\displaystyle  \epsilon = \frac{0.30\text { mm}}{{15\text { mm}}}=0.02\; \frac{\text {mm}}{\text {mm}}=2\% \text { strain}  $   (5.3)

By setting timePeriod=2, the increments correspond to strain increments, i.e.,

  $\displaystyle  \Delta \epsilon = \frac{2}{{2}}\times {0.001}=0.1\% \text { strain}  $   (5.4)

Python

# create a Step
Step = Model.StaticStep(timePeriod=float(ModelParameters['Strain']),
                        initialInc=0.00001,
                        minInc=0.00000001,
                        maxInc=0.00001,
                        maxNumInc=100000,
                        name='ApplyStrain',
                        previous='Initial')