# Time Step Control Methods

The time step can often be increased using some of these time step control methods.

One of the most common issues with an explicit finite element simulation is the amount of time the simulation takes to solve. The larger the model’s time step, the less cycles that are required to solve a simulation which results in a lower solution time.

Ignoring contact stiffness, the minimum time step of a simulation is a function of the mesh size, material stiffness, and density. Therefore, the first way to increase the time step of a model is to improve the mesh quality by modifying elements with small edge lengths relative to the average element length of the mesh.

Once the mesh is improved, another common problem is a reduction in time step, due to deformation of the mesh. As mentioned earlier, the minimum time step is calculated during each cycle of a simulation and as deformation occurs the elements size may reduce which cause a reduction in time step. If there is a large reduction in time step, there will be a large increase in simulation time. There are various methods to deal with the reduction in time step.

With some minor variation, all of these methods use this input format.
• /DT/option/Keyword3/Iflag
• $\text{Δ}{T}_{sca}$ $\text{Δ}{T}_{\mathrm{min}}$
Where,
$\text{Δ}{T}_{sca}$
Scale factor for the critical nodal time step
$\text{Δ}{T}_{\mathrm{min}}$
Minimum model time step that activates the time step control

For all options, the time step control is activated when $\text{Δ}{T}_{\mathrm{min}}\ge \text{Δ}{T}_{sca}*\text{Δ}{t}_{option}$ ; where, $\text{Δ}{t}_{option}$ is the time step calculation, based on the option being used such as nodal, element, or interface.

Lagrangian elements whose volume becomes negative during a simulation will automatically switch to the strain formulations to allow the simulation to continue. When this occurs, a Warning message will be printed in the Engine output file.
Table 1. Supported Options
Element Type and Formulation Strain Formulation Negative Volume Handling Method
/BRICK, Isolid =1, 2, 14, 17, 24

/TETRA4, Itetra = 0

/TETRA10

Full geometric nonlinearities

Ismstr = 2, 4

Switch to small strain using element shape from cycle before negative volume
Lagrange type total strain

Ismstr = 10, 12

Lagrange type total strain with element shape at time=0.0

The automatic switch to small strain can be disabled by setting Keyword2 to STOP in /NEGVOL.