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
  • Δ T sca Δ T min
Where,
Δ T sca
Scale factor for the critical nodal time step
Δ T min
Minimum model time step that activates the time step control

For all options, the time step control is activated when Δ T min ≥ Δ T s c a * Δ t o p t i o n MathType@MTEF@5@5@+= feaagKart1ev2aaatCvAUfeBSjuyZL2yd9gzLbvyNv2CaerbuLwBLn hiov2DGi1BTfMBaeXatLxBI9gBaerbd9wDYLwzYbItLDharqqtubsr 4rNCHbGeaGqiVu0Je9sqqrpepC0xbbL8F4rqqrFfpeea0xe9Lq=Jc9 vqaqpepm0xbbG8FasPYRqj0=yi0dXdbba9pGe9xq=JbbG8A8frFve9 Fve9Ff0dmeaabaqaciGacaGaaeqabaWaaeaaeaaakeaacqqHuoarca WGubWaaSbaaSqaaiGac2gacaGGPbGaaiOBaaqabaGccqGHLjYScqqH uoarcaWGubWaaSbaaSqaaiaadohacaWGJbGaamyyaaqabaGccaGGQa GaeuiLdqKaamiDamaaBaaaleaacaWGVbGaamiCaiaadshacaWGPbGa am4Baiaad6gaaeqaaaaa@4B96@ ; where, Δ t o p t i o n MathType@MTEF@5@5@+= feaagKart1ev2aaatCvAUfeBSjuyZL2yd9gzLbvyNv2CaerbuLwBLn hiov2DGi1BTfMBaeXatLxBI9gBaerbd9wDYLwzYbItLDharqqtubsr 4rNCHbGeaGqiVu0Je9sqqrpepC0xbbL8F4rqqrFfpeea0xe9Lq=Jc9 vqaqpepm0xbbG8FasPYRqj0=yi0dXdbba9pGe9xq=JbbG8A8frFve9 Fve9Ff0dmeaabaqaciGacaGaaeqabaWaaeaaeaaakeaacqqHuoarca WG0bWaaSbaaSqaaiaad+gacaWGWbGaamiDaiaadMgacaWGVbGaamOB aaqabaaaaa@3EA0@ 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. The following options are supported:
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.