# Time Step Control

- Element time step
- Nodal time step

The time step used by the solver is the largest possible time step, as determined by the Courant condition that will maintain stability. If the default large strain formulation is used, the time step is computed at each cycle. Large element deformation can give a large time step decrease. If the deformation is too large, negative volumes can result, which make it impossible to invert the Jacobian matrix and to integrate the stress over the volume. If the small strain formulation is used, assuming a constant Jacobian matrix during time and also a constant volume, all spatial variables are defined at $t=0$ . This is either the beginning of the analysis or the time at which the small strain formulation is initiated. If the sound speed is constant, the time step thus becomes constant. Using this formulation, the time step has no effect on the computation since the initial volume is used.

## Element Time Step Control

The stable element time step was detailed in Courant Condition Stability and is restated as:

- $l$
- Element characteristic length
- $c$
- Speed of sound in the material

This is the default setting.

The element time step is computed at the same time as the internal forces. The characteristic length and the sound speed are computed for each element in every cycle.

The computed time step is compared to a minimum time step value and a scale factor is applied to ensure a conservative bound. Different minimum time step values can be given to different element types by using the option: /DT/Keyword.

`Keyword`- Defined in the user manual as the element type

- Stop the analysis when the minimum time step value is reached. This is the default for brick and quadrilateral elements.
- Delete the element(s) defining the time step. This is the default for shell elements.
- Implement small strain formulation using a constant time step. This only works for shell and brick elements.

These options are defined using a third keyword: STOP, DEL, CST, AMS or SET

## Nodal Time Step Control

The nodal time step is calculated after the computation of all the internal forces at each node using:

- $m$
- Nodal mass
- $k$
- Equivalent nodal stiffness

The nodal stiffness is one half of eigen value from element stiffness matrix; for a truss element this value is equal to the diagonal term of the stiffness matrix. It is computed from the accumulation of element and interface stiffness'. These stiffness' are obtained during internal force computation.

For a regular mesh, the element time step and nodal time step conditions are identical. Consider the element time step condition for a truss element.

The nodal time step condition is written as:

with

Therefore:

To select the nodal time step when running Radioss the option /DT/NODA has to be used.

As for the element time step, minimum time step and scale factors are required. The default value for the scale factor is 0.9. If the minimum time step is reached, the analysis can either be stopped or a mass scaling formulation can be applied. In the latter case, mass is added to the affected nodes so that the time step remains constant at the minimum value. This option can be enabled using the same third keyword as used in the element time step control. It must be checked that added masses do not affect the accuracy of results. If one uses the nodal time step, the element time step is ignored.

## Interface Time Step Control

Finally, the time step is influenced by existence of interfaces. The interface time step control depends on the type of interface being used.

For the interfaces in which the contact conditions are defined by applying kinematic conditions, no time step restriction is required. This is the case of interface TYPE 2 of Radioss.

In addition, for the interfaces TYPES 3, 4, 5, and 8 in Radioss a small stiffness is used. Therefore, the interfaces are stable if a time step scale factor less than or equal to 0.9 is used.

TYPES 7, 10 and 11 interfaces use a variable stiffness and if this stiffness is not small compared to the element stiffness, a stability condition must be adhered to.

Default (element) time step without interfaces TYPES 7, 10 or 11 | Element time step is computed and a scaling factor of 0.9 (default) is applied. |

Option /DT/NODA is used with or without interface TYPES 7 and/or 10, 11 | Nodal time step is computed and a scaling factor of 0.9 (default) is applied. |

Default time step with interface TYPES 7 or 10, 11 | Nodal and element time steps are computed and the smallest is used. |

If the deletion option is applied with the /DT/INTER/DEL interface time step control, the node controlling the minimum time step is deleted from the interface.

Mass scaling, where mass is added to an interface node, can be enabled using the option /DT/INTER/CST.