When looking at the output file of my solver, I have been told that the time-step taken by the solver depends on parameters like the total number of elements and their relative size in my geometry, or the material properties. A material with a high Young modulus could decrease the time step taken by the solver, as well as high number of elements, or elements with great difference in size. I am solving under explicit solver.

More specifically, the time step appears to be the time needed for the information to go through one element to another.

This gets me quite confused. How is time step related with these parameters ? Is there any formal physical relationship ? What about this time to go through an element, does it have mathematical foundation? Is there any advice to get it fit correctly ?

Edit: I am running a time-dependent linear elastic simulation in solid mechanics indeed.

  • $\begingroup$ Can you give some more details on the simulation you're running? $\endgroup$
    – wogsland
    Commented Mar 6, 2017 at 11:45

2 Answers 2


It sounds as if you're running a time-dependent linear elasticity simulation, right? Most likely, you're running an "Explicit" time-stepping scheme, which means that all of your information at time $t_{i+1}$ is computed entirely using information from time $t_i$ (or $t_{i-1}$...).

One consequence of such a scheme is that in order to be a stable time stepping scheme, it must be able to propagate a wave through the material without the wave moving more than a single element distance in a single time step.

This imposes a relationship between your Young's Modulus $E$, density $\rho$, your mesh sizing $\Delta x$, and $\Delta t$. Imprecisely, you need something like $\sqrt{\frac{E}{\rho}}\frac{\Delta t}{\Delta x}$ to be small in order for most schemes to be stable. The exact size of this ratio will depend on the time stepping scheme used (and the ratio is usually expressed using other elastic constants, but this scales in the same way).

This condition is called the "CFL" condition. It tells us that large $E$, small $\rho$, and small $\Delta x$ all force the solver to use a smaller $\Delta t$. In addition, this is a global restriction on the time step. It will pick the smallest element in your mesh to compute the stable time step. This is why a large difference in element sizes will result in a seemingly small time step compared to a mesh with uniform elements (that all happen to be larger).

As a way to check if this is what is going on, try increasing your density by a factor of 100. The solver should pick a time step that is ~10x larger than the one it's using now.

  • $\begingroup$ Would that mean it would be practically impossible to run an explicit simulation with millimeter scale steel model for one month for example ? $\endgroup$ Commented Mar 8, 2017 at 14:01
  • $\begingroup$ It's impossible to give much guidance on that without details of your model and the hardware at your disposal to run it. I have difficulty coming up with a real example for why you'd need something like that with full dynamics. $\endgroup$ Commented Mar 8, 2017 at 14:56
  • $\begingroup$ Well it's more a conceptual question. Would such a model allegedly take much longer time to solve in an explicit simulation if it is scaled in millimeter rather than meters ? $\endgroup$ Commented Mar 8, 2017 at 15:55
  • 1
    $\begingroup$ I'm not sure I understand your question. The units you use in your model are irrelevant. In fact, many solvers have no notion of units whatsoever, so it's up to you to ensure that they are consistent. At the end of the day, given two different meshes (presuming that you're representing the same physical space with your mesh and using the same material properties) the one with the smaller elements will require you to use a smaller time step. $\endgroup$ Commented Mar 8, 2017 at 17:23

The most commonly used explicit ODE solver in structural analysis is the central difference method. Because it is explicit, the solution becomes unstable if the time step is larger than a so-called critical time step. The calculation of this critical time step is straightforward and can be found in many references (e.g. page 808 in this text by Bathe ) and is given by

$$\Delta t = \frac{2}{\omega_{max}}$$

where $\omega_{max}$ is the maximum vibration frequency of the model.

It is generally too computationally costly to calculate $\omega_{max}$ exactly so, it is often assumed that the largest frequency in the model is approximately that of the ``smallest'' element. This frequency depends on the characteristics of the model and the specific finite elements used but is given by a formula in the form

$$\omega_e = \frac{c_e}{L_e}$$

where $L_e$ is a characteristic element length and $c_e$ is the wave speed in the material (e.g $\sqrt{E/\rho}$). The wave speed is the speed of a stress wave propagating through the material (or elements in the mesh).

Robust explicit ODE solvers estimate this critical time step during the calculation and adjust the numerical time step as necessary so that it is smaller than critical.


Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.