Author Topic: How do I set an appropriate Physical timescale size for steady state calculation  (Read 1011 times)

Offline pitney1

  • Jr. Member
  • **
  • Posts: 62
  • Reputation: +0/-0
  • Searching for solution
    • View Profile
How do I set an appropriate Physical timescale size for steady state calculations?

Offline william

  • Full Member
  • ***
  • Posts: 151
  • Reputation: +14/-0
  • Know it, share it.
    • View Profile
For steady-state problems, the CFX-Solver uses a robust, fully implicit formulation so that relatively large timesteps can be selected accelerating the convergence to steady-state as fast as possible. However, if the timestep is too large the resulting convergence behaviour will be ¿bouncy¿. If this is observed, then the first thing you should try is to reduce the timestep size, say, by a factor of four. If there is no noticeable improvement, then the convergence problem may be caused by another factor. Note that if the timestep is too small, then convergence will be very slow.
Note that also depending on your initial guess, a significantly smaller timestep may be required for the first few iterations of a problem.

In addition to the advice in the following sections, you will probably require a small physical timestep for the following situations:
- poor mesh quality
- transonic flow
- large regions of separated flow
- Openings with simultaneous inflow and outflow
- Free Surface flows (in these cases it is often sufficient to use a smaller timestep only for the Volume Fraction equations)
- Multiphase flows.

In order to set an appropriate Physical timestep size, you must check which phenomena is dominating your flow:

1) Advection dominated flows

The physical timestep size should be some fraction of a length scale divided by a velocity scale. A good approximation is the Dynamical Time for the flow. This is the time taken for a point in the flow to make its way through the fluid domain. For many simulations a reasonable estimate is easy to make based on the length of the fluid domain and the mean velocity, for example ?t = L / 2U

If the domain contains largely varying velocity and length scales, you should try to estimate an average value. If you get divergence, check in the Output File that your timestep size is not larger than the Advection Time Scale value given in the Average Scale Information at the end of the run. A ¿small¿ timestep can beconsidered to be less than 1/3 the smallest length/velocity_scale in the simulation. Values higher than this can be considered a ¿large¿ timestep.

2) Buoyancy driven flows

The maximum physical timestep size may be estimated using the following relationship:
?t_max ~ sqrt(L / (ß g ?T))

L is a length scale associated with the vertical temperature gradient
?T is the temperature variation in the fluid
ß is the thermal expansivity of the fluid
g isthe gravitational acceleration.

3) Free surface flows

The timestep for free surface flows should be based on a L/U (Length/Velocity) scale. The length scale should be a geometric length scale. The velocity scale should be the maximum of a representative flow velocity and a buoyant velocity, which is given by:
U_buoyant = sqrt(g L)

In addition, it is often helpful to reduce the timestep for the volume fraction equations by an order of magnitude below that of the other equations.

4) Multiphase Flow (Inhomogeneous)

For bubble columns, use first a fraction of the bubble rise time for a total of one rise time, then increase the timestep to a fraction of the fluid circulation time. If species mass transfer is modelled, it can take a considerable amount of time for some species to come to equilibrium. Try setting the timestep size for the mass fraction equations to a large value if convergence is very slow for this equation class.

For dilute particle cases, use a fraction of the dynamical timescale for the momenta. This is essentially a fluid travel time through or around the region of interest.
If volume fraction convergence is slow, then the timescale for these equations can be increased suitably.

5) Combustion

It is often useful to apply a largertime step to temperature and species than the remaining equations. Try starting with a relatively large timestep to let the material sweep through the domain. You can reduce the timestep later to achieve better resolution of the simulation conditions, and therefore convergence.
When using the Finite Rate Chemistry model, using a timestep that is too large at the beginning may cause the solver to fail due to reaction rates not converging. Under these circumstances, the timestep must be reduced.

Finally, note that it may happen that simulations which are run in steady state mode will have difficulty converging, and no matter what action you take regarding mesh quality and timestep size, the solution does not converge. This could be an indication of transient behaviour. If you have run a steady state calculation and you see oscillatory behaviour of the residual plots, you can test to see if you are observing a transient effect by reducing/increasing the timestep size by a known factors. If the period of oscillation of the residual plot changes by changes the timestep size, then the phenomenon is most likely a numerical effect. If the period stays the same, then it is probably a transient effect.