convergence problem
Hi, I had to solve a problem with chemical reaction (not conbustion), and I have difficulty with convergence. All of Max RMS, is approximately 10^5 (good convergence), but Global balance of energy and mass fraction is superior with 15 % Can any one give me some idea of cause of this problem?
Thanks. Regards 
Re: convergence problem
Hi Mohamed,
You probably have transients which have not stabilized, regions of fluid which have not mixed and reacted for instance. Try increasing your timestep by a factor of 10. You may also want to plot the transient history of some gloabal quantities, energy balance for instance. Regards, Robin 
Re: convergence problem
Hi Robin, I test your suggestion, without result. When I increase my relaxation time, my solution diverge. For the moment I use local time Factor, I reach to converge but after much iterations. Is that the local time factor, influence the final solution ? Thank

Re: convergence problem
Hi Mohamed,
Don't use the local timestep factor. Use a physical timestep instead. Robin 
Re: convergence problem
Hi Robin, I tested with physical time factor. I do not manage to converge my solution. I do not have much experiment in CFD, to see the origin of this problem, but I think that the chemical processes are faster than dynamics process. What is difference between local and physical time factor, and what is their influence on the physical result? Thank

Re: convergence problem
Hi Robin, I tested with physical time factor. I do not manage to converge my solution. I do not have much experiment in CFD, to see the origin of this problem, but I think that the chemical processes are faster than dynamics process. What is difference between local and physical time factor, and what is their influence on the physical result? Thank

Re: convergence problem
Hi Mohamed,
When using a local timescale factor, the solver calculates a characteristic timescale for every control volume (L/V) and multiplies this local timescale by the factor you provide. This is sometimes useful for getting the code through a difficult startup transient, but rarely needed. Most of the time, a good initial guess and Physical Timescale selection will be better. When you choose a Physical Timescale or Autotimestep, the code will use a single timestep for all the controlvolumes, advancing all the equations together in time. Since the CFX5 solver is fully implicit, this timescale can be chosen to be as large as you want, though too big a timescale at an unstable part of the run may cause divergence. In general, you want to choose a timescale which is ~1/10 of the dominant physical timescale (advection time for instance, or 1/omega for rotating problems) at the start of the run. Once the residuals are coming down monotonically (after ~20 iterations), you can increase this timestep (to as large as you can get away with). By default, the same physical timescale will be used for all equation sets. However, when solving a steady state simulation, it is possible to define different timesteps for each equation. In your case, if the hydrodynamic timescale is large, you will want a large timestep for the massmomentum equation set. Since, the chemical process of iterest may occur much faster, you may want to define a smaller timestep for the mass fraction equations. Advancing the equation sets at different rates will not affect the final steady state solution, as the transient terms will cancel out at steady state. That said, the using the local timestep factor will not necessarily mean that the transient terms cancel out, as neigboring control volumes are advanced at different rates. So if you use a local timestep factor, you should ALWAYS COMPLETE THE RUN WITH A PHYSICAL TIMESCALE! Regards, Robin 
Re: convergence problem
Thank you Robin

All times are GMT 4. The time now is 07:58. 