Hello Everyone,

For a gas-solid two phase flow in a vertical pipe with chemical reactions, upwind method can lead a converged solution while higher resolution not. Could anyone please give some suggestions? Thanks.

Regards...Sherry

Hi Sherry

I'ven't used it to your specific case before. But High Resolution basically automatically set Blend Factor based on local solution field. So you might say, it takes quality of both 1st Order and 2nd Order Upwind Scheme to give you the best results. So you might not expect the same result as using one of those. You might try the ff:

1.Reduce the Timestep to say 0.3 of Physical Timestep. 2.switching to Specify Blend: say blend factor of 0.8 3.start High Resolution using the Upwind solution to initialise it

More help can also be found in the CFX5.7 manuel, under Solver Modelling, click on Advice on Flow Modelling!!

regards!!

If you meet a old drinking friend, you are more likely to converge to a the nearest bar than to converge to a nearest church with your old pastor.

Convergence in itself may not tell you much about the true value (accuracy). Say, I use upwind to start, if i still do not get the same level of accuracy, i could check other things, domain imbalance balance, pressure, etc.

I have done solid-liquid, gas-liquid and what I do is to start with upwing and then fine tune the blend factor, starting with a low blend factor and increasing it gradually. Sometimes i get poorer convergence with high blend factor, however, when I check those parameters I have metioned, including experimental data, i still fall back on to the asssumed poorely converged high blend factor simulation. In my case anything more than 5x1.0^-4 normalised mass residuals is poor. But please do remember this is also problem dependent.

Good luck Anne

Anne is right. Moreover, your specific problem might not have a steady state solution. Have you tried a transient analysis?

Hi Sherry,

The Upwind scheme is only 1st order accurate and therefore adds a large amount of numerical diffusion. Yes, upwind will converge faster, but to the wrong result. You would need a very fine grid to match the 2nd order accurate results provided by the High Resolution scheme. You would also find that as you refine your grid, the upwind scheme will become more unstable, since you will begin to resolve some of the turbulent structures.

There are two potential problems with High Res.

1. Timestep is too small. The High Res scheme will give you a sharper resolution of shear layers, for instance, and the high gradients across these shear layers is more likely to make them unstable. Another way to think of it is that the "numerical diffusion" introduced by the 1st order upwind scheme reduces your effective Reynolds number. In any case, if you grid scale is smaller than the large turbulent structures and your timescale is smaller than the turbulent timescale, you will resolve these turbulent fluctuations and your residuals will not settle down.

The characteristics are usually smooth, wavy fluctuations in the residuls, rather than sharp ones. The fix is to increase your timestep. The turbulent fluctuations should damp out and their effect will appear in the turbulence quantities, such as turbulent kinetic energy and dissipation.

2. Timestep is too large. The High Resolution scheme uses an active blend factor. Basically, you add a second order correction to the 1st order upwind term. If you add the entire correction, you have a fully second order scheme, but risk numerical overshoots and undershoots (numerical dispersion) in the solution. The High Res scheme multiplies this second order correction by a blend factor, beta, which is between 0 and 1. The value is calculated based on the local solution field in order to keep the solution bounded.

Problem is, since Beta is calculated from the local flowfield and it is also used to calculate the local flowfield, it can have feedback into the system. In short, it's a non-linear term. If the value of beta is changing rapidly in an area of the solution, it will manifest itself as sharp changes in residual from one iteration to the next. The solution is to reduce you timestep, which will relax the rate at which these changes occur.

It's generally a good idea to use a large timestep at the beginning of your run. This will help get you through the start-up transients quickly. If you don't converge with a large timestep, increase it or decrease it based on what you are seeing. You can also plot values such as forces at boundaries, averaged pressures at boundaries, montor points, etc. which can help you determine if you are still going through a transient or not.

Lastly, you can view the residuals by selecting them to be output to your backup or results file (from the Output Control dialog in Pre). It's a good idea to add the residuals to backup files, since these are what you will review during a run. Create a new variable in Post equal to the absolute value of the residual of interest ( abs() function) and create an isovolume of the residuals above your target criteria. The resulting isovolume represents the region where the solution is still changing. If it is away from your region of interest, you can probably ignore it.

If you are still confused, go to the ANSYS CFX Community Site and view the tech tip entitled "Monitoring and Improving Convergence". If you are still in doubt, you can always contact ANSYS CFX support.

Best regards, Robin