everybody:

this has never happened to me before. I'm encountering convergence difficulties in the unsteady simulation of laminar reacting flow. as always, I had generated a semi-converged steady solution (segregated solver, 2nd order schemes, DO radiation, single step Ch4-Air chemistry). instead of the residuals falling even more (which used to be the case earlier for another reacting flow simulation through a simpler geometry), they go up by an order of magnitude, especially the continuity one (which is the only one which refuses to come down).

I've reduced the time step to 10^(-8) s, but it still doesn't work. normally, for the kind of laminar combustion I've been working with, a time step of 10^(-5) s was a sufficiently low step size.

is grid adaptation a possible remedy ? based on what criterion should I adapt the grid ? I've checked gradients, and the only gradients which were high were the enthalpy ones [O(10^3)].

I'm using the second order scheme for pressure and PISO for p-v coupling.

the residuals are in the range of:

continuity 1.7377e+00

x-velocity 1.5850e-05

y-velocity 1.7548e-04

energy 5.3650e-08

do-intensi 8.7784e-08

ch4 6.8593e-08

o2 6.8611e-08

co2 7.2894e-08

h2o 7.4620e-08

(1). When you have convergence problem, make sure that precision is not a problem in your code in the first place. Try double precision math. This is the first step. (2). The mesh is a place where something can be done, if your mesh is highly stretched or distorted. Only you know the solution. (3). Beyond this point, the only thing you can do is to try out different options available in the code.

john:

I changed the solver setting to DP. the continuity residual fell by one order of magnitude and is maintaining a value of approx 0.45, not going down further.

as far as the mesh is concerned, I'm using a quad grid and have checked for stretching. the equiangle skew is fine and so is the cell volume range.

I'm confused because the momentum, energy, radiation and species residuals are really low but continuity stays so high. any possible explanation for this behavior ?

as far as the solution is concerned, I've compared my temperature data with experimental results and they seem to be very close. also, the physical phenomena of flame stabilization over the honeycomb ceramic flame holder is working fine. the profiles of velocities as well as the flame speed is near perfect, which comes as a surprise because the losses to the atmosphere from the quartz chimney, that we've been using in the experiments, is not properly defined and I'm using an arbitrary heat transfer coefficient for free convection.

thanks anyway for the suggestions. at least the continuity residual came down one order!

prateep

Hi Prateep,

in my calculations, increasing relaxation for pressure and decreasing it for momentum very frequently decreased the continuity residual.

Petr

Try the following. 1). Write an interpolation file with all the variables you are solving. 2). Initialize again the solution (the values of the variables do not matter, you just want to nullify the residuals). 3) Read the interpolation file. 4) restart the case again. It might work. I myself many times observed this behaviour. Very small residuals for all variables except mass, and the solution was very much converged (frozen monitor values, etc.). This occured when I have Fluent open for a cas/dat files and then I start running for another set of BC's for example (e.g. change the velocity value at an inlet). So, I think that Fluent keeps info from previous states. I don't think this is exactly your case but try the above.

Also, you may take a look if you have a small number of cells that keep your residual high (Display/Contours/Residuals/Mass Balance), while the rest flow field is o.k. If this is the case check first if the residuals remain high at specific cells or if they move around in a certain region from iteration to iteration. If the problem is located in a region adapt this region only and give it a try.

Hello,

My name is Paulina. I was wonder if you can help me? I have a problem with my simulation, exactly with convergence. I'm modeling liquid-liquid systems (dispersion)in the static mixers. The first fluid is a water and the second one is an engine-oil, with the density 920 [kg/m^3]. I use an Algebraic Slip Model in Fluent 5.4. The flow is turbulence, so I have also two additional parameters: k and epsilon. I tried to solve my problem many times and to do this I made many steps. Once I changed the solve controls, I decreased them to the level about 1e-03. But it doesn't help.Last time I started my calculation from 1e-06 for k and epsilon and the another parameters for example slip velocity about 1e-04. Unfortunatly I haven't got a solution.Also I should tell that I modeling this case for laminar flow and I obtain a solution very quicly. So I can't understand my problems with this case. Also I should tell that to simulation I use the "multigrid solver" too. I know that it isn't easy case because I have very complicate static mixers, but do you think that there is a possibility to not obtain a solution? I would be very happy for any advice! Thanks! Best regards!Paulina

Is it a steady state problem? Try solving it unsteady anyway, it might help. When you say that you do not get a solution what do you mean? 1) divergence or 2) high residuals?

I am afraid that I am not familiar with Algebraic slip model but usually multiphase models are quite unstable and difficult to converge. What I do know is that decreasing under-relaxation so much, means that the problem is somewhere else. Probably to the initial values of k and epsilon. Values of 10-6 for both does not quarantee that you are going to get a solution. You must try combinations of k and epsilon initial values that will not lead to divergence, so eventually you will get a solution (steady state problem).

Hello, thanks for your response. When I told that I haven't got a solution I mean that I obtain a high residuals. Now, I will try solving my problem as unsteady. Also I started my calculation using only flow, volume fraction and velocity slip in the "solve controls", but I put the velocity for wather and oil for turbulence flow. As you know I got the solution for the laminar flow using Algebraic Slip Model. I'm going to join k and epsilon when I get the convergence. I hope it will help. Also I will remember about your advice concerning to k and epsilon initial values. If you have more idea please give me a know. Thanks for your advice and time. Best regards. Paulina