Sounds like a software problem, not a chemical one. Ditch the canned CFD code.

Thank you so much, Dudley.

I am using FLUENT. Maybe I should try Openfoam.

By the way, FLUENT suggests the Eddy Dissipation Model should be used for one-step or two-step reaction. Multi-step reactions with EDM will generate unrealistic solutions. Because EDM tends to give every step of reaction a same reaction rate. But I am not sure if it is the reason for non-conservation of atoms when using two-step reaction.

Just a question: could you please show the convergence plot of your residual values for this result in addition? Otherwise no comment can be made. With weak convergence any error in a CFD solution could be possible.

Regards,

Dr. Th. Frank.

Is the overall mass balance fulfilled, i .e. does the total mass flow going in equal the total mass flow going out?

Also, why are temperatures so low ( I assume the unit is °C)? With stoichiometric CH3OH / O2 combustion, you should have an adiabatic combustion temperature of about 2650 °C.

I agree that the overall element balance should be fulfilled anyway in a converged solution but are these low temperatures ntentional? For non-conventional combustion processes like oxy-fuel combustion, small reaction mechanisms may lead to very unphysical results. Models with look-up tables (e. g. PDF-equilibrium or PDF-Flamelet) are often better in this context.

Dear Dr Frank,

Thanks for your interest. The residual values of continuity is lower than 1e-2. And other residual values of species and energy are lower. But small fluctuations can be seen after many iterations. I forgot to save the picture of residual values. I will re-run the simuluaion and attach the residual picture.

Dear Dr Leicher,

Many thanks for your reply.

- the mass balance is fulfilled. The mass difference between inlet and outlet is less than 1e-2.

- the low temperature is because the concentrations of the O2 and CH3OH are very low. The oxidation occurs in a reactor filled with supercritical water. The Jet injects the O2 and CH3OH that are in water solution.

- Thanks for the suggestion of LUTs. But I am not familiar with that. Do you know how to get it? In literature or via experiment? I am afraid that my experiment condition is too harsh to obtain the LUTs. Because the reactor must stand with the high pressure and high temperature of supercritical water. It is hard to put thermal couples inside.

Many thanks,

Zhaojian

A residual value (In ANSYS Fluent this is a mesh averaged RSM residual !) of 1.e-2 is not at all a converged solution. Corresponding errors in the conservation of physical properties are thereby very likely.

Regards,

Dr. Th. Frank.

@Thomas Frank

Hi, Dr Frank.

Thanks for pointing out a potential solution to this problem. I have tried to make the case converged. I tried all methods that I know(Use first order upwind first and then use second order upwind for momentum and energy equations; ajust the relaxation factors for pressure and momentum; use finer grid y+~1). But the residual was just fluctuating between 1e-2 and 1e-3. Do you know some other tricks that might be helpful for convergence.

Some basic info:

I ran about 7000 iterations, monitoring the temperature, mass flow rate and species flow rate of outlet. Finally, all the residual values and monitored values have small fluctuations in a small range. How can I get rid of the annoying fluctuations :(

Hopefully, I will upload a residual figure here. Many thanks for your time.

Best,

Zhaojian

Do you have the same convvergence problems if you run your case without chemical reactions?

Zhaojian Liang : I do not know the details of your setup. But for steady-state simulations I'm regularly using: coupled solver, pseudo-transient solution algorithm, HOTR=on. Then you can play with the underrelaxation factors and trying to set the pseudo-timescale as large as the stability of the solver is allowing it. By that you can dampen out small-scale fluctuations, which might be triggered by inherent small-scale transient phenomena in the physics of the studied flow.

But there is no guarantee and no "user right" to obtain a steady-state solution for an inherent transient flow. In that case you need to run the case as a transient solution and after establishing fully developed flow conditions, you need to apply time-averaging for a statistically representative timeframe of your flow solution. At least in the transient solution any flow case should be able to get converged. If this is not the case for your application, something in your physical setup might be not yet right (e.g. contradicting boundary conditions).

Regards,

Dr. Th. Frank.

Hi, Dr Jörg Leicher. Thanks for your question. I don't have the convergence problem without reactions in my case. And for the case with a one-step reaction, the residual values damp quickly. The annoying fluctuations occur after I replace the one-step reaction with a two-step one.

Dear Dr Thomas Frank. Many thanks for sharing your experience. I will try on your suggestions.

I re-run the simulation today. The residual figure and monitored data are shown in the attachments. The simulation might be not well converged since the residual of continuity is at around 1e-1 with small fluctuations. All the residuals just keep dancing around some values but not dropping. That is confusing. I should try to solve the convergence problem and then check the conservation of atom 'C'. Many thanks for all the answers. They are very helpful to me. I will let you know if I have further developments on this problem.

Hi, my friends. I fixed the problem of non-conservation of atoms when using two-step reactions in ANSYS Fluent today. I am so glad now. I'd like to appreciate all of you Thomas Frank Jörg Leicher Dudley J Benton who tried to do favors.

The reason for the non-conservation of atoms and bad convergence is that I used the wrong order of the material list. My case involves a mixture of CH3OH, O2, CO, CO2, and H2O(bulk species). To solve the mass field of this case, the CFD solver needs to solve 5 mass transport equations for every species. But ANSYS Fluent says, I am gonna solve only 4 mass transport equations to acquire the mass fraction of 4 species, and the mass fraction of the last species is calculated by 1 minus the mass fractions of the other four species. For accuracy, we need to tell ANSYS Fluent that H2O is the bulk species, just solve the mass equations of CO, CO2, CH3OH, and O2 will be fine. To do so, we need to put the H2O at the last position of the material list, shown in the figures attached.

By mistake, I set the product CO, instead of H2O, as the bulk species. Then, I got the non-conservation of atoms and bad convergence. After I amend this mistake, all the things go well -- conservation of atoms and quick convergence.

Interesting finding. And glad to see, that you found a way to fix your issue. Shouldn't the solver issue some kind of warning to the user in such a case?

Best regards,

Dr. Th. Frank.

Hi, Dr. Thomas Frank

There is no warning when running the solver. That issue is only mentioned in the tutorial. They should add a warning though.