Dear everyone,

I am preparing model for mass transfer and reaction depending on temperature, which is using dynamic meshing method (transient condition).

2 UDS are calculated in my model, and they are transfered and reacted each other. Of course, appropriate boundary conditions for tempeature and UDS are given in this model.

To calculate mass transfer and chemical reaction, temperature has to be soloved first.

The concerning point is that temperature calculation has to be converged prior to mass transfer and reaction, since mass transfer and reasction are the function of temperature. However, calculation for temperature, mass transfer and reaction are claculated at same time so that mass transfer and reaction are being calculated from unconverged temperature. If I am using steady state, I can manually control calculation sequence. But, this is unsteady condition.

Could you let me know what method is apprpriate to converge temperature before calculating the mass flow and reaction? In a given time step, temperature needs to be converged. Then, mass transfer and reaction have to be calculated. In next time step, this sequence needs to be repeated to get correct calculated results.

Your kind reply will be very much apprciated.

Thanks,

J.W.Ryu

Dear J.W.Ryu,

I don't know exactly what is the situation of that simulation. But let me to turn basically to the Heat-Mass Transfer/Reaction problem and the dependency of thos phenomena. To do it, I just introduce a very simple case. Suppose that there is an elemental volume of fluid caled X that heat is transfered to it. Component "A" in this element has a concentration Ca at that volume. The concentration of this component in the neighborhood volumetric elemnt is Can. Also consider that those there is another components like "B" and "D" which can react to each other and generate (or consume) component "A". So in this case we can simply say:

Heat transfer to (from) element X: change Temperature

Reaction: nCb+mCd-->Ca R=Ka*Cb^n*Cd^m

Mass transfer: j=Km*dCa/dx

Now the point is, as heat transfered, the value of Ka (reaction constant) will be changed as:

Ka=Ko*T^w*exp(-Eact/RT)

which "w" will be 0,1/2 or 1 according to Boltzman, Collision or Transient theorem.

Also the value of Ca (depends on fluid) will be changed. It means that the Reaction will be effected and so the value of Ca will be changed and also the Temperature since of Reaction will be differed. So it means that also the rate of Heat transfer will be changed and so the value of mass transfer since of chage in Km and Ca will be changed.

I mean that I think the judge that the Temperature has to be converged and then the Reaction and Mass Transfer has to be solved is basically not so true.

The idea in programming for such a case in mass transfer was like this (as previously I did):

1.Geuss Temperature, T 2.Solve tha value of Ca since of reaction, if the rate of reaction is more rapid that the rate of mass transfer. This should be cheked by an assumption which is seting the T and Ca and find out how much component "A" will be transferd and Produced (or consumed) by reaction and comparing them. I think that there is a Dimensionless number (like Sc and or the other that I forget) that can judge about it. 3.correct the temperature changed by reaction. 4.Obtain the value of mass transfer. 5. correct the values of fluid and temperature and pressure in the system. 6. Solve the heat transfer.

So I think that they are conjugated toeach other. But I think it is better to set the temperature in various constant values and then solve the mass and reaction. Next to it you will understand the sensibility and the effect of temperature on the solution. By this you can judge that at first which part has to be solved.

I hope that a little bit it should help you.

Best regards Koorosh

Dear Koorosh,

Thanks for your comment. But, I think you did not undersand what I asked. Two components are chemically reacted in my model. But, it was assumed that no heat exchange is happened. therefore, I just need to solve enery equation and UDS for two components. I am using dynamic meshing of Fluen v6.0.20 so that all of equations are solved at same time. But, UDS needs to be solved temperature to get much precise solution. So, I asked how I can use sequential calculation at dynamic meshing method, which are temperature first and then UDS calculation.

Could you let me know your good idea?

Best regards,

J.W.Ryu

Dear J. W. Ryu,

I'm so sorry that understood you wrong. Unfortunately I hav no experiences in that kind of simulation. So please appologize me.

Thank a lot and with best regards

Koorosh

Dear Koorosh,

Don't mention it. Thanks for your help and kindness.

With best regards,

J.W.Ryu

I haven't used dyanmic meshing, but I don't actaully see how it makes a big difference to the solution process anyway.

At each time-step Fluent will use an iterative method to converge all solution variables. In a fixed grid simulation once convergence is obtained, Fluent increments the time step to the next level and repeats.

Now in dynamic meshing there can be additional source terms for the mesh motion (which may or may not depened on the solution itself) which need to be added to the conservation equations. However, I assume/imagine that the same iterative method is still used.

So, for your coupled heat and mass transfer problem you will need to solve all variables until all convergence. The idea that you can converge temperature independent of mass and chemical reaction is in general incorrect. In these problems there is often a strong coupling between the physics and that's why iterative methods are needed to solve the non-linear equation sets. For some classes of problem of course one effect may be insignificant and a simpler solution process can be used.

Anyway, in the end, what I'm getting at is that at each time step you will need to solve Fluents standard equations and your UDSs simultaneously. Fluent should then increment the time-step and do the dyanamic meshing once convergence is reached.

I've done this for static meshes and it works fine.

Have you got your algorithm working for a static mesh? If so, what's causing problems in the dyanamic mesh model??

Greg

Dear Greg,

Thanks for your comment. Your estimaion for computing algorithm is correct.

In static meshes, Fluents standard equations and my UDSs were computed simultaneously, as same as dynamic meshes.

Frackly, my UDSs are function of Temperature so converged temperature field is needed to solve UDSs.

I am calculating point defects diffusion and interaction in solid material, and UDS are corresponding to two different point defect, which are vacancy and interstitial atom. Diffusion and pair annihilation of vacancy and interstitial atom in solid matrix are dependent on temperature, and these are computing in solid assumed as fluid. With given drift velocity (convection term) of solid, dyamic meshes are generated. Of course, convection term of mass transfer is considered with this given velocity.

Yes. all scalars are calculated at same time. But, as I mentioned above, UDSs need converged temperature field to compute. So, I posted how I can use sequential calculation of temperature and UDSs.

Anyway, simultaneous calculation showed quite reasonable result so far, since converging speed of temperature is much faster than that of UDSs in given tim step. In converged temperature within short time, it seems UDSs are being converged.

If I can realize clear sequential computing of temperature and UDSs in given time step, it will be much creditable results.

Thanks again for your comment.

J.W.Ryu

I think I understand your problem (a little).

However, why do you NEED a converged temperature field before calculating the UDS???

If your UDSs don't have a two-way coupling with the energy equation (and other equations such as momentum, or have a very weak coupling), then yes, you can solve the system by solving the main flow equations first and then sequentially solving the UDSs. However, this is really a special case.

The standard Fluent algorithm enables one to solve the general case involving two-way coupling between each pair of transport equations. Thus in the early stages a temperature estimate will be used to solve your UDSs etc., then as iterations proceed a converged temperature and UDS field should develop - which is your desired solution.

Thus, even though you may save some time with a sequential algorithm, the fully-coupled algorithm in Fluent is in fact the more comprehensive and hence more exact method. In my view, the sequential algorithm is a "special" case of the general coupled algorithm.

Basically, the algorithm in Fluent should solve your problem without any worries (though it might not be as efficient as a sequential method).

Now if you want to try out a seuqential method, this is possible to implement.

First turn off the solution of your UDS equations in the solve/control panel. Only solve for the standard flow variables - u,v,w,turbulence,temperature,species,radiation (whatever you have). Then obtain a converged solution. As I gather your UDSs don't generate any source terms back in these equations so this should be fine.

Next, you can turn off these equations and then turn on your UDSs. Solve them to convergence. This is the sequential method you talk about. (The only problem here could be how Fluent applies the dynamic mesh update - after the for the first set of equations converge you don't want Fluent to apply the dyanmic mesh. I imagine you can configure this using the text interface by not doing a full time-update - see tui manual).

Now, if you have some weak two-way coupling you can see its influence by comparing the solutions for the two methods. That will tell you something about the sequential method. However, in both cases the standard solution algorithm will give the correct results.

Its also worth noting that turning on/off equations can be useful in obtaining solutions where strong two-way coupling exists. This and under-relaxation are often needed to get solutions at all!

Greg