Hi All,

I do not know whether this is a good approach for checking if a problem has been properly set up. Apart from temperature check and mass balance check, can one use Fluent to check the total heat flux at all inlets and outlets to see if they will balance as is done in the case for mass balance? I have done it and the heat fluxes could not balance out. I thought the difference will be as a result of the heat release during combustion. Using the heating value of the fuel and the fuel mass flow rate, i computed the heat of combustion. This value was far greater than the difference i had after adding the heat fluxes from the inlets and outlet. My mass balance check was alright and so was the adiabatic temperature check.

Is there something I am doing wrong? I need help, please.

James

I was confused about the same issue and think I was able to work through it with the help of my Fluent support engineer.

At the outlet boundary, sensible heat is negative using their convention. For combustion products, the net chemical heat (or sums of the heats of formation) will likely be negative, but since it flows out the boundary the chemical heat will be positive (-ve times -ve). So summing sensible and chemical heats at the outlet will give the difference between the two, and a much smaller number than the heat of combustion.

Hope this helps.

Hi Allan,

Thanks for your help. I want to clarify this other issue. In case your mass flow inlet is now changed. What I mean is that I am looking at droplet combustion where my droplets size, velocity, position and mass flow rate are being provided by an external file using the DPM panel in Fluent. How can one calculate the total enthalpy in this case for the mass flow inlet?

Regards,

James

The first part is to work through the flux menu and make sure you are satisfied that the energy balance is working - splitting up sensible heat and heats of formation of species using Fluent's conventions for the signs.

Then you can use the Fluent Report->volume-integral->sum of the DPM Enthalpy Source to find this value in your domain.

The magnitude of DPM Enthalpy Source should equal the net-heat-transfer reported from the flux report of total heat transfer, once the case has converged.

Hi Allan,

Thanks so much for the insight.I am so grateful. I did what you suggested and it worked out.

Have a good day.

James

hello i need help about energy when starting convergent in combustion it convergent some iterate but after that it goes on high and so divergance detected AMG solver Temperature message given help about this all radiation and energy on

i would seriously advise you to do some simple example problems first then to directly doing a combustion analysis. i do have done lot of work with combustion and things are not so straight forward with combustion as you might excpect.

you have not mentioned what combustion model you are using, AMG solver divergence suggest that you are trying to work with finite rate chemestry, with large number of species in it.

try a less number of species on a realtively simple mesh, and see you could get the solution to converge or not. then solve a very coarse mesh problem which is similar to your actual case and try to get the solution on it, then finally move to the best mesh you could make.

and when you mention your problem, it would be kind of you to mention what exactly you are doing, since half question do not result in even half answers.

rest, best of luck with your work

Hellow ,

I am doing the premixed combustion analysis. the combustion model is cylindrical along with the heat exchanger.i have got the converged solution. i have set the relaxation factor randomly. i want help about how to decide the relation factor. i also want to know that it is advisable to use the default values of the relaxation factor.i have carried out non-premixed combustion analysis.here the relaxation factor for the convergence of energy is kept 0.3 But as we move towards 1 the convergencxe process becomes very lengthy. so i want to know on what factors the relaxation factors depends and how we have to decide its value.thank you.

Hi Allan,

Sorry that I have to disturb you.I will be grateful if you can offer me some help on this issue. I have had a coverged solution for a steady oil case (to be specific gas oil, C16H29) and now i have to switch the simulation to unsteady for both the continuous case and the droplets injection. I actually do not understand what fluent does when the droplets injection are changed to unsteady. I have made the following observations:

1. During the steady calculation, number of particles tracked was 16000. This number stayed pretty much the same for all DPM injections. Now, it is fluctuating and as of now, it is at 5833. The number of droplets evaporating has also droped. Would this affect my flame temperature since my impression is that i am having a leaner mixture now. What i do not know is what happens at the end of the injection time. I expect that it should track the 16000 particles. Is this observation right?. If so, would this remain the same after that or will it begin to fall when injection ceases? What looks good is that the injection rate is constant at 160 particles at every time step.

2. I specified an injection start time of zero and a stop injection time of 0.05 and a particle time step size of 0.001. Fluent is not using the particle time step size i specified for the DPM iteration but rather it is using the flow time step size of 0.00005, even though in the DPM panel, i specified particle time step. Does it mean that fluent automatically advances the particle at the flow time step and uses the particle time step size for solving the DPM flow equations?

3. From your experience, what is the best set up approach for unsteady droplets simulation in Fluent in order to achieve optimum results? I am using the k-epsilon turbulence model and with this, i was able to switch the turbulent dispersion of particles on and changed the default default value of the time constant from 0.15 to 0.3.

My intension is to switch later to the LES turbulence model. Any suggestions on any precautions I am to take will be appreciated.

Counting on your usual assistance.

James

Hi Mann As you know relaxation factors affect on solution time,but there is no way to find out which value of URF(Under Relaxation Factor) is the best value. It is just experimental to find best value of URF for any kind of problem. But default values recommended by FLUENT are almost usefull with exception of values of 1 . In these cases you must change factors to a value lower than 1.Certainly changing default value of 0.3 to a greater value causes to a longer time of solution.

*snip* Certainly changing default value of 0.3 to a greater value causes to a longer time of solution. *snip*

I think u mean 'lower value'?

Hi,I mean it is better not to change value of 0.3