Has anyone come across a problem that, not matter how well 'converged' doesn't give anywhere near a proper heat balance when viewed according to: REPORT FLUXES

Total Heat Transfer Rate

Select all boundaries and then hit compute.

The problem is a combustion problem that is 'converged' so that all residuals are below 1e-7 and have all bottomed out with no noticeable change in any variable over 1000 iterations. Results look ok, but total heat transfer rate is miles off. For added info... the combustion 'box' is adiabatic (done to figure out what's going on). The mass flow rate balance in the flux reports is 1e-9 kg/s which I'm fairly happy with and the predicted exit gas composition is as expected.

By the way, the imbalance reported is such that I am getting twice as much heat out of the exit as I put in with the fuel. (patent pending......)

(1). In any CFD calculations, I normally use hand calculation to compute and check the global flow variables and performance. (2). So, try to use hand calculation to check the average velocity, temperature, density, pressure, total pressure, and mass flow rate,.... (do not trust any GUI)

Make sure check your definition of heat of formation for the reactants and define those in SI units in Fuent. We had found an unit conversion bug in the earlier version of Fluent. I am sure it has been fixed. But SI units seem always safer.

Hi Jason! I had the same problem and you can get rid of it this way: After your solution is converged othervice, select solution control and set the energy to be the only equation solved (if you model radiation select that as well). Set the underrelaxation factors to 1 for the selected equations. Let the iteration converge (will take only a few iterations; depending on your model obviously): and you have a solution that have correct energy balance.

Best Regards,

Jouni

Thanks for the input Jouni. Unfortunately I've already tried all the convergence tricks without any joy. In the interim I've been playing around with this problem. Wrote a simple spreadsheet to calculate what the true enthalpy should be.....miles out from fluents value on my 'odd' case. However, when applied to a tutorial gas combustion case it's more or less spot on (indicating no errors in spreadsheet at least). For the earlier comments on gui's, I've been doing all of this from the text interface (not that it's much better....). Thought it might be a UDF I invoke but same prob occurs without it. Support reckons on turning species inlet diffusion off but this doesn't affect things...I get a match on inlet enthalpies. I'll crack it, and, if there's a general caveat, I'll post the info.

Have you cracked it Jason? I think I've got a similar problem and was hoping someone could post some useful answers.

Hmmm this sounds really interesting! Can you please justify why you're doing this please. It is my opinion that you are decoupling the heat transfer calculation from the rest of the flow, or once you have the heat transfer 'converged' do you start solving the rest of the equations again?

allan

It does sound weird, doesn't it.

I basically have found that at least in my cases the heat balances affect very little little to do with the rest of the equations in Fluent. I have no idea what is behind it, maybe somebody from fluent could explain why it behaves like it does. It works in practice though.

I normally iterate with all the equations after iterating the heat balances, but as I said it does not necessarily cause very much changes.

Nowadays, I usually change all the underrelaxation factors for energy (energy, radiation) into 1, that way the energy balance follows more closely the "real" values during iteration.

Some people tend to decrease underrelaxation factors when they do not get converged energy, but fluent does not work that way.

Best regards,

Jouni Valtatie

It is iteresting to hear you say that the flow fields do not change much when you solve only for heat transfer. What type of geometry are you modelling?

allan

If you are a user of fluent try it yourself, this is not a question of physics, but Fluent's peculiar way of handling heat balances.

You may have a calculation result where temperatures are something you would expect, but heat balance is wrong by miles. Then you can iterate the heat balances alone, without the temperatures changing very much. I can only conclude that fluent does not use its heat flux to the boundaries in order to compute fluid temperatures involved.

I hope that somebody from fluent comments on this one.

Best Regards,

Jouni

I do use fluent, and some others have tried this method and they say it works. What I find very difficult to believe is that this is a valid method. I thought that cfd codes worked out flowfield temperatures velocities etc based on boundary conditions. If the temperatures are more or less correct and the heat balance is wrong then I would expect the heat transfer coefficient to be wrong. genereally heat transfer coefficients are functions of velocity. Therefore I suppose that either the way that fluent calculates heat transfer coefficients are wrong or the predicted velocity next to the wall is not correct. I just can't understand this illogical approach. Like you I hope someone else can comment on this.

allan

I've used the same technique. It is fully valid if the flow-field is not affected by your temperature/energy field. This is also the case in many applications. It is of course not valid if you have bouancy effects or if you have significant density changes due to temperature variations. You can also use this to check how a change in a temperature boundary will affect your global temperature field - what you are doing is basically to solve heat-conduction and heat-convection in a frozen flow-field.

thanks jonas, I totally agree with you, but this technique appears to be applied almost at random by some people where it is not really applicable.

allan