[CFD_Michele]

Hello everyone,

I'm doing a transient simulation of buthane evaporating in a radiator, using VOF and evap/cond Lee model. Furthermore, I'm giving the saturation temperature as input (piecewise polynomial).
The simulation is running but mass flowing in and out the system is not balanced. I'm computing mass imbalance through inlet and outlet, and I got 95% (mass_out - mass_in / mass_in).
So I analysed the mass flow at different stages in the system, and I noticed mass was "disappearing" when evaporation was happening. I changed some value and I got a good improvement (from 95% to 50%) but now I'm stuck again.

Here what I did:
Scheme from Coupled to SIMPLE (everything is 1st order, I tried to get accuracy with 2nd order but nothing changed)
Condensation frequency from 0.1 to 0.5 (I tried to change also evap freq but was useless)
In solution controls, Volume Fraction from 0.5 to 1

I tried to change also Volume Fraction Parameters and Interface Modeling, since I thought the problem was linked to multiphase and evaporation model but nothing (positive) happened.

What do you think? I did not find many helpful info on the web, but I read under-relaxation factor and evaporation/condensation frequencies should play the major roles.

Thanks in advance,

Michele

[vinerm]

For a transient simulation, instantaneous values of and will almost always be unbalanced. You need to compare their time-integral or time-average values.

[CFD_Michele]

Originally Posted by vinerm

For a transient simulation, instantaneous values of and will almost always be unbalanced. You need to compare their time-integral or time-average values.

Thanks for your reply!
I was thinking about that, but I didn't expect such a high error. Anyway, even if the sim is transient, I think now it reached a steady condition, since mass and pressure values converged.

Meanwhile I did some other change, moving the timestep from 0.001s to 0.01s, and that helped mass balance.
As you suggested I did the time average of the last 8 seconds, but the balance is still high (31%).

Furthermore, all the changes that I did to improve mass balance raised only the liquid fraction and not the vapour. And this is not good since I am trying to match a test where all the liquid evaporates.

[vinerm]

And how are you measuring the mass flow rates at the boundaries?

[CFD_Michele]

Originally Posted by vinerm

And how are you measuring the mass flow rates at the boundaries?

I set a Mass Flow Rate in Report Definition, on inlet and outlet boundaries.
I did the same for each phase.

[vinerm]

Since there is phase change, mass flow rate of individual phase will change, however, mass flow rate of mixture should remain same within a certain error. Usually, 1% is an acceptable error in multiphase flows but higher than that could be caused due to multiple reasons, such as, minimum volume fraction cut-off. If mesh is coarse, then, a volume fraction smaller than cut-off in a cell gets lost. But the error you have is rather high and cannot be explained by cut-off until and unless you have a very coarse mesh, which I don't expect.

[CFD_Michele]

Originally Posted by vinerm

Since there is phase change, mass flow rate of individual phase will change, however, mass flow rate of mixture should remain same within a certain error. Usually, 1% is an acceptable error in multiphase flows but higher than that could be caused due to multiple reasons, such as, minimum volume fraction cut-off. If mesh is coarse, then, a volume fraction smaller than cut-off in a cell gets lost. But the error you have is rather high and cannot be explained by cut-off until and unless you have a very coarse mesh, which I don't expect.

I tried to change cut-off, reducing it from the default value (1e-6) down to 0, but nothing changed. Anyway I'll try again since it was something I did when I had 95% of imbalance.

I'm using a 2.1 mln elements mesh, that's neither coarse nor fine. Now I am doing a coarser mesh in order to check mesh sensitivity.

Are cut-off and mesh density related? So if I have a finer mesh I would use a lower cut-off.

[vinerm]

Cut-off volume fraction is defined as ratio of the volume occupied by a phase and the volume of the cell. So, if the mesh is finer, the absolute volume occupied by a phase also reduces if the cut-off is kept same. 1e-6 is small enough and no need to reduce it further. Don't set it to 0, if you want to go lower, set it to 1e-9. But if cut-off is already 1e-6, reducing it won't improve the solution.

[CFD_Michele]

Thanks for your help!

I am now looking into outlet BC, I set pressure outlet and for the phase I selected Backflow Volume Fraction.
I am not sure about that since I am not expecting any re-circulation and I am expecting that the outlet flow is 99-100% vapour.
Should I use From Neighboring Cell? The guide is not so clear about that method.

[vinerm]

If Fluent does not report any flow reversal for your case, then it does not matter what option you choose. However, if there is flow reversal, then it matters. If the outlet is connected to a reservoir, such as, a tank or the open atmosphere, then depending upon the orientation of the outlet, it could either be light phase or heavy phase that could come in. However, if the outlet is taken midway in a duct, then it is better to use the option From the Neighboring Cells.

[CFD_Michele]

Hello guys, I'm back again.

I tried to change some setting as well as trying different meshes but nothing changed.

Now I am working on evaporation/condensation frequencies. Do someone knows how those two factors drive the simulation?
Default values are 0.1 [1/s] for both, and now I have 5 for evaporation and 7 for condensation. It seems to me that vapour fraction is highly influenced by both while liquid is not (I still have mass imbalanced > 10%).
Anyway, vapour fraction is more or less right while I still have a high liquid fration at outlet that shouldn't be there.

Any clues?

Cheers!

[vinerm]

The frequencies are tuning parameters of this model and need to be tuned to match with experimental data. If you are not getting enough evaporation, then increase the frequency. You can go very high, say, 1000 or even higher.

[CFD_Michele]

Originally Posted by vinerm

The frequencies are tuning parameters of this model and need to be tuned to match with experimental data. If you are not getting enough evaporation, then increase the frequency. You can go very high, say, 1000 or even higher.

Hi vinerm, thanks for your help!
It seemed to me that the frequencies are not directly correlated to each volume fraction, but maybe I am wrong.
In my case I was increasing evaporation frequency but I got a higher liquid fraction.

Anyway, now I have evaporation at 3 [1/s] and condensation at 8 [1/s] because I read that they have to be in a 1:10 ratio. If you say that I can go higher I will try that too.

Cheers!

[vinerm]

Ratio is not that important. Since the primary direction is evaporation, you should have higher frequency for evaporation and lower for condensation.

[CFD_Michele]

Originally Posted by vinerm

Ratio is not that important. Since the primary direction is evaporation, you should have higher frequency for evaporation and lower for condensation.

Hi vinerm,

Thanks for your reply.

As you said, I was expecting a higher frequency for evaporation than condensation. But as you can see from the enclosed picture I have the opposite! In the picture you can see how liquid and vapour fractions vary, changing the cond/evap frequencies.
I did different chenges to record the volume fractions behaviours. Starting from a frequency of 5 [1/s] for both evaporation and condensation, I increased evaporation frequency and decreased condensation, but I got an unexpected behaviour (increased volume fraction).
After that, in multiple steps, I incresed condensation up to 9 [1/s] and decreased evaporation down to 3 [1/s], and it seems it is working, even if I still have a high liquid fraction.
Eventually, just to underline this strange behaviour I raised condensation frequency to 30 [1/s] and you can see the vapour fraction got a steep ramp, while liquid didn't change so much.

Hope it was clear enough!

Cheers,

Michele

[vinerm]

How much vapor phase exists at the inlet or at the initial stage? Is it 0?

[CFD_Michele]

Originally Posted by vinerm

How much vapor phase exists at the inlet or at the initial stage? Is it 0?

No it's not zero. It is 1% of vapour at inlet, and it should be 99% of vapour at outlet (or close to 99%).
Now it's 90% of vapour at outlet, and mass imbalance is around 5%.

[vinerm]

And is there enough heat being supplied for this much vapor to form. Do note that an x volume of liquid leads to 2000x volume of vapor.

[CFD_Michele]

Originally Posted by vinerm

And is there enough heat being supplied for this much vapor to form. Do note that an x volume of liquid leads to 2000x volume of vapor.

I am not imposing the heat transfered but I defined the pipes and radiator temperatures as it was recorded during the test. Because at this stage I am trying to validate my system against experimental data.

Yes I imagine that there will be a huge expansion through the evaporation, but I did not understand what do you mean. How this is influencing my results? Do you think I have to measure my quantities in a different way?

[vinerm]

You might have used temperature boundary condition, however, you need to observe the heat being transferred to the liquid. If the heat transferred is not enough for the evaporation, then it will not evaporate. Also ensure that the material properties are given correctly, especially, enthalpies for liquid and vapor. It is their difference that is important and not their actual values.

Expansion of vapor is important since it requires that much space to be available. If the system is open, then it can flow out. However, if the space is closed, then vapor must be modeled as ideal gas.