evapPhaseChangeFOAM

sahas · September 6, 2013, 05:03

Quote:

Originally Posted by Sasy

Hi Alexsander
Thank you for Reply
I see now...

is this solver that you are attach,simulate the evaporation at the interface between fluid and gas by increasing Temp?is this solver have source term for phase change?
i dont work with interPHasechangeFoam solver....but i think this solver simulate Cavitation with reduce pressure....

Yes, you are right: original interPhaseChangeFoam was designed for cavitation but the numerical model is also suitable for evaporation (cavitation is just some source terms in alpha equation, evaporation is too). The dependence of evaporation source from temperature should be in evaporation model (source in alpha equation). In our model such dependence is present. So all the answers to your questions is "yes"

Sasy · September 6, 2013, 05:17

Quote:

Originally Posted by sahas

Yes, you are right: original interPhaseChangeFoam was designed for cavitation but the numerical model is also suitable for evaporation (cavitation is just some source terms in alpha equation, evaporation is too). The dependence of evaporation source from temperature should be in evaporation model (source in alpha equation). In our model such dependence is present. So all the answers to your questions is "yes"

so thank you very much for attach this solver...

i have a another question...

is this solver useFull for condensation? or if i use for condensation,i should modify that?

sahas · September 6, 2013, 05:27

Quote:

Originally Posted by Sasy

so thank you very much for attach this solver...

i have a another question...

is this solver useFull for condensation? or if i use for condensation,i should modify that?

yes, you should perform some (minor) modifications because we created solver only for evaporation and source term is considered to be always negative. But as I think it does not matter - evaporation or condensation - for numerical model.

Sasy · September 6, 2013, 06:06

Quote:

Originally Posted by sahas

yes, you should perform some (minor) modifications because we created solver only for evaporation and source term is considered to be always negative. But as I think it does not matter - evaporation or condensation - for numerical model.

Hi Alexander
do you have test case for youre solver?I will be grateful if you can provide me the test case...

sahas · September 6, 2013, 09:38

Quote:

Originally Posted by Sasy

Hi Alexander
do you have test case for youre solver?I will be grateful if you can provide me the test case...

Some troubles with test case arose. I hope I find solution and post test case in near future.

Sasy · September 6, 2013, 09:45

Quote:

Originally Posted by sahas

Some troubles with test case arose. I hope I find solution and post test case in near future.

thank you for Reply
It means you dont validate youre solver with any case that show the solver have a good result?

sahas · September 6, 2013, 20:50

Quote:

Originally Posted by Sasy

thank you for Reply
It means you dont validate youre solver with any case that show the solver have a good result?

Something like that =) We validated it earlier but now there are some problems with reproducing the results (because validating were performed by student, not by me directly)

Sasy · September 7, 2013, 16:19

Quote:

Originally Posted by nimasam

i have developed a solver based on interFOAM, to solve energy equation and besides consider mass transfer between two phases, this solver works correctly for one dimensional case (stephan phase change problem)
but for two case studies, temperature at interface behaves strangely
now any suggestion, cooperation or idea will be helpful

P.S
developed files and case studies are available in attachment
+
some descriptions

can be found here:

http://www.4shared.com/document/-eBG...OF_method.html

Hi Nima
Do you modify youre solver for 2D case?can I have modifid solver?or guide me how correct this solver...
Regards,

ageorg · September 11, 2013, 16:24

Dear nimasam

I would also like to have a look at your final code (a few years later than the other users of the forum/evapPhaseChangeFoam) if this is possible i would be really grateful .

Thank you very much in advance

Ageorg
email: anastasios.georgoulas@gmail.com

sara zand · October 15, 2013, 08:24

Quote:

Originally Posted by nimasam

i have developed a solver based on interFOAM, to solve energy equation and besides consider mass transfer between two phases, this solver works correctly for one dimensional case (stephan phase change problem)
but for two case studies, temperature at interface behaves strangely
now any suggestion, cooperation or idea will be helpful

P.S
developed files and case studies are available in attachment
+
some descriptions

can be found here:

http://www.4shared.com/document/-eBG...OF_method.html

hi nima
could you please send me your code and accessories.
this is my mail:
sara65.zand@gmail.com
thank you Mr sam;I so need it;

llidito · October 15, 2013, 13:25

Hi Nima,

I would really appreciate if you could send me your code and accessories as well.

My email is:

llido1_2@hotmail.com

many thanks in advance,
José.

sahas · December 17, 2013, 04:34

Hello!

Above I wrote about a code developed sometimes ago (see my posts #29 and #31). In our test case I find an error: actually we did not include evaporation heat source in energy equation (but I wonder that the results of numerical computations were close to the experimental one). I cannot explain why is this. "Turning on" the source term lead to bad temperature field although the energy equation (with evaporation heat term) is right.

Unfortunately I am not engaged in this problem for now and attach our test case of evaporating drop for persons interested in. It should work but sometimes the problems with convergence may arise.

P.S. I forget to mention: during creation of the code we disable dimensions checking. So find and set to zero:

Code:

dimensionSet 0;

in $WM_PROJECT_DIR/etc/controlDict

sahas · March 27, 2014, 05:21

Hello everyone!

Long long time ago I posted about our experience in drop evaporation problem (see my posts #29 and #31). But as I studied out later an error with source term was in the energy equation.

But now it seems that I found solution for the problem

The idea is: instead of using simple L*Y term in energy equation one should use next energy equation

fvScalarMatrix TEqn
(
rhoC*fvm::ddt(T) + rhoC*fvm::div(phi, T) - fvm::laplacian(K , T) + L*Y*rhoC/(rho2*C2+alpha1*(rho1*C1-rho2*C2))
);

So the factor rhoC/(rho2*C2+alpha1*(rho1*C1-rho2*C2)) is appeared. If anyone is interested why is this I will write explanation and derivation of the formula (the idea is quite simple).

I have tested (preliminary) solver for the problem of drop evaporation with "new" energy equation and have obtained quite good results.

Update: unfortunately, this is not solved problem completely. The root of the problem is in overestimated value of source term in energy equation due to "smearing" of phase interface.

Miki12 · April 4, 2014, 06:05

Hello Alexander,

I'm very interested by your model, I am trying to simulate the condensation process which is quite close to evaporation. I'm so interested to know the reason of the addition of your ratio. I suppose that it is a correction of the latent heat term? I would really appreciate if you could send to me some documentation.

Thank you very much,

Miki

sahas · April 4, 2014, 08:19

Hello, Miki!

The modification of the source term L*Y in energy equation is obtained by the following simple model.

Let us consider close volume in which the interphase front is (this will be a cell of computational grid). During evaporation (or condensation) the following equality should have place on the interphase front:
$q_l - q_g = \dot m L$ ,
there

- heat flux in liquid and gas, $\dot m$ - mass flux of the evaporated steam,

- latent heat. So, generated heat (due to evaporation) should warm both liquid and gas.
Let $\Omega$ be a volume of the cell, $\alpha$ - volume concentration of the liquid in the cell. So during some period $\Delta t$ the liquid and gas in the cell will be warmed as follows:

$\rho_l \alpha \Omega C_{pl} \Delta T_l = - \beta \dot m L S \Delta t$ ,
$\rho_g (1-\alpha) \Omega C_{pg} \Delta T_g = - (1-\beta) \dot m L S \Delta t$

Here $\Delta T_l, \Delta T_g$ - temperature increase in liquid and gas (in the cell),

- heat capacity,

- density,

- square of evaporation. Quantity $\beta$ is unknown. For its determination let us suppose that $\Delta T_l = \Delta T_g$ . So:

$\beta = \frac{\alpha \rho_l C_{pl}}{\rho_g C_{pg}+\alpha (\rho_l C_{pl}-\rho_g C_{pg})}$

Hence

$\rho C_p \frac{\Delta T}{\Delta t} = - \frac{\rho C_p \dot m L}{\rho_g C_{pg}+\alpha (\rho_l C_{pl}-\rho_g C_{pg})} \frac{S}{\Omega}$ ,

where $\rho C_p = \alpha \rho_l C_{pl} + (1-\alpha) \rho_g C_{pg}$ .

Another possible model, for example, if we suppose that all heat released will warm only liquid (so $\beta=1$ ). In this case simple term L*Y is appeared.

As I understand, in VOF such evaporation model should be applied only in one cell of liquid-gas interface. Presently I do not know exactly how to do it.

cypherpunk01 · April 7, 2014, 16:43

Alexander,

First of all thank you very much for posting your code and continuing to develop this thread. I am also interested in this work and am attempting to port your code to 2.3.0.

A suggestion to reduce the interface smearing that you are experiencing would be to increase the cAlpha term in the fvSolution PIMPLE subdictionary (I notice you currently use a value of 1).

Since OpenFOAM uses the Weller scheme for interface compression, cAlpha determines the magnitude of the artificial velocity.

Rusche's thesis section 4.2.1 discusses it and gives some references.

-Joe

sahas · April 8, 2014, 04:17

Joseph, thank you very much for the reference and suggestion! Increasing of the cAlpha may improve the situation but I think that if interface smears greater than one cell the problem will not be solved completely. So, the decision may be in considering so-called level function (which is distance from phase interface to given point). Or I think one needs a reformulation of evaporation energy source term like it is done with surface tension in momentum equation...

Moncef · November 15, 2014, 16:40

Hello,
First, thank you Mr. Alexander for sharing the solver, and giving useful explanations.
I think there is an error in species mass fraction equation in the alphaEqn.H ( evapEnterFoam solver) , there is no pressure field!
so I think that :

volScalarField YSAT( 18.0*YSAT2/(18.0*YSAT2+29.0*(1.0-YSAT2)) );

should be :

volScalarField YSAT( 18.0*YSAT2/(18.0*YSAT2+29.0*(P-YSAT2)) );

As I released this is Yan and Soong expression for species fraction!
I think also, that the saturated vapor pressure derived from Antoine equation should be multiplied by 133.23 instead of 0.00132! so it would be in Pa (Kg/(m*s²)).

Can you, please, explain what you mean by div_n_k2, and what model have you used for the source term in energy equation. is it m'*Latent heat ? Can you please send me some useful documentation or work papers for modeling evaporation with the VOF method?
Thank you so much.

sahas · November 16, 2014, 12:38

Hello, Monssif!

Concerning YSAT: it is the mass fraction of evaporated vapour whereas YSAT2 is the molar fraction that can be calculated as (saturation pressure)/(atmosphere pressure). So the formula is correct.

Antoine equation for water vapour is correct - it is in mm Hg, 0.00132 is 1/(760 mm Hg).

div_n_k2 is not more than absolute value of div_n_k (I do not remember about coefficient 0.5). div_n_k is div(n) or simple curvature in another words.

> what model have you used for the source term in energy equation. is it m'*Latent heat
I wrote about model in details above, please read. As for now the model for heat equation is not correct due to overestimated heat source (for details see my previous posts).

yangzie2014 · January 21, 2015, 02:49

Dear nimasam:
I need to simulate droplet evaporation in OF but I could not find any solver for that. From this forum I found that you have developed your own code. Is it for May I have the final version?thank you very much!
my Email: yangwei@tju.edu.cn
Best Wishes!
Yang
2015-1-21

March 27, 2014, 05:21		#53
sahas Member Alexander Join Date: Mar 2009 Posts: 49 Rep Power: 17	Hello everyone! Long long time ago I posted about our experience in drop evaporation problem (see my posts #29 and #31). But as I studied out later an error with source term was in the energy equation. But now it seems that I found solution for the problem The idea is: instead of using simple LY term in energy equation one should use next energy equation fvScalarMatrix TEqn ( rhoCfvm::ddt(T) + rhoCfvm::div(phi, T) - fvm::laplacian(K , T) + LYrhoC/(rho2C2+alpha1(rho1C1-rho2C2)) ); So the factor rhoC/(rho2C2+alpha1(rho1C1-rho2C2)) is appeared. If anyone is interested why is this I will write explanation and derivation of the formula (the idea is quite simple). I have tested (preliminary) solver for the problem of drop evaporation with "new" energy equation and have obtained quite good results. Update: unfortunately, this is not solved problem completely. The root of the problem is in overestimated value of source term in energy equation due to "smearing" of phase interface. Last edited by sahas; March 27, 2014 at 11:13.*

April 4, 2014, 06:05	New Energy Equation	#54
Miki12 New Member Join Date: Jan 2014 Posts: 13 Rep Power: 12	Hello Alexander, I'm very interested by your model, I am trying to simulate the condensation process which is quite close to evaporation. I'm so interested to know the reason of the addition of your ratio. I suppose that it is a correction of the latent heat term? I would really appreciate if you could send to me some documentation. Thank you very much, Miki

April 7, 2014, 16:43		#56
cypherpunk01 New Member Joseph Levi Dobmeier Join Date: May 2011 Posts: 1 Rep Power: 0	Alexander, First of all thank you very much for posting your code and continuing to develop this thread. I am also interested in this work and am attempting to port your code to 2.3.0. A suggestion to reduce the interface smearing that you are experiencing would be to increase the cAlpha term in the fvSolution PIMPLE subdictionary (I notice you currently use a value of 1). Since OpenFOAM uses the Weller scheme for interface compression, cAlpha determines the magnitude of the artificial velocity. Rusche's thesis section 4.2.1 discusses it and gives some references. -Joe Last edited by cypherpunk01; April 9, 2014 at 16:13.

November 15, 2014, 16:40	Error in the the surface species mass fraction determination	#58
Moncef New Member Monssif Join Date: Mar 2014 Posts: 5 Rep Power: 12	Hello, First, thank you Mr. Alexander for sharing the solver, and giving useful explanations. I think there is an error in species mass fraction equation in the alphaEqn.H ( evapEnterFoam solver) , there is no pressure field! so I think that : volScalarField YSAT( 18.0YSAT2/(18.0YSAT2+29.0(1.0-YSAT2)) ); should be : volScalarField YSAT( 18.0YSAT2/(18.0YSAT2+29.0(P-YSAT2)) ); As I released this is Yan and Soong expression for species fraction! I think also, that the saturated vapor pressure derived from Antoine equation should be multiplied by 133.23 instead of 0.00132! so it would be in Pa (Kg/(ms²)). Can you, please, explain what you mean by div_n_k2, and what model have you used for the source term in energy equation. is it m'Latent heat ? Can you please send me some useful documentation or work papers for modeling evaporation with the VOF method? Thank you so much.

September 11, 2013, 16:24		#49
ageorg Member Anastasios Join Date: Mar 2009 Posts: 34 Rep Power: 17	Dear nimasam I would also like to have a look at your final code (a few years later than the other users of the forum/evapPhaseChangeFoam) if this is possible i would be really grateful . Thank you very much in advance Ageorg email: anastasios.georgoulas@gmail.com

October 15, 2013, 13:25		#51
llidito New Member Jose Join Date: Oct 2012 Posts: 6 Rep Power: 13	Hi Nima, I would really appreciate if you could send me your code and accessories as well. My email is: llido1_2@hotmail.com many thanks in advance, José.

April 4, 2014, 08:19		#55
sahas Member Alexander Join Date: Mar 2009 Posts: 49 Rep Power: 17	Hello, Miki! The modification of the source term LY in energy equation is obtained by the following simple model. Let us consider close volume in which the interphase front is (this will be a cell of computational grid). During evaporation (or condensation) the following equality should have place on the interphase front: $q_l - q_g = \dot m L$ , there - heat flux in liquid and gas, $\dot m$ - mass flux of the evaporated steam, - latent heat. So, generated heat (due to evaporation) should warm both liquid and gas. Let $\Omega$ be a volume of the cell, $\alpha$ - volume concentration of the liquid in the cell. So during some period $\Delta t$ the liquid and gas in the cell will be warmed as follows: $\rho_l \alpha \Omega C_{pl} \Delta T_l = - \beta \dot m L S \Delta t$ , $\rho_g (1-\alpha) \Omega C_{pg} \Delta T_g = - (1-\beta) \dot m L S \Delta t$ Here $\Delta T_l, \Delta T_g$ - temperature increase in liquid and gas (in the cell), - heat capacity, - density, - square of evaporation. Quantity $\beta$ is unknown. For its determination let us suppose that $\Delta T_l = \Delta T_g$ . So: $\beta = \frac{\alpha \rho_l C_{pl}}{\rho_g C_{pg}+\alpha (\rho_l C_{pl}-\rho_g C_{pg})}$ Hence $\rho C_p \frac{\Delta T}{\Delta t} = - \frac{\rho C_p \dot m L}{\rho_g C_{pg}+\alpha (\rho_l C_{pl}-\rho_g C_{pg})} \frac{S}{\Omega}$ , where $\rho C_p = \alpha \rho_l C_{pl} + (1-\alpha) \rho_g C_{pg}$ . Another possible model, for example, if we suppose that all heat released will warm only liquid (so $\beta=1$ ). In this case simple term LY is appeared. As I understand, in VOF such evaporation model should be applied only in one cell of liquid-gas interface. Presently I do not know exactly how to do it.

April 8, 2014, 04:17		#57
sahas Member Alexander Join Date: Mar 2009 Posts: 49 Rep Power: 17	Joseph, thank you very much for the reference and suggestion! Increasing of the cAlpha may improve the situation but I think that if interface smears greater than one cell the problem will not be solved completely. So, the decision may be in considering so-called level function (which is distance from phase interface to given point). Or I think one needs a reformulation of evaporation energy source term like it is done with surface tension in momentum equation...

November 16, 2014, 12:38		#59
sahas Member Alexander Join Date: Mar 2009 Posts: 49 Rep Power: 17	Hello, Monssif! Concerning YSAT: it is the mass fraction of evaporated vapour whereas YSAT2 is the molar fraction that can be calculated as (saturation pressure)/(atmosphere pressure). So the formula is correct. Antoine equation for water vapour is correct - it is in mm Hg, 0.00132 is 1/(760 mm Hg). div_n_k2 is not more than absolute value of div_n_k (I do not remember about coefficient 0.5). div_n_k is div(n) or simple curvature in another words. > what model have you used for the source term in energy equation. is it m'*Latent heat I wrote about model in details above, please read. As for now the model for heat equation is not correct due to overestimated heat source (for details see my previous posts).

January 21, 2015, 02:49		#60
yangzie2014 New Member WeiYang Join Date: Jan 2014 Location: China Posts: 3 Rep Power: 12	Dear nimasam: I need to simulate droplet evaporation in OF but I could not find any solver for that. From this forum I found that you have developed your own code. Is it for May I have the final version?thank you very much! my Email: yangwei@tju.edu.cn Best Wishes! Yang 2015-1-21