CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

evapPhaseChangeFOAM

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree7Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   September 6, 2013, 06:03
Default
  #41
Member
 
Alexander
Join Date: Mar 2009
Posts: 37
Rep Power: 7
sahas is on a distinguished road
Quote:
Originally Posted by Sasy View Post
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 likes this.
sahas is offline   Reply With Quote

Old   September 6, 2013, 06:17
Default
  #42
New Member
 
sasan
Join Date: Sep 2013
Posts: 28
Rep Power: 3
Sasy is on a distinguished road
Quote:
Originally Posted by sahas View Post
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?
Sasy is offline   Reply With Quote

Old   September 6, 2013, 06:27
Default
  #43
Member
 
Alexander
Join Date: Mar 2009
Posts: 37
Rep Power: 7
sahas is on a distinguished road
Quote:
Originally Posted by Sasy View Post
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 likes this.
sahas is offline   Reply With Quote

Old   September 6, 2013, 07:06
Default
  #44
New Member
 
sasan
Join Date: Sep 2013
Posts: 28
Rep Power: 3
Sasy is on a distinguished road
Quote:
Originally Posted by sahas View Post
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...
Sasy is offline   Reply With Quote

Old   September 6, 2013, 10:38
Default
  #45
Member
 
Alexander
Join Date: Mar 2009
Posts: 37
Rep Power: 7
sahas is on a distinguished road
Quote:
Originally Posted by Sasy View Post
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 likes this.
sahas is offline   Reply With Quote

Old   September 6, 2013, 10:45
Default
  #46
New Member
 
sasan
Join Date: Sep 2013
Posts: 28
Rep Power: 3
Sasy is on a distinguished road
Quote:
Originally Posted by sahas View Post
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?
Sasy is offline   Reply With Quote

Old   September 6, 2013, 21:50
Default
  #47
Member
 
Alexander
Join Date: Mar 2009
Posts: 37
Rep Power: 7
sahas is on a distinguished road
Quote:
Originally Posted by Sasy View Post
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)
sahas is offline   Reply With Quote

Old   September 7, 2013, 17:19
Default
  #48
New Member
 
sasan
Join Date: Sep 2013
Posts: 28
Rep Power: 3
Sasy is on a distinguished road
Quote:
Originally Posted by nimasam View Post
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,
Sasy is offline   Reply With Quote

Old   September 11, 2013, 17:24
Default
  #49
New Member
 
Anastasios
Join Date: Mar 2009
Posts: 25
Rep Power: 7
ageorg is on a distinguished road
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
ageorg is online now   Reply With Quote

Old   October 15, 2013, 09:24
Default
  #50
New Member
 
sara zand
Join Date: Oct 2013
Posts: 1
Rep Power: 0
sara zand is on a distinguished road
Quote:
Originally Posted by nimasam View Post
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;
sara zand is offline   Reply With Quote

Old   October 15, 2013, 14:25
Default
  #51
New Member
 
Jose
Join Date: Oct 2012
Posts: 6
Rep Power: 4
llidito is on a distinguished road
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,
Josť.
llidito is offline   Reply With Quote

Old   December 17, 2013, 05:34
Default
  #52
Member
 
Alexander
Join Date: Mar 2009
Posts: 37
Rep Power: 7
sahas is on a distinguished road
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
Attached Files
File Type: gz test_drop.tar.gz (7.0 KB, 33 views)
sahas is offline   Reply With Quote

Old   March 27, 2014, 07:21
Default
  #53
Member
 
Alexander
Join Date: Mar 2009
Posts: 37
Rep Power: 7
sahas is on a distinguished road
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.

Last edited by sahas; March 27, 2014 at 13:13.
sahas is offline   Reply With Quote

Old   April 4, 2014, 07:05
Post New Energy Equation
  #54
New Member
 
Join Date: Jan 2014
Posts: 13
Rep Power: 3
Miki12 is on a distinguished road
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
Miki12 is offline   Reply With Quote

Old   April 4, 2014, 09:19
Default
  #55
Member
 
Alexander
Join Date: Mar 2009
Posts: 37
Rep Power: 7
sahas is on a distinguished road
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 q_l, q_g - heat flux in liquid and gas, \dot m - mass flux of the evaporated steam, L - 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), C_p - heat capacity, rho - density, S - 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.
sahas is offline   Reply With Quote

Old   April 7, 2014, 17:43
Default
  #56
New Member
 
Joseph Levi Dobmeier
Join Date: May 2011
Posts: 1
Rep Power: 0
cypherpunk01 is on a distinguished road
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 17:13.
cypherpunk01 is offline   Reply With Quote

Old   April 8, 2014, 05:17
Default
  #57
Member
 
Alexander
Join Date: Mar 2009
Posts: 37
Rep Power: 7
sahas is on a distinguished road
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...
sahas is offline   Reply With Quote

Old   November 15, 2014, 17:40
Default Error in the the surface species mass fraction determination
  #58
New Member
 
Monssif
Join Date: Mar 2014
Posts: 5
Rep Power: 2
Moncef is on a distinguished road
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*s≤)).

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.
Moncef is offline   Reply With Quote

Old   November 16, 2014, 13:38
Default
  #59
Member
 
Alexander
Join Date: Mar 2009
Posts: 37
Rep Power: 7
sahas is on a distinguished road
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).
sahas is offline   Reply With Quote

Old   January 21, 2015, 03:49
Default
  #60
New Member
 
WeiYang
Join Date: Jan 2014
Location: China
Posts: 2
Rep Power: 0
yangzie2014 is on a distinguished road
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
yangzie2014 is offline   Reply With Quote

Reply

Tags
boiling, evaporation, interfoam, phase change

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On



All times are GMT -4. The time now is 09:59.