[cyw]

Dear all,

does anybody simulate a single bubble rising in quiescent liquid[1] with interFoam? I simulate several cases but I cannot repeat all the regions with interFoam. I mean the bubble shapes and paths can not match the published results in [1]. Or did I do something wrong?Attachment 62371 I have attached the case file, please help me!


[1] Sharaf, D. M., et al. "Shapes and paths of an air bubble rising in quiescent liquids." Physics of Fluids 29.12 (2017): 122104.

[cyw]

Originally Posted by cyw

Dear all,

does anybody simulate a single bubble rising in quiescent liquid[1] with interFoam? I simulate several cases but I cannot repeat all the regions with interFoam. I mean the bubble shapes and paths can not match the published results in [1]. Or did I do something wrong?Attachment 62371 I have attached the case file, please help me!


[1] Sharaf, D. M., et al. "Shapes and paths of an air bubble rising in quiescent liquids." Physics of Fluids 29.12 (2017): 122104.

The author of the paper uses gerris.

[einstein_zee]

Originally Posted by cyw

The author of the paper uses gerris.

Hey there,

other than that there are many things which are different from your case. I looked at your case, first and foremost they have done a DNS simulation but you are using k-epsilon for turbulence modeling. moreover, they are solving their own derived equations which is different from the approach in OF. Also there might be differences in the discretization schemes and many more issues which all and all are leading to failure in your case.

[cyw]

Originally Posted by einstein_zee

Hey there,

other than that there are many things which are different from your case. I looked at your case, first and foremost they have done a DNS simulation but you are using k-epsilon for turbulence modeling. moreover, they are solving their own derived equations which is different from the approach in OF. Also there might be differences in the discretization schemes and many more issues which all and all are leading to failure in your case.

Thank you for your answer. The author of the papaer uses another openfoam source software gerris to simulate the case.

[piu58]

Dear Foamers,

may be you know the very extended work of Hysing et alii which compares different approaches for calculation fo bubble dynmics. The case there is a 2D rising bubble of diameter 0.5 in a cuvette of width 1 and height 2, slip b.c. at the walls. Two different setups were used, one rather describing an oil bubble in water and another, numerical more challenging which is close to an air bubble in water.
In the paper three software packages were used, all FEM codes. In a picture, some examples were shown for CFX, Comsol and Fluent, but no real numeral results for these codes. OpenFoam was not used.

The authors found two measures which describe the solution all in all: The center of mass, maximum rise velocity and the "circularity" which describes deformations mathematical.

I simulated the second, more complicated case with interfoam, turbulence off (laminar). I used the finest grid mentioned in the publication, around 50 thousand elements. Only with a maxCo as low as 0.01 I got results which very close to the ones in the reference solutions. The shape of the deformed bubble was most similar to the results of FReeLife, a free surface library for a FEM code. I give both results as appendix: Left is the paraFoam output, right is the repainted version of Fig. 19/Hysing.

The center of mass for my solution at the end of the simulation (t=3s) was 1.14. The others got 1.138 - 1.125 - 1.138.

[cyw]

Originally Posted by einstein_zee

Hey there,

other than that there are many things which are different from your case. I looked at your case, first and foremost they have done a DNS simulation but you are using k-epsilon for turbulence modeling. moreover, they are solving their own derived equations which is different from the approach in OF. Also there might be differences in the discretization schemes and many more issues which all and all are leading to failure in your case.

Originally Posted by piu58

Dear Foamers,

may be you know the very extended work of Hysing et alii which compares different approaches for calculation fo bubble dynmics. The case there is a 2D rising bubble of diameter 0.5 in a cuvette of width 1 and height 2, slip b.c. at the walls. Two different setups were used, one rather describing an oil bubble in water and another, numerical more challenging which is close to an air bubble in water.
In the paper three software packages were used, all FEM codes. In a picture, some examples were shown for CFX, Comsol and Fluent, but no real numeral results for these codes. OpenFoam was not used.

The authors found two measures which describe the solution all in all: The center of mass, maximum rise velocity and the "circularity" which describes deformations mathematical.

I simulated the second, more complicated case with interfoam, turbulence off (laminar). I used the finest grid mentioned in the publication, around 50 thousand elements. Only with a maxCo as low as 0.01 I got results which very close to the ones in the reference solutions. The shape of the deformed bubble was most similar to the results of FReeLife, a free surface library for a FEM code. I give both results as appendix: Left is the paraFoam output, right is the repainted version of Fig. 19/Hysing.

The center of mass for my solution at the end of the simulation (t=3s) was 1.14. The others got 1.138 - 1.125 - 1.138.

Thank you for your kind reply. I have validated the case you mentioned in the paper of Hysing et alii. The result is good. But I want to make a step further. So I simulated the 3D cases with interFoam. Gerris uses the Geometric VOF method with height function, which is more accurate while interFoam uses algebraic VoF method. I wonder if there is something wrong with my setting or with the accuracy of the solver. I hope it is my wrong setting that makes the result unaccurate. If so, please help me to correct it.

[sadra2003]

Originally Posted by piu58

Dear Foamers,

may be you know the very extended work of Hysing et alii which compares different approaches for calculation fo bubble dynmics. The case there is a 2D rising bubble of diameter 0.5 in a cuvette of width 1 and height 2, slip b.c. at the walls. Two different setups were used, one rather describing an oil bubble in water and another, numerical more challenging which is close to an air bubble in water.
In the paper three software packages were used, all FEM codes. In a picture, some examples were shown for CFX, Comsol and Fluent, but no real numeral results for these codes. OpenFoam was not used.

The authors found two measures which describe the solution all in all: The center of mass, maximum rise velocity and the "circularity" which describes deformations mathematical.

I simulated the second, more complicated case with interfoam, turbulence off (laminar). I used the finest grid mentioned in the publication, around 50 thousand elements. Only with a maxCo as low as 0.01 I got results which very close to the ones in the reference solutions. The shape of the deformed bubble was most similar to the results of FReeLife, a free surface library for a FEM code. I give both results as appendix: Left is the paraFoam output, right is the repainted version of Fig. 19/Hysing.

The center of mass for my solution at the end of the simulation (t=3s) was 1.14. The others got 1.138 - 1.125 - 1.138.

Hello Uwe Pilz,

Thank you for the info you provided here.
I would be appreciative if you let me know your opinion. (I have attached my case)
I am also working on the terminal velocity of bubbles. Using the paraView, I measure the center of a bubble location in two successive time step, then by deviding the displacement of the center of bubble to the time difference, I wannt to calculate the velocity. The problem is, the value that I gain is 50 % lower than the reported values in the literature. I am using a 2D mesh in openFoam 8 using interFoam.
The contents of my 0 folder are:

U file:

dimensions [0 1 -1 0 0 0 0];

internalField uniform (0 0 0);

boundaryField
{
bottom
{
type noSlip;
}
outlet
{
type noSlip;
}
walls
{
type slip;
}
defaultFaces
{
type empty;
}
}


p_rgh file:
dimensions [1 -1 -2 0 0 0 0];

internalField uniform 0;

boundaryField
{
bottom
{
type zeroGradient;
}

outlet
{
type zeroGradient;
}

walls
{
type zeroGradient;
}

defaultFaces
{
type empty;
}
}

alpha file:


dimensions [0 0 0 0 0 0 0];

internalField uniform 0;

boundaryField
{
bottom
{
type zeroGradient;
}

outlet
{
type zeroGradient;
}

walls
{
type zeroGradient;
}

defaultFaces
{
type empty;
}
}


transportProperties file:

phases (air water);

air
{
transportModel Newtonian;
nu nu [ 0 2 -1 0 0 0 0 ] 1.5E-5;
rho rho [ 1 -3 0 0 0 0 0 ] 1.18;

}

water
{
transportModel Newtonian;
nu nu [ 0 2 -1 0 0 0 0 ] 7.22E-7;
rho rho [ 1 -3 0 0 0 0 0 ] 995.7;

}

Thanks a lot.

[piu58]

I have added my case. I hope you have success with it.

If you have any questions please write me a note.

[sadra2003]

Originally Posted by piu58

I have added my case. I hope you have success with it.

If you have any questions please write me a note.

Thank you Uwe Pilz.
Could you get accurate results for different bubble size with this case?
The results that I get is really fluctuating for a 4mm bubble movement in water at realistic conditions (g=9.8). I would like to know whether you also get the same results or the bubble terminal velocity in your case approaches a distinct value?
atached, please see my result. The average of my result is correct for the terminal velocity of a 4mm bubble but the instantaneious velocity fluctuates alot.

[piu58]

From my notes (2017):
The most important change I made was reducing maxCo. A a mesure I used the coordinate of the center of gravity y_c. From Hysing it hast to be 1.14 for t=3.

maxCo y_c    time for calculation/h
1     0.86
0.5   0.88   0.24
0.1   1.03   0.8
0.03  1.10   2.7 
0.01  1.12   7.3 
0.003 1.123 22.3
0.001 1.124 62

Eventual, I stayed with maxCo=0.01. The simulation run for more than 7 hours with my computer of 2017.

I changed schemes too, but that gave not an important effect.

[fengyi]

Originally Posted by sadra2003

Thank you Uwe Pilz.
Could you get accurate results for different bubble size with this case?
The results that I get is really fluctuating for a 4mm bubble movement in water at realistic conditions (g=9.8). I would like to know whether you also get the same results or the bubble terminal velocity in your case approaches a distinct value?
atached, please see my result. The average of my result is correct for the terminal velocity of a 4mm bubble but the instantaneious velocity fluctuates alot.

Hi Sadra:
1.it is not surprised that bubbles' rising velocity simulated by 2D is smaller than that by 3D or by experiment. You can read this paper which compare rising velocity of 2D and 3D simulation using another free CFD software basilisk(Tripathi M K, Sahu K C. Motion of an air bubble under the action of thermocapillary and buoyancy forces[J]. Computers & Fluids, 2018, 177: 58-68.).I think 2D simulation means infomation is lost in one dimension compared with 3D simulation, so the result is incorrect more or less. My suggestion is that using full 3D simulation for bubble rising problem and for some bubble experencing recttilinear path you may use the 2.5D simulation(axisymmetry wedge grid).
2.the result concerning 4mm bubble's instantaneous velocity in water may be right. I think you must know that if bubbles are so big, they will experience an instability path, which may result in instablity. Of course, your result show a stong amplitude, but I read a paper presenting the similar velocity amplitude for big bubble in water(Antepara O, Balcázar N, Rigola J, et al. Numerical study of rising bubbles with path instability using conservative level-set and adaptive mesh refinement[J]. Computers & Fluids, 2019, 187: 83-97.)
Hope it is useful for you.


Best regards,

Feng

[sadra2003]

Hi Feng,

I really appreciate your help and your response.
Its true that in a 2D simulation, the results is not like a 3D simulation. I actually expected some differenceas between the results. My main problem / question is fluctuation of the terminal velocity of bubbles. Its amplitude is high for all bubbles that I have simulated yet (2D) while the terminal velocity that the other people plotted in this forum does not behave like mine. Almost all of them have a mild amplitude and the velocity does not flictuate a lot. In some cases, they considered g=0.98 to have a milder fluctuation in velocity but I am not sure whether in a realistic case (g=10), the velocity fluctuates a lot or not.

[sadra2003]

Originally Posted by fengyi

Hi Sadra:
1.it is not surprised that bubbles' rising velocity simulated by 2D is smaller than that by 3D or by experiment. You can read this paper which compare rising velocity of 2D and 3D simulation using another free CFD software basilisk(Tripathi M K, Sahu K C. Motion of an air bubble under the action of thermocapillary and buoyancy forces[J]. Computers & Fluids, 2018, 177: 58-68.).I think 2D simulation means infomation is lost in one dimension compared with 3D simulation, so the result is incorrect more or less. My suggestion is that using full 3D simulation for bubble rising problem and for some bubble experencing recttilinear path you may use the 2.5D simulation(axisymmetry wedge grid).
2.the result concerning 4mm bubble's instantaneous velocity in water may be right. I think you must know that if bubbles are so big, they will experience an instability path, which may result in instablity. Of course, your result show a stong amplitude, but I read a paper presenting the similar velocity amplitude for big bubble in water(Antepara O, Balcázar N, Rigola J, et al. Numerical study of rising bubbles with path instability using conservative level-set and adaptive mesh refinement[J]. Computers & Fluids, 2019, 187: 83-97.)
Hope it is useful for you.


Best regards,

Feng

Hi Feng,

I really appreciate your help and your response.
Its true that in a 2D simulation, the results is not like a 3D simulation. I actually expected some differenceas between the results. My main problem / question is fluctuation of the terminal velocity of bubbles. Its amplitude is high for all bubbles that I have simulated yet (2D) while the terminal velocity that the other people plotted in this forum does not behave like mine. Almost all of them have a mild amplitude and the velocity does not flictuate a lot. In some cases, they considered g=0.98 to have a milder fluctuation in velocity but I am not sure whether in a realistic case (g=10), the velocity fluctuates a lot or not.
Attached, you can see the velocity and the trajectory of a 10 mm bubble (diameter) in water. Do you think that this fluctuiation is normal?

Thanks again.

[sadra2003]

Originally Posted by piu58

From my notes (2017):
The most important change I made was reducing maxCo. A a mesure I used the coordinate of the center of gravity y_c. From Hysing it hast to be 1.14 for t=3.

maxCo y_c    time for calculation/h
1     0.86
0.5   0.88   0.24
0.1   1.03   0.8
0.03  1.10   2.7 
0.01  1.12   7.3 
0.003 1.123 22.3
0.001 1.124 62

Eventual, I stayed with maxCo=0.01. The simulation run for more than 7 hours with my computer of 2017.

I changed schemes too, but that gave not an important effect.

Hi Uwe,

Thank you so much for your help. I reduced the CO number and my results get better but still they fluctuate. Is this fluctuation normal for g=10 and diameter of 10mm?

[fengyi]

Originally Posted by sadra2003

Hi Feng,

I really appreciate your help and your response.
Its true that in a 2D simulation, the results is not like a 3D simulation. I actually expected some differenceas between the results. My main problem / question is fluctuation of the terminal velocity of bubbles. Its amplitude is high for all bubbles that I have simulated yet (2D) while the terminal velocity that the other people plotted in this forum does not behave like mine. Almost all of them have a mild amplitude and the velocity does not flictuate a lot. In some cases, they considered g=0.98 to have a milder fluctuation in velocity but I am not sure whether in a realistic case (g=10), the velocity fluctuates a lot or not.
Attached, you can see the velocity and the trajectory of a 10 mm bubble (diameter) in water. Do you think that this fluctuiation is normal?

Thanks again.

Hi Sadra:
1. In fact, I am a beginner for OpenFOAM, too. I don't know why you use g=0.98m/s2 instead of g=9.81m/s2 in reality. According to my 3D simulation experience about bubbles rising in pure water in really gravity g=9.81m/s2, bubbles whose diameter are larger than 2mm may experience a oscillating path and result in a oscillating velocity.

2. I recommend you validate your simulation procedure by using some robust simulation or experiment results first. Of course, you'd better begin with the simplest one--rectilinear path. Just chose some situation as your initial condition(eg. 1mm bubble in pure water) and compare your results with the reference.

BTW, following is a starting case associated with a paper focusing on bubble rising problem using OpenFOAM-v2012 which may help you:https://wiki.openfoam.com/Bubble_ris...nning_the_case

Best regards,

Feng

[sadra2003]

Originally Posted by fengyi

Hi Sadra:
1. In fact, I am a beginner for OpenFOAM, too. I don't know why you use g=0.98m/s2 instead of g=9.81m/s2 in reality. According to my 3D simulation experience about bubbles rising in pure water in really gravity g=9.81m/s2, bubbles whose diameter are larger than 2mm may experience a oscillating path and result in a oscillating velocity.

2. I recommend you validate your simulation procedure by using some robust simulation or experiment results first. Of course, you'd better begin with the simplest one--rectilinear path. Just chose some situation as your initial condition(eg. 1mm bubble in pure water) and compare your results with the reference.

BTW, following is a starting case associated with a paper focusing on bubble rising problem using OpenFOAM-v2012 which may help you:https://wiki.openfoam.com/Bubble_ris...nning_the_case

Best regards,

Feng

Hi Feng,

Thanks.
I did not use g=0.98. I used g=9.81 to be realistic. I have seen some literature that the other researchers used g=0.98.
I checked my results with the experiment and the final results are good. The problem is, in the experimental works, just one value is reported as the velocity in many of the papers and the velocity fluctuation over time is not reporrted by the researchers. So, if I make an average over my data for terminl velocity, it is almost correct, compared to the reported value by experimentalists. I would like to know the bubble velocity behavior vs time flow.

Best,
SM

[fengyi]

Originally Posted by sadra2003

Hi Feng,

Thanks.
I did not use g=0.98. I used g=9.81 to be realistic. I have seen some literature that the other researchers used g=0.98.
I checked my results with the experiment and the final results are good. The problem is, in the experimental works, just one value is reported as the velocity in many of the papers and the velocity fluctuation over time is not reporrted by the researchers. So, if I make an average over my data for terminl velocity, it is almost correct, compared to the reported value by experimentalists. I would like to know the bubble velocity behavior vs time flow.

Best,
SM

Hi Sadra:
Sorry for my misunderstanding. Yes, experimentalist usually report their average terminal velocity only. I'm sorry that I can not provide you more suggetion.

Best regards,

Feng

[sadra2003]

Originally Posted by fengyi

Hi Sadra:
Sorry for my misunderstanding. Yes, experimentalist usually report their average terminal velocity only. I'm sorry that I can not provide you more suggetion.

Best regards,

Feng

Hi Feng,

Thankd for your guidance. I would be apprecitive if you update me if you obtain new insight on this topic.

Warm regards,
SM