Boundary conditions for Two-phase Flow with Different Inlet Pressures

mizzou · November 9, 2016, 05:46

Quote:

Originally Posted by Fauster

Hi Mizzou,

Here are different results :

The first one is for alpha = 0.3 and u = 0.3 m/s, and the second is for alpha = 0.6 and u = 0.2 m/s. With alpha = 0.3 and u = 0.3 m/s the regime seems to be churn.

As you can see with alpha=0.6 and u = 0.2 m/s the flow tends to be slug regime but I am not satisfied. More settings are needed to get a proper slug flow.

I am wondering the same thing.

Maybe by using conservation of mass :

the total superficial velocity is given by :

$j_{tot} = \rho_l\,(1-\alpha)\,v_l+\rho_g\,\alpha v_g$

So you can know superficial velocities of liquid and gas at inlet at least.

Did you take a look at Taitel and Duckler map ? Maybe it's also possible to evaluate Martinelli-Nelson parameter and others non dimensional parameters to get information about flow structures.

EDIT : I am running this case on 9 cores.

Dear Paul,

Thanks for sharing the information. Good job, I guess you are simulating the vertical 2P flow. But let's talk about horizontal flow since I am simulating horizontal cases now. Actually for the superficial velocities, I was thinking since we already set the value of velocity at the inlet, it means we have same actual velocity for both phases(vg=vl=v). Also we set the alpha to a certain value. So we would have the following equation:
Liquid superficial vel.=U*alpha
Gas Superficial vel.=U*(1-alpha)
Am I wrong?
Regarding your mention about Titel-Dukler map, still to use that flow map we need to somehow find the correct value for corresponding velocities in our simulation. Because if you loot at the vertical axis, there is still velocity behind the parameters!
Also, regarding your current model, are you able to simulate slug or annular flow (for horizontal case)?

Thank you,

Fauster · November 9, 2016, 07:13

Quote:

Originally Posted by mizzou

Dear Paul,

Thanks for sharing the information. Good job, I guess you are simulating the vertical 2P flow. But let's talk about horizontal flow since I am simulating horizontal cases now. Actually for the superficial velocities, I was thinking since we already set the value of velocity at the inlet, it means we have same actual velocity for both phases(vg=vl=v). Also we set the alpha to a certain value. So we would have the following equation:
Liquid superficial vel.=U*alpha
Gas Superficial vel.=U*(1-alpha)
Am I wrong?

No you are right. As I said :
$G = \rho_l\,(1-\alpha)\,v_l+\rho_g\,\alpha$
It means that the mass flux of the mixture is equal to the sum of two terms. One for each phase:
$j_{l} = (1-\alpha)\,v_l$
$j_{g} =$ $\alpha v_g$

Be careful, in OPENFOAM alpha = 1 means "water". Usually in the literature it's the opposite.

Quote:

Regarding your mention about Titel-Dukler map, still to use that flow map we need to somehow find the correct value for corresponding velocities in our simulation. Because if you loot at the vertical axis, there is still velocity behind the parameters!

Yes...
I am really not sure if it's possible to predict the flow regime only using superficial velocity at inlet. Aee explained it very well in a previous post. From my point of view

is constant at any section of the pipe (if we suppose that the flow is "stationary"). But the two components of

change as the flow develops. $j_{g}$ rise when $j_{l}$ decrease in order to maintain

constant.

I guess it's not the good way to take this problem.

PS : sorry for my very bad English...
EDIT : I changed my notation. I replaced $j_{tot}$ by

. It's less confusing

mizzou · November 9, 2016, 22:59

Quote:

Originally Posted by Fauster

I am really not sure if it's possible to predict the flow regime only using superficial velocity at inlet. Aee explained it very well in a previous post. From my point of view [/COLOR][/COLOR]

is constant at any section of the pipe (if we suppose that the flow is "stationary"). But the two components of

change as the flow develops. $j_{g}$ rise when $j_{l}$ decrease in order to maintain

constant.

Paul,

Thats correct. But is that against the reality? I mean even for a real physical sense, this will happen, right? As you know, the well-know flow regime maps for predicting adiabatic two-phase flow (such as Mandhane, Taitel-Dukler,...) are based on superficial velocities of gas and liquid. I think even in those flow maps, the values of superficial velocities represent the inlet ones as it changes by developing the flow. The same thing happens here in the simulation, and it should be possible to use the flow map by superficial velocities of the phases. (Please correct me if I am not true)

If you look at this paper:
http://ccsenet.org/journal/index.php...cle/view/42063
They compared their 2D simulation with Taitel-Dukler map, however, when I tried to calculate the parameters in Table 2, I could not get those values for X, F and T. for example for the case (U=0.1 and alpha=0.1) how they ended up with X=40.7696, F=0.0014 and T=0.0432?

mizzou · November 10, 2016, 01:33

Quote:

Originally Posted by Fauster

Be careful, in OPENFOAM alpha = 1 means "water". Usually in the literature it's the opposite.

Yes. As such, I think you should change your equations then:
Jl=alpha*vl
Jg=(1-alpha)*vg

I've attached 3 screenshot out of my 2D simulations hereby. The geometry of all the cases are 1m * 11mm
The first one is for 11000 mesh (1000*11) whereas U=0.3 , alpha=0.5 using RAS turbulence model. The flow is stratified.

The 2nd one is for 44000 mesh (2000*22) with U=0.59 and alpha=0.6 ( I don't know exactly about this flow regime type, probably similar to slug flow)

The 3rd one is for another inlet condition which I used to use earlier. the inlet is just divided to 7 separate inlet (3 for gas and 4 for water). I used 198000 mesh (3000*66) and the flow is plug regime. However, as Aee said before, this is not physical as there should be always gradient between neighbors. But the result shows something at least.

Yet I cannot capture wavy and annular flow from my model. I even used very fine mesh (up to 790000 cells with various values for alpha and U). I was wondering if you can get from your model or not.

Thank you,
Milad

Fauster · November 10, 2016, 10:21

Quote:

Originally Posted by mizzou

Yes. As such, I think you should change your equations then:
Jl=alpha*vl
Jg=(1-alpha)*vg

I've attached 3 screenshot out of my 2D simulations hereby. The geometry of all the cases are 1m * 11mm
The first one is for 11000 mesh (1000*11) whereas U=0.3 , alpha=0.5 using RAS turbulence model. The flow is stratified.

The 2nd one is for 44000 mesh (2000*22) with U=0.59 and alpha=0.6 ( I don't know exactly about this flow regime type, probably similar to slug flow)

The 3rd one is for another inlet condition which I used to use earlier. the inlet is just divided to 7 separate inlet (3 for gas and 4 for water). I used 198000 mesh (3000*66) and the flow is plug regime. However, as Aee said before, this is not physical as there should be always gradient between neighbors. But the result shows something at least.

Yet I cannot capture wavy and annular flow from my model. I even used very fine mesh (up to 790000 cells with various values for alpha and U). I was wondering if you can get from your model or not.

Thank you,
Milad

HI Mizzou,

Thanks for you reply. I knew the paper of our Russians friends. Very interesting. I got same problem than you. I wasn't able to capture annular flow but I had small wave on another one.

Quote:

The 2nd one is for 44000 mesh (2000*22) with U=0.59 and alpha=0.6 ( I don't know exactly about this flow regime type, probably similar to slug flow)

Yes probably.

In fact I think the problem come from the length of the pipe. If the length is too short the flow regime can't develop (do you agree ?). Did you try to run your simulation on a 10 m pipe ?

Actually I am simulating different flows patterns on a vertical pipe (because it's run faster and I have only 9 cores on my workstation).

Paul

mizzou · November 10, 2016, 13:09

Quote:

Originally Posted by Fauster

In fact I think the problem come from the length of the pipe. If the length is too short the flow regime can't develop (do you agree ?). Did you try to run your simulation on a 10 m pipe ?

Yes maybe. That's a good point. I haven't tried such a long pipe but I will do later.
BTW, have you simulated two phase flow in a 3D pipe instead of 2D? I wonder if the only difference between 2D and 3D simulation should be just creating the geometry or is there any other difference? Actually, I've just recently started to simulate in a 3D pipe, but still I am keep using the similar boundary conditions and system files for my simulation. However, I am not pretty sure if that should work or not.

Thanks,
Milad

Fauster · November 11, 2016, 04:06

Quote:

Originally Posted by mizzou

Yes maybe. That's a good point. I haven't tried such a long pipe but I will do later.
BTW, have you simulated two phase flow in a 3D pipe instead of 2D? I wonder if the only difference between 2D and 3D simulation should be just creating the geometry or is there any other difference? Actually, I've just recently started to simulate in a 3D pipe, but still I am keep using the similar boundary conditions and system files for my simulation. However, I am not pretty sure if that should work or not.

Thanks,
Milad

Yes I tried to simulate thow phase flow in a 3D pipe but it's very cost computing. The only different thing between 3D or 2D is your blockMesh file. If you keep the same patch you can also keep your BC files. I am not very used to blockMesh for 3D case. I prefer to create my mesh with fluent and convert it to openFoam format.

Fauster · November 11, 2016, 05:26

Quote:

Originally Posted by mizzou

Paul,
If you look at this paper:
http://ccsenet.org/journal/index.php...cle/view/42063
They compared their 2D simulation with Taitel-Dukler map, however, when I tried to calculate the parameters in Table 2, I could not get those values for X, F and T. for example for the case (U=0.1 and alpha=0.1) how they ended up with X=40.7696, F=0.0014 and T=0.0432?

HI Mizzou !

Yes it works. You just need to use rigorously Froude Number, Lockhart–Martinelli parameter and Taitel/Dukler parameter (well described on page 2 and 3).

For the case (U=0.1 and alpha=0.1) the regime is laminar. Use 64/Re for the friction factor. When it's turbulent I used Blasius' correlation (0.3164Re^(-0.25)).

Be careful there is a mistake in their paper. They have forgotten the square on the velocity (formula 4, page 3).

Paul

mizzou · November 13, 2016, 13:22

Quote:

Originally Posted by Fauster

HI Mizzou !

Yes it works. You just need to use rigorously Froude Number, Lockhart–Martinelli parameter and Taitel/Dukler parameter (well described on page 2 and 3).

For the case (U=0.1 and alpha=0.1) the regime is laminar. Use 64/Re for the friction factor. When it's turbulent I used Blasius' correlation (0.3164Re^(-0.25)).

Be careful there is a mistake in their paper. They have forgotten the square on the velocity (formula 4, page 3).

Paul

Yes, actually there is also another mistake I just found in the page4. The gas (air) density is supposed to be 1.2 kg/m3 rather than 12 kg/m3. But still I can't get the same values as in the Table2. Could you please check out the attached file? I've just provided my calculations to find F,X and T for the case U=0.1 and alpha=0.1.

Thanks,
Milad

Fauster · November 13, 2016, 14:03

Quote:

Originally Posted by mizzou

Yes, actually there is also another mistake I just found in the page4. The gas (air) density is supposed to be 1.2 kg/m3 rather than 12 kg/m3. But still I can't get the same values as in the Table2. Could you please check out the attached file? I've just provided my calculations to find F,X and T for the case U=0.1 and alpha=0.1.

Thanks,
Milad

Wrong gas density....

...and your Renolds number are also wrong. The Reynolds number for liquid phase is 180 and for gas phase is 54.054.

mizzou · November 13, 2016, 15:27

Quote:

Originally Posted by Fauster

Wrong gas density....

...and your Renolds number are also wrong. The Reynolds number for liquid phase is 180 and for gas phase is 54.054.

Why? Could you elaborate how you came up with 180 and 54 for Reynolds numbers? I checked my calculations many times and I couldn't figure out which parameter is wrong in my calculations?

The gas is air and air density is 1.2 kg/m3.
https://en.wikipedia.org/wiki/Density_of_air
If you are saying this is not correct. What would be true value then?

Thanks,
Milad

Fauster · November 13, 2016, 15:40

Quote:

Originally Posted by mizzou

Why? Could you elaborate how you came up with 180 and 54 for Reynolds numbers? I checked my calculations many times and I couldn't figure out which parameter is wrong in my calculations?

The gas is air and air density is 1.2 kg/m3.
https://en.wikipedia.org/wiki/Density_of_air
If you are saying this is not correct. What would be true value then?

Thanks,
Milad

Look at carrefully the paper. The gas density is...12 kg/m^3

mizzou · November 13, 2016, 17:21

Quote:

Originally Posted by Fauster

Look at carrefully the paper. The gas density is...12 kg/m^3

U=0.1 , alpha=0.1 ---> Jg=U(1-alpha)=0.1(1-0.1)=0.09
Dh=0.08
kinematic viscosity of gas (nug)=1.48*(10^-5)
Reg=Jg*Dh/nug = (0.09)(0.08)/(1.48*10^-5)=486.5 !!!!!!!!!

About the gas density I said in my previous post that if the gas is air, the authors did a mistake on the paper as the correct value of air density is 1.2 kg/m3 not 12. However, even choosing 12 as air density, this value has nothing to do with calculating the Reynolds number as long as we already have the kinematic viscosity.

Thanks,
Milad

Fauster · November 13, 2016, 17:34

Quote:

Originally Posted by mizzou

U=0.1 , alpha=0.1 ---> Jg=U(1-alpha)=0.1(1-0.1)=0.09
Dh=0.08
kinematic viscosity of gas (nug)=1.48*(10^-5)
Reg=Jg*Dh/nug = (0.09)(0.08)/(1.48*10^-5)=486.5 !!!!!!!!!

About the gas density I said in my previous post that if the gas is air, the authors did a mistake on the paper as the correct value of air density is 1.2 kg/m3 not 12. However, even choosing 12 as air density, this value has nothing to do with calculating the Reynolds number as long as we already have the kinematic viscosity.

Thanks,
Milad

In wich cases the density of air could be 12 kg/m^3 ? In other words are you sure that the density of air couldn't be 12 kg/m^3 ?
Are you sure you are using the good definition of alpha when evaluating Reynolds Number ? Remember I wrote something about alpha on litterature...

Paul.

mizzou · November 15, 2016, 18:24

Quote:

Originally Posted by Fauster

In wich cases the density of air could be 12 kg/m^3 ? In other words are you sure that the density of air couldn't be 12 kg/m^3 ?
Are you sure you are using the good definition of alpha when evaluating Reynolds Number ? Remember I wrote something about alpha on litterature...

Paul.

Thanks Paul, it worked for Ug=alpha*U and air density=12 kg/m3.

mizzou · December 7, 2016, 00:27

For this kind of problem which criteria is best to check the grid dependency? which parameter you usually used in two-phase flow to show that the case is mesh independent?

Thanks,
Milad

Udayraj12 · August 8, 2018, 14:09

Hello everyone,

I am simulating gas-liquid two phase flow in a horizontal pipeline of L/D ratio 150. I have divided the inlet in two parts. I am entering water at 0.2m/s and air at 1.2m/s. The volume fraction of water at water_inlet is 1. The solver scheme used is PISO and PRESTO for pressure. The mesh is fine with 1.6 M cells. The flow initially converges and start diverging after some time steps. what could be the reason behind it?

your reply is highly appreciated.

Thank you.

suheng · September 25, 2018, 21:55

Quote:

Originally Posted by Fauster

Hi Mizzou,

I am trying to simulate a similar case. I am pretty sure you forgot the gravity...

EDIT : My apologize, it's ok. Your pipe is just vertical..Anyway with your settings on a horizontal pipe the flow is stratified

When I run the multiphase flow (air water, SST turbulence model) on a horizontal 2D pipe (length 1 m, diameter : 0.02 m) whit the following BC :

Inlet Alpha = 0.5, v = 0.3 m/s
Outlet = 0 bar

The flow pattern is stratified..

My mesh is enough fine I guess (1000x40 meshs).

i meet the same question ,and could you please give me some suggestions about the selection of the solvers about p and U in the system/fvsolution

December 7, 2016, 00:27	Grid dipendency	#36
mizzou Member Milad Join Date: Jul 2015 Location: USA Posts: 45 Rep Power: 11	For this kind of problem which criteria is best to check the grid dependency? which parameter you usually used in two-phase flow to show that the case is mesh independent? Thanks, Milad

August 8, 2018, 14:09	Slug flow in horizontal pipeline	#37
Udayraj12 New Member Udayraj Thorat Join Date: Jul 2018 Posts: 4 Rep Power: 8	Hello everyone, I am simulating gas-liquid two phase flow in a horizontal pipeline of L/D ratio 150. I have divided the inlet in two parts. I am entering water at 0.2m/s and air at 1.2m/s. The volume fraction of water at water_inlet is 1. The solver scheme used is PISO and PRESTO for pressure. The mesh is fine with 1.6 M cells. The flow initially converges and start diverging after some time steps. what could be the reason behind it? your reply is highly appreciated. Thank you.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
sliding mesh problem in CFX	Saima	CFX	46	September 11, 2021 08:38
How to specify an inlet boundary conditions for a fully developed gas flow in a duct.	legendyxg	FLUENT	2	May 11, 2010 08:32
ATTENTION! Reliability problems in CFX 5.7	Joseph	CFX	14	April 20, 2010 16:45
Pulsating flow with non-reflective inlet boundary	cc1000	CFX	6	April 27, 2009 09:10
Boundary conditions for two phase flow	Adel Ataki	FLUENT	2	November 9, 2000 05:24