CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   STAR-CCM+ (http://www.cfd-online.com/Forums/star-ccm/)
-   -   Two-phase flow in vertical pipe (http://www.cfd-online.com/Forums/star-ccm/88145-two-phase-flow-vertical-pipe.html)

Ladnam May 9, 2011 14:38

Two-phase flow in vertical pipe
 
Have anyone been able to model two-phase flow (water-air) in a vertical pipe and reproduced the observed flow regimes (annular flow, slug flow etc.)? Or maybe have experience with problems related to this?

This is almost the same model as the Hibiki bubble column tutorial except it is upside down.

I have tried steady and unsteady simulation with different BC and IC with VOF and multiphase segregated flow, but the solution either diverges or will not converge to a steady or realistic solution.

abdul099 May 10, 2011 03:06

Are you sure, VOF is the right model?
You should have a mesh resolution small enough to have several cells in one bubble (I assume, there will be some bubbles of air, oil or whatever phase).
Therefore VOF is not suitable to simulate a flow with a very intensive mixture of the different phases.
And not to forget: A steady state VOF simulation is just crap.

When you want to run a case with very intensive mixture or you HAVE to do it steady state, think about a Eulerian / Eulerian multiphase. But be aware, this will NOT resolve single bubbles. And good luck when you try to prevent it from divergence...

Ladnam May 10, 2011 05:26

1 Attachment(s)
I actually got a steady VOF simulation to converge.
But it is not free falling water. I use a velocity inlet at one end with 30% water and a pressure outlet at the other end.

It converges to an annular flow which is realistic.

niriosrat August 25, 2011 04:40

Hi,

Did you model slug flow? it is because I am trying to model slug flow, but is not working, so I wonder which conditions did you used on the VOF?

Ladnam August 29, 2011 08:07

1 Attachment(s)
Yes I think I got some resonable results.
I got slug flow for Froude numbers larger than about 1.5.
I dind't do anything special with the VOF model.
I used a vertical pipe with air intake (pressure outlet) and velocity inlet and a pressure outlet at the bottom end.

niriosrat August 30, 2011 02:52

1 Attachment(s)
My vertical tube has a diameter of 2.53 cm and 4 m length, due to symemtry I am modelling just half of it.

In CCM+ I can not define a single inlet (I think) with air and water coming together with a specific mixture velocity (=0.5 m/s) and a volume fraction of 0.5-0.5. Therefore, I split the inlet in two velocity inlets (for water and air), where each inlet had a velocity of 0.5 m/s. I am using a time-step of 5e-4 sec and the bubbels develop at the inlet (red volume fraction) but after they just disappeared (green volume fraction) and I don't know why?

Ladnam August 30, 2011 07:29

You can use a mixture of two phases but it is not good to use with the VOF model I guess. You can try having two separate inlets for water and air. And maybe the outlet needs to be bigger to avoid backflow. E.g connecting a big box to the outlet. You can also try using the full model (no symmetry) to give the flow more freedom.

ping September 3, 2011 02:11

VOF is for modelling immiscible fluids - no mixing. Each cell in theory should have 100% of one fluid and none of the other(s). Transitions from one fluid to the next should ideally be across just one cell with a 'mixture' of the phases. To achieve this you need a fine mesh is some cases - eg to capture bubbles/drops as mentioned above. Otherwise you must use normal Eulerian multi-phase. In your contour plots as soon as you see zones of colours other than red or blue you are using VOF incorrectly. And so to try to model slug flow in steady mode is crazy - think about what slug flow looks like!

jignesh_thaker2007 January 22, 2012 04:28

hi everyone
 
I am also trying to solve the air-water two phase flow problem in horizontal pipe i also split this pipe in two part and define it to water and air and gave them different velocity. i also used the interDyMFoam solver. but my problem is it possible to get the bubbly flow regime? if possible then how?


Quote:

Originally Posted by ping (Post 322725)
VOF is for modelling immiscible fluids - no mixing. Each cell in theory should have 100% of one fluid and none of the other(s). Transitions from one fluid to the next should ideally be across just one cell with a 'mixture' of the phases. To achieve this you need a fine mesh is some cases - eg to capture bubbles/drops as mentioned above. Otherwise you must use normal Eulerian multi-phase. In your contour plots as soon as you see zones of colours other than red or blue you are using VOF incorrectly. And so to try to model slug flow in steady mode is crazy - think about what slug flow looks like!


niriosrat May 23, 2012 08:26

Hi,

I have an horizontal pipe with ID of 5 cm and a length of 30 m. I defined and inlet (velocity inlet) and outlet (pressure outlet). I am not familiar with field functions and I don't have two-inlets in my geometry. So I wonder if someone knows how to write a field function for the inlet in Star CCM+ where I can set half of the cross-sectional area with air and the other half with water and put a fix velocity for each phase. E.g. the top part with air with a velocity of 0.15 m/s and the bottom with water and a velocity of 2 m/s.

ping May 23, 2012 09:07

the help has lots of detail and examples. and if you do the first vof training tutorial you will see how to do a field function which is very similar to what you require to change from air to water at a certain position. then create an equivalent one for the boundary normal velocity scalar. or a vector field function if you want to express the flow in components.

niriosrat May 30, 2012 09:07

Hi, I defined two field functions for the void fraction of water and air:

water = ($$Centroid[1]<0)?1:0
air = 1-$Water

but I don't know how to define the velocity vector in direction (i). I tried

[($$Centroid[1] < 0) ? 2 : 0.5,0,0]

but doesn't work. Below the center is 2 m/s (water) and above 0.5 m/s (air). However, how I can define the direction i?

abdul099 May 30, 2012 18:52

Velocity is a vector input. So you need to specify three components for each case. Your if-statement defines only one component for the first case ($$Centroid[1]<0 -> 2) and three components for the second case ($$Centroid[1]>=0 -> 0.5,0,0).

niriosrat June 6, 2012 09:06

Thank you for the help with the velocity, I have also another question. I need to monitor: 1) the length of the slug bubbles and 2) the liquid film thinness (between the bottom of the tube and the bubble inter-phase).

For 1) I think I will define just a monitor of phase located in the top to know if is gas or liquid and determine after the distance based on the time step. For 2) I though to define a line on the radial direction as after extract the volume fraction vs height. I wonder if can be a more "automatic" option to determine the height of the liquid thickness?. Or which other options do you recommend. I hope I made myself clear.

niriosrat June 8, 2012 11:22

Hi,

Regardign the velocity, how I can just define the velocity distribution as:

If water volume fraction is 1---> Vel=2 m/s , else---> Vel=0.5 m/s

I mean how I can write that in a field function.

abdul099 June 10, 2012 14:52

Something like
$VolumeFractionWater=1?2:0.5
should work. But you have to make sure, there will be no intermediate value.
Of course, when you're providing only one value, you should switch the input method to composite and put the field function to the right component.

niriosrat June 11, 2012 09:28

1 Attachment(s)
Hi,

It doesn't work when I put the velcoity condition fuction of the volume fraction of water and I don't know why. Have a look to this figure...

There you will see where I define the velocity field function based on your early suggestion of the vector and the void fraction. However, when I look into the velocity (k) nothing appear.

AdarshGouda February 28, 2013 09:00

Why not DPM?
 
Cant we use DPM for such casses. Like Water being the primary phase and we "inject" bubbles into the flow.

I am trying to simulate using DPM with coalscense. Was wondering if I am doing it wrong.

Please Advice.


Adarsh.
Grad Student.

JuanMa22 June 29, 2013 10:49

Multiphase flow
 
hi guys, i have one question. Im simulate two-phase flow in fluent, im trying to do annular flow in a vertical pipe of d=1in and length=10m, but my time step is 1e-05 and de simulations turn tooooo slow, my cuestion is i can obtain annular flow in this geometry? is 2D. :confused: please help me, already obtain bubble, slug and churn. thanks a lot guys. oh and my velocities are Vsl=1m/s and Vsg=40m/s im using VOF model and k-e with enhanced wall treatment

mecman July 23, 2013 10:52

Hi all
i want simulate two phase flow with fluent.my case is a pipe that filled of working fluid,and Tube wall have constant Heat flux,after boiling the fluid in pipe,we have two phase(vapor,liquid)...and i want see the bubble ...
how simulate this case with fluent?
plz help
regard


All times are GMT -4. The time now is 08:19.