CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > FLUENT

Urgent: Slug Flow

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

Reply
 
LinkBack Thread Tools Display Modes
Old   January 15, 2006, 03:18
Default Urgent: Slug Flow
  #1
Paul_C
Guest
 
Posts: n/a
Dear All,

Does anyone have any experience in simulating slug flow using Fluent's VOF model????

Any help will be appreciated.

Thanks in advance
  Reply With Quote

Old   January 24, 2006, 11:46
Default Re: Urgent: Slug Flow
  #2
Sandra
Guest
 
Posts: n/a
Hello Paul,

Can you be more specific? Is it horizontal or vertical slug flow? Which fluids? I have experience in the simulation of horizontal two-phase flows, making use of the VOF model. If you can be more specific, maybe I will be able to help you.

Greetz, Sandra
  Reply With Quote

Old   January 25, 2006, 01:58
Default Re: Urgent: Slug Flow
  #3
Paul_C
Guest
 
Posts: n/a
I am simulating slug flow through a horizontal mini channel, I have adpoted the VOF model with a constant surface tension. I have also assumed the flow to be laminar

For BC: I have specified a constant velocity inlet of 4.2e-3, an outflow and non-slip wall condition.

For IC: I have patch a arbituary sized gas bubbles cylindrical in shape in the channel (volume fraction 1)

The square channel of size 2 x 2 X 50 mm grid size of 26 X 26 X 635

I have tried to reduce the under-relaxation factors but was unable to get satisfactory results. Do you have any suggestions to resolve the problem? Did I miss out any other parameters/conditions required?

Sincerely appreciate your kind assistance. Thanks in advance.

  Reply With Quote

Old   January 26, 2006, 08:58
Default Re: Urgent: Slug Flow
  #4
Sandra
Guest
 
Posts: n/a
Hi Paul,

When I want to perform a two-phase flow calculation, I always start with the converged solution of the flow of one the phases. This increases the stability of the two-phase flow calculation.

Maybe you can try this first. However, if you still have problems, let me know.

Greetz, Sandra
  Reply With Quote

Old   January 27, 2006, 22:24
Default Re: Urgent: Slug Flow
  #5
Paul_C
Guest
 
Posts: n/a
Dear Sandra,

Thanks for the advice. However, i am still having problems with the simulation. I recieve this error message :

"Too many (1859) VOF sub-timesteps. The velocity field is probably diverging. Please check the solution, and reduce the time-step if necessary"

while iteration.

What does this error message means?

  Reply With Quote

Old   January 30, 2006, 03:51
Default Re: Urgent: Slug Flow
  #6
Sandra
Guest
 
Posts: n/a
Hi Paul,

This means that the time step that you have defined for the unsteady simulation is too large. I always use 0.001s, normally this time step should be small enough to avoid divergence. I hope this can solve the problem.

Greetz, Sandra
  Reply With Quote

Old   January 31, 2006, 04:36
Default Re: Urgent: Slug Flow
  #7
Paul_C
Guest
 
Posts: n/a
Dear Sandra,

Can i check with you on what is the initial and boundary conditions that you have used? Also did you include any other factors like surface tension and contact angle for your 2 phase simulation?

Thanks alot for your help

Best Regards

  Reply With Quote

Old   February 3, 2006, 00:29
Default Re: Urgent: Slug Flow
  #8
Paul_C
Guest
 
Posts: n/a
Dear Sandra,

Sorry to bother you again.

I have tried to reduce the time step from 0.001s to 0.00025s but i will still get the same error msg when the iteration hits time 0.002s.

Do you have any advice on this?

Thanks in advance for your help

Best Regards
  Reply With Quote

Old   February 3, 2006, 03:48
Default Re: Urgent: Slug Flow
  #9
Sandra
Guest
 
Posts: n/a
Dear Paul,

I did include a constant surface tension for the simulations. I did not define any contact angle. I always used the geometric reconstruction scheme for the reconstruction of the interface.

Concerning your divergence problem, I don't see a solution right away. For me, reducing the time step was always the solution. Maybe you can increase the number of VOF iterations in each time step and you can also decrease the underrelaxation factors for the calculation of the velocities. I hope this will work.

Greetz, Sandra
  Reply With Quote

Old   February 3, 2006, 04:20
Default Re: Urgent: Slug Flow
  #10
Paul_C
Guest
 
Posts: n/a
Dear Sandra,

Sorry can i check with you how do i change the number of VOF iteration for every time step?

And also how does Fluent takes into account the capiliary forces?

Thanks for your advice. I will try on it.

Best Regards
  Reply With Quote

Old   February 4, 2006, 04:42
Default Re: Urgent: Slug Flow
  #11
kharicha
Guest
 
Posts: n/a
Usually when you model this kind of flow with hihly curved interfaces, you need a very very small time step.... The interface should not move by a distance less than the size of one grid size.

Another problem could be also the curvature of the interfaces versus the grid size. The 1/curvature at any point should be smaller than your grid size. In practice, this means that a drop should be much bigger than your grid size.

To get bigger 1/curvature, increase slowly the surface tension by a factor of 10-1000, and start again your calculation. If your calculation is better....then this was the reason.

By the way what VOF method are you using....

  Reply With Quote

Old   February 4, 2006, 08:46
Default Re: Urgent: Slug Flow
  #12
Paul_C
Guest
 
Posts: n/a
Dear Kharicha,

Thanks for your kind advice.

I will be trying your suggestion.

I am using the geometric reconstruction scheme to reconstruct the interface.

Best Regards.

  Reply With Quote

Old   February 6, 2006, 02:04
Default Re: Urgent: Slug Flow
  #13
kharicha
Guest
 
Posts: n/a
If you have a very long interface(many bubbles), the geometric reconstruction will be to heavy for you.

I suggest to you to use more stable method as implicit....
  Reply With Quote

Old   February 6, 2006, 05:29
Default Re: Urgent: Slug Flow
  #14
Paul_C
Guest
 
Posts: n/a
Dear Kharicha,

I am simulating the flow of a slug bubble through a square channel. So there is only one bubble in the domain.

I have tried increasing the surface tension and it seems that the calculation seems to get worse. so i was wondering if i should reduce the mesh size.

I am currently using a mesh size of 0.05 x 0.05 mm.

Thanks for your kind help

Best Regards

  Reply With Quote

Old   February 6, 2006, 06:02
Default Re: Urgent: Slug Flow
  #15
kharicha
Guest
 
Posts: n/a
You can increase the value of surface tension only if your interface is smooth.... to get a smooth interface, initialize your system, ...i.e patch your bubble domain.

Now you can see that the interface is irregular, following your mesh... Switch to "implicit" version of VOF, do several time iterations with your surface tension value.

You will get a well shaped bubble.

save the results..data

then switch to georecontructor version of VOF. If it is converging, then keep it like that...

if no, then come back to "implicit", and increase slowly the surface tension, then again come back to "georeconstructor"....

If it doesn't work, I will need more details...
  Reply With Quote

Old   February 8, 2006, 05:28
Default Re: Urgent: Slug Flow
  #16
Paul_C
Guest
 
Posts: n/a
Dear Kharicha,

I have tried implicit method but the iteration was unable to converge.

Thanks in advance for your kind help

Best Regards
  Reply With Quote

Old   February 17, 2006, 05:28
Default Re: Urgent: Slug Flow
  #17
Paul_C
Guest
 
Posts: n/a
Dear Kharicha,

i have reduced the time step for the iteration to 1 e-5s and there is no problem of divergence.

However the solution the i am getting is not as expected. That is the shape of the resulting bubble is not as expected.

Is there any advice u can give me?

Thanks alot for your kind advice.

Best Regards

  Reply With Quote

Old   February 17, 2006, 08:13
Default Re: Urgent: Slug Flow
  #18
Kharicha
Guest
 
Posts: n/a
The solution you can get is highly dependant on the curvature definition of the surface of your bubble. So did you reach grid independant results ?

You can also use adaptive mesh refinement technique to increase the number of cells only at the interface....
  Reply With Quote

Reply

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


Similar Threads
Thread Thread Starter Forum Replies Last Post
Flow meter Design CD adapco Group Marketing CD-adapco 3 June 21, 2011 08:33
Help with slug flow simulation. Kes FLUENT 2 May 27, 2008 04:48
Modeling Slug flow Demetrios FLUENT 0 November 23, 2006 17:49
Can 'shock waves' occur in viscous fluid flows? diaw Main CFD Forum 104 February 16, 2006 06:44
Slug flow in square channel PaulC FLUENT 0 December 5, 2005 03:03


All times are GMT -4. The time now is 14:25.