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

VOF in AVL FIRE

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

Reply
 
LinkBack Thread Tools Display Modes
Old   October 27, 2009, 01:47
Question VOF in AVL FIRE
  #1
New Member
 
Morshed Alam
Join Date: Oct 2009
Posts: 6
Rep Power: 7
morshed_alm is on a distinguished road
I am using commercial CFD software AVL FIRE. I am trying to simulate gas jet impinging on liquid surface and using the volume of fluid (VOF) method for tracking the interface. Whenever I use any turbulence model with VOF method, the simulation does not run. The simulation runs only when I assume Laminer flow. Could anyone please tell me what is the problem of using turbulence model with VOF method?

Thanks in Advance.

Morshed
morshed_alm is offline   Reply With Quote

Old   October 27, 2009, 13:45
Default VOF with FIRE
  #2
Senior Member
 
CFDtoy
Join Date: Mar 2009
Location: United States
Posts: 145
Blog Entries: 2
Rep Power: 8
CFDtoy is on a distinguished road
Hello Morshed,
First of all which version of FIRE are you using? v8.5 or newer version or older? VOF in FIRE is very robust and uses the advanced interface tracking procedure and works very well with laminar and turb effects. My guess is - you may have a problem in the set up with VOF - with/without surface tension.

Make sure you are satisfying Courant criteria - since the interface tracking procedure used normally works extremely well under Co <= 0.2 (several tests available in this regard).

Thanks,

CFDtoy

Quote:
Originally Posted by morshed_alm View Post
I am using commercial CFD software AVL FIRE. I am trying to simulate gas jet impinging on liquid surface and using the volume of fluid (VOF) method for tracking the interface. Whenever I use any turbulence model with VOF method, the simulation does not run. The simulation runs only when I assume Laminer flow. Could anyone please tell me what is the problem of using turbulence model with VOF method?

Thanks in Advance.

Morshed
CFDtoy is offline   Reply With Quote

Old   October 28, 2009, 09:06
Default
  #3
New Member
 
Morshed Alam
Join Date: Oct 2009
Posts: 6
Rep Power: 7
morshed_alm is on a distinguished road
Hi CFDTOY,

Thanks for the reply. I am using Fire 2008.2. I am injecting air on water surface. I have used 0.072 surface tension and 90 degree contact angle in the CSF model of VOF. My courent no is also less then 0.5 but still the simulation is not running with the turbulence model. It stops just before first iteration. The simulaton only runs for the Laminer flow. I don't know what is the problem. Could you please give me any example problem where VOF is used with turbulence model. Any such help would be greately appreciated.
morshed_alm is offline   Reply With Quote

Old   October 28, 2009, 11:03
Default fire vof
  #4
Senior Member
 
CFDtoy
Join Date: Mar 2009
Location: United States
Posts: 145
Blog Entries: 2
Rep Power: 8
CFDtoy is on a distinguished road
Hi morshed,
I have seen error messages from FIRE. Could you post the error messages if any. Well, quick questions
(1) does the simulation start?
(2) If it does -> how many TS do you proceed?
(3) Does it indicate the simulation diverged? if so after how many iterations or TS
- Did you try lowering your time step
- Did you try using upwind schems of momentum and continuity and other variables
-Did you try different initialization of the turbulent flow field (k and epsilon)
-Did you try different turb models (i am assuming u started with k-e - try k-z-f or others)

Let me know the outcome. If you have snapshot of diverged file..post it here.

Thanks,

CFDtoy

Quote:
Originally Posted by morshed_alm View Post
Hi CFDTOY,

Thanks for the reply. I am using Fire 2008.2. I am injecting air on water surface. I have used 0.072 surface tension and 90 degree contact angle in the CSF model of VOF. My courent no is also less then 0.5 but still the simulation is not running with the turbulence model. It stops just before first iteration. The simulaton only runs for the Laminer flow. I don't know what is the problem. Could you please give me any example problem where VOF is used with turbulence model. Any such help would be greately appreciated.
CFDtoy is offline   Reply With Quote

Old   October 29, 2009, 08:57
Default
  #5
New Member
 
Morshed Alam
Join Date: Oct 2009
Posts: 6
Rep Power: 7
morshed_alm is on a distinguished road
Dear CFDtoy,

My simulation does not start at all. It stops just before the first time steps. Then it says simulation finished. I have lowerd my time steps up to 10^-6 second. But nothing happened. I have used upwind scheme for momentum and Central differencing scheme for pressure equation (continuity).I tried k-epsilon and k-zeta-f model. But I haven't changed the initial condition of the turbulence flow field.

Thanks for your help.

Cheers,
Morshed










Quote:
Originally Posted by CFDtoy View Post
Hi morshed,
I have seen error messages from FIRE. Could you post the error messages if any. Well, quick questions
(1) does the simulation start?
(2) If it does -> how many TS do you proceed?
(3) Does it indicate the simulation diverged? if so after how many iterations or TS
- Did you try lowering your time step
- Did you try using upwind schems of momentum and continuity and other variables
-Did you try different initialization of the turbulent flow field (k and epsilon)
-Did you try different turb models (i am assuming u started with k-e - try k-z-f or others)

Let me know the outcome. If you have snapshot of diverged file..post it here.

Thanks,

CFDtoy
morshed_alm is offline   Reply With Quote

Old   October 29, 2009, 09:46
Default fire vof
  #6
Senior Member
 
CFDtoy
Join Date: Mar 2009
Location: United States
Posts: 145
Blog Entries: 2
Rep Power: 8
CFDtoy is on a distinguished road
Hi Morshed,
Ok. So, does it even go past the print of first TS? I mean lets say - it starts by (i hope they still preserve the same format for res values etc)

1. Time step = .... dt = ...
iter resu,v,w field values

below this do you get any numbers at all ? or the code stops before this print statement?

Also, if there was a diverging statement - could you pass it on ..for example, a diverged statement would say something like

%fire-I-..... etc...does it say anything?


Thanks,

CFDtoy


Quote:
Originally Posted by morshed_alm View Post
Dear CFDtoy,

My simulation does not start at all. It stops just before the first time steps. Then it says simulation finished. I have lowerd my time steps up to 10^-6 second. But nothing happened. I have used upwind scheme for momentum and Central differencing scheme for pressure equation (continuity).I tried k-epsilon and k-zeta-f model. But I haven't changed the initial condition of the turbulence flow field.

Thanks for your help.

Cheers,
Morshed
CFDtoy is offline   Reply With Quote

Old   October 29, 2009, 12:14
Default VOF FIRE - turb model works !!
  #7
Senior Member
 
CFDtoy
Join Date: Mar 2009
Location: United States
Posts: 145
Blog Entries: 2
Rep Power: 8
CFDtoy is on a distinguished road
Hi there,
I got it. Go to turbulent interfacial exchange and set up an exchange interface - Activate homogenous and use a general model flag !!! If you activate turb model this is required.


Hope it worked for you as well.


Regards,

CFDtoy



Quote:
Originally Posted by CFDtoy View Post
Hi Morshed,
Ok. So, does it even go past the print of first TS? I mean lets say - it starts by (i hope they still preserve the same format for res values etc)

1. Time step = .... dt = ...
iter resu,v,w field values

below this do you get any numbers at all ? or the code stops before this print statement?

Also, if there was a diverging statement - could you pass it on ..for example, a diverged statement would say something like

%fire-I-..... etc...does it say anything?


Thanks,

CFDtoy
CFDtoy is offline   Reply With Quote

Old   October 30, 2009, 06:02
Smile
  #8
New Member
 
Morshed Alam
Join Date: Oct 2009
Posts: 6
Rep Power: 7
morshed_alm is on a distinguished road
Dear CFDtoy,

Thank you very very much. It is working now. I will never forget your help. I hope we will remain friend from now on.

Thanks again.

Morshed
morshed_alm is offline   Reply With Quote

Old   October 30, 2009, 09:32
Default Fire
  #9
Senior Member
 
CFDtoy
Join Date: Mar 2009
Location: United States
Posts: 145
Blog Entries: 2
Rep Power: 8
CFDtoy is on a distinguished road
Glad I could help. btw, are you planning to publish your work? Let me know how your simulation goes.

/CFDtoy

Quote:
Originally Posted by morshed_alm View Post
Dear CFDtoy,

Thank you very very much. It is working now. I will never forget your help. I hope we will remain friend from now on.

Thanks again.

Morshed
CFDtoy is offline   Reply With Quote

Old   November 1, 2009, 18:58
Smile
  #10
New Member
 
Morshed Alam
Join Date: Oct 2009
Posts: 6
Rep Power: 7
morshed_alm is on a distinguished road
Thanks for your help again. Yes I am planning to publish my work. May it will take approx. 2 months. My simulation is going good. I will update you once I get some results.Take care.

Cheers,
Morshed

Quote:
Originally Posted by CFDtoy View Post
Glad I could help. btw, are you planning to publish your work? Let me know how your simulation goes.

/CFDtoy
morshed_alm is offline   Reply With Quote

Reply

Tags
turbulence model, volume of fluid

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
NEED HELP on IC engine simulation with AVL FIRE! Mohsen khalafi Main CFD Forum 2 February 6, 2014 08:47
AVL Fire transonic simulation Ainil Main CFD Forum 1 August 24, 2010 15:53
gas properties in AVL Fire Morshed Alam Main CFD Forum 1 August 24, 2010 15:47
Combustion model for CAI/HCCI in AVL FIRE stoodent Main CFD Forum 0 July 19, 2009 18:37
FIRE 7.2 AVL Simone Lazzara Main CFD Forum 0 July 11, 2002 05:30


All times are GMT -4. The time now is 14:53.