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

Eulerian–Eulerian coupled with VOF

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

Reply
 
LinkBack Thread Tools Display Modes
Old   November 21, 2012, 14:24
Default Eulerian–Eulerian coupled with VOF
  #1
Senior Member
 
Jamal Foroozesh
Join Date: Oct 2012
Location: Iran
Posts: 126
Rep Power: 4
jamalf64 is on a distinguished road
Hi Dear friends,
How do Coupled Eulerian–Eulerian homogeneous multiphase Model with a VOF method in fluent?
(Eulerian–Eulerian homogeneous multiphase Models to calculate the flow field and VOF to determine shape of the free surface)
TNX
jamalf64 is offline   Reply With Quote

Old   November 22, 2012, 03:24
Default
  #2
Senior Member
 
ghost82's Avatar
 
Daniele
Join Date: Oct 2010
Location: Italy
Posts: 920
Rep Power: 15
ghost82 will become famous soon enough
Hi,
as I know you can only choose one multiphase model, eulerian multiphase or vof model.

Daniele
ghost82 is offline   Reply With Quote

Old   November 22, 2012, 03:35
Default
  #3
Senior Member
 
Jamal Foroozesh
Join Date: Oct 2012
Location: Iran
Posts: 126
Rep Power: 4
jamalf64 is on a distinguished road
Quote:
Originally Posted by ghost82 View Post
Hi,
as I know you can only choose one multiphase model, eulerian multiphase or vof model.

Daniele
Dear Daniele,
Thank you so much
Can you help me in my problem? (free surface simulation of stirred tank)
jamalf64 is offline   Reply With Quote

Old   November 22, 2012, 03:50
Default
  #4
Senior Member
 
ghost82's Avatar
 
Daniele
Join Date: Oct 2010
Location: Italy
Posts: 920
Rep Power: 15
ghost82 will become famous soon enough
Quote:
Originally Posted by jamalf64 View Post
Dear Daniele,
Thank you so much
Can you help me in my problem? (free surface simulation of stirred tank)
I can get you some tips; my experience in stirred tanks is limited to mrf steady state and unsteady sliding mesh, both single and multiphase (rushton turbines, maxblend impellers, anchor impellers, helicoidal impellers and "in-house impellers ").
However I never used the vof model to study the free surface: my "top" boundary condition was a simmetry condition in all simulations.
Post a sketch of what you want to do (domain, dimensions) and add some more details on fluids you want to mix.

Daniele
ghost82 is offline   Reply With Quote

Old   November 22, 2012, 04:17
Default
  #5
Senior Member
 
Jamal Foroozesh
Join Date: Oct 2012
Location: Iran
Posts: 126
Rep Power: 4
jamalf64 is on a distinguished road
Quote:
Originally Posted by ghost82 View Post
I can get you some tips; my experience in stirred tanks is limited to mrf steady state and unsteady sliding mesh, both single and multiphase (rushton turbines, maxblend impellers, anchor impellers, helicoidal impellers and "in-house impellers ").
However I never used the vof model to study the free surface: my "top" boundary condition was a simmetry condition in all simulations.
Post a sketch of what you want to do (domain, dimensions) and add some more details on fluids you want to mix.

Daniele
I want to simulate free surface of stirred tank, whether steady or transient. and VOF or eulerian-eulerian multiphase.

Last edited by jamalf64; November 22, 2012 at 07:27.
jamalf64 is offline   Reply With Quote

Old   November 22, 2012, 05:14
Default
  #6
Senior Member
 
ghost82's Avatar
 
Daniele
Join Date: Oct 2010
Location: Italy
Posts: 920
Rep Power: 15
ghost82 will become famous soon enough
Quote:
Originally Posted by jamalf64 View Post
I want to simulate free surface of stirred tank, whether steady or transient. and VOF or eulerian-eulerian multiphase.
Ok, since you want to study the water-air interface, I would suggest to use the vof model; as a first try you can try to see if with the implicit steady formulation you can obtain a converged solution (use low under relaxation factors, expecially for momentum); try the presto scheme for pressure discretization.
If you can't have a converged solution or your results are not accurate you have to switch to unsteady simulation (implicit formulation, less accurate then the explicit, but more stable); the time step will be dependent on the rotational speed of your impeller (the solution has to converge in max 40 iterations, if it doesn't reduce the time step).
As a first try I use a time step "time to complete one revolution/8".
For unsteady simulation you can use either mrf or sliding mesh approches: sliding mesh is more accurate, but it is more more expensive in therm of computational time.
Since you have not baffles, mrf should give good results.
Try to setup in fluent your problem, then report back if you have problems.

Daniele
ghost82 is offline   Reply With Quote

Old   November 22, 2012, 05:20
Default
  #7
Senior Member
 
Jamal Foroozesh
Join Date: Oct 2012
Location: Iran
Posts: 126
Rep Power: 4
jamalf64 is on a distinguished road
Quote:
Originally Posted by ghost82 View Post
Ok, since you want to study the water-air interface, I would suggest to use the vof model; as a first try you can try to see if with the implicit steady formulation you can obtain a converged solution (use low under relaxation factors, expecially for momentum); try the presto scheme for pressure discretization.
If you can't have a converged solution or your results are not accurate you have to switch to unsteady simulation (implicit formulation, less accurate then the explicit, but more stable); the time step will be dependent on the rotational speed of your impeller (the solution has to converge in max 40 iterations, if it doesn't reduce the time step).
As a first try I use a time step "time to complete one revolution/8".
For unsteady simulation you can use either mrf or sliding mesh approches: sliding mesh is more accurate, but it is more more expensive in therm of computational time.
Since you have not baffles, mrf should give good results.
Try to setup in fluent your problem, then report back if you have problems.

Daniele
Thank you so much
jamalf64 is offline   Reply With Quote

Old   November 22, 2012, 14:51
Default stirred tank
  #8
Senior Member
 
Jamal Foroozesh
Join Date: Oct 2012
Location: Iran
Posts: 126
Rep Power: 4
jamalf64 is on a distinguished road
dear friend,

I attached a file about my broblem.
if possible for you, please help me.
thank you so much

Last edited by jamalf64; November 22, 2012 at 17:18.
jamalf64 is offline   Reply With Quote

Old   November 22, 2012, 15:57
Default
  #9
Senior Member
 
ghost82's Avatar
 
Daniele
Join Date: Oct 2010
Location: Italy
Posts: 920
Rep Power: 15
ghost82 will become famous soon enough
Quote:
Originally Posted by jamalf64 View Post
dear friend,

I attached a file about my broblem.
if possible for you, please help me.
thank you so much
Hi!
please elaborate more "System must be stable after a period of time, but is not and results are wrong".
Why "impeller" is stationary?it should be rotating as shaft and fluid rotor..
Maybe also a pressure outlet for the top is more indicated instead of simmetry.

If possibile upload somewhere cas/dat files, if not possible post some contour picture of phases.

Daniele
ghost82 is offline   Reply With Quote

Old   November 22, 2012, 16:22
Default
  #10
Senior Member
 
Jamal Foroozesh
Join Date: Oct 2012
Location: Iran
Posts: 126
Rep Power: 4
jamalf64 is on a distinguished road
System should be stable after a period of time, but did not stable and it seems that results are wrong
Why "impeller" is stationary? Because tutorial of fluent(stirred tank) like this.
I set top of tank as pressure inlet (like tutorial of fluent) but results dont change.
Attached Images
File Type: jpg tuto+tphase2.jpg (33.4 KB, 23 views)
File Type: jpg tuto+tphase5.jpg (32.8 KB, 17 views)
File Type: jpg tuto+tphase8.jpg (34.9 KB, 14 views)
File Type: jpg tuto+tphase11.jpg (32.4 KB, 12 views)
File Type: png tuto+tphase14.PNG (37.3 KB, 13 views)

Last edited by jamalf64; November 22, 2012 at 17:39.
jamalf64 is offline   Reply With Quote

Old   November 22, 2012, 16:26
Default
  #11
Senior Member
 
Jamal Foroozesh
Join Date: Oct 2012
Location: Iran
Posts: 126
Rep Power: 4
jamalf64 is on a distinguished road
It is not possible to send case/dat files because their sizes is large (20MB).
forgive me
Attached Images
File Type: jpg tuto+tphase29.jpg (44.0 KB, 16 views)
File Type: jpg tuto+tphase38.jpg (28.9 KB, 8 views)
File Type: jpg tuto+tphase41.jpg (45.3 KB, 16 views)
jamalf64 is offline   Reply With Quote

Old   November 23, 2012, 04:11
Default
  #12
Senior Member
 
ghost82's Avatar
 
Daniele
Join Date: Oct 2010
Location: Italy
Posts: 920
Rep Power: 15
ghost82 will become famous soon enough
Are you sure you obtained a converged solution?
what are the values of residuals?
Can you create a vertical plane and post a contour of velocity magnitude?

Then, in fluent create 2 planes, below and above the impeller, then monitor the area weight velocity magnitude: the values must not change in each iteration; if the values are changing yet when the next iteration starts you have not a converged solution.
(Refer to the tank tutorial to monitor velocity magnitude values)

Shaft and impeller have to rotate: you can set the shaft to rotate with absolute rotational velocity and the impeller to rotate with 0 relative rotational velocity (in respect to the rotor fluid rotational velocity).

Daniele
ghost82 is offline   Reply With Quote

Old   November 23, 2012, 04:30
Default
  #13
Senior Member
 
Jamal Foroozesh
Join Date: Oct 2012
Location: Iran
Posts: 126
Rep Power: 4
jamalf64 is on a distinguished road
Quote:
Originally Posted by ghost82 View Post
Are you sure you obtained a converged solution?
what are the values of residuals?
Can you create a vertical plane and post a contour of velocity magnitude?

Then, in fluent create 2 planes, below and above the impeller, then monitor the area weight velocity magnitude: the values must not change in each iteration; if the values are changing yet when the next iteration starts you have not a converged solution.
(Refer to the tank tutorial to monitor velocity magnitude values)

Shaft and impeller have to rotate: you can set the shaft to rotate with absolute rotational velocity and the impeller to rotate with 0 relative rotational velocity (in respect to the rotor fluid rotational velocity).

Daniele
Im not sure.I'll do the things you said and report the results to you.all reseduals are 0.001
Attached Images
File Type: jpg tuto+tphase1.jpg (37.8 KB, 41 views)
File Type: jpg tuto+tphase4.jpg (37.8 KB, 27 views)
File Type: jpg tuto+tphase16.jpg (42.9 KB, 28 views)
File Type: jpg tuto+tphase31.jpg (44.7 KB, 18 views)
File Type: jpg tuto+tphase40.jpg (35.3 KB, 19 views)
jamalf64 is offline   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
problem about VOF and species couple Cloud FLUENT 0 June 15, 2012 01:23
the initialization of the coupled level set method and vof model in FLUENT 13.0 dutliang FLUENT 3 December 13, 2011 22:28
DPM model coupled with VOF Doug FLUENT 0 March 1, 2005 17:37
Difficult BCs about Freesurface Simulation by VOF Yongguang Cheng FLUENT 0 September 19, 2003 07:39
Coupled 1D/3D STAR-CD Training CD adapco Group Marketing CD-adapco 1 November 13, 2002 16:48


All times are GMT -4. The time now is 09:19.