CFD Online Discussion Forums

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   FLUENT (https://www.cfd-online.com/Forums/fluent/)
-   -   Eulerian–Eulerian coupled with VOF (https://www.cfd-online.com/Forums/fluent/109607-eulerian-eulerian-coupled-vof.html)

jamalf64 November 21, 2012 13:24
Eulerian–Eulerian coupled with VOF
 
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

ghost82 November 22, 2012 02:24
Hi,
as I know you can only choose one multiphase model, eulerian multiphase or vof model.

Daniele

jamalf64 November 22, 2012 02:35
Quote:
Originally Posted by ghost82 (Post 393593)
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)

ghost82 November 22, 2012 02:50
Quote:
Originally Posted by jamalf64 (Post 393595)
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

jamalf64 November 22, 2012 03:17
Quote:
Originally Posted by ghost82 (Post 393598)
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.

ghost82 November 22, 2012 04:14
Quote:
Originally Posted by jamalf64 (Post 393601)
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

jamalf64 November 22, 2012 04:20
Quote:
Originally Posted by ghost82 (Post 393611)
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 November 22, 2012 13:51
stirred tank
 
dear friend,

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

ghost82 November 22, 2012 14:57
Quote:
Originally Posted by jamalf64 (Post 393699)
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

jamalf64 November 22, 2012 15:22
5 Attachment(s)
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.

jamalf64 November 22, 2012 15:26
3 Attachment(s)
It is not possible to send case/dat files because their sizes is large (20MB).
forgive me

ghost82 November 23, 2012 03:11
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

jamalf64 November 23, 2012 03:30
5 Attachment(s)
Quote:
Originally Posted by ghost82 (Post 393762)
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

DEVARAJAN K May 23, 2016 08:08
Quote:
Originally Posted by jamalf64 (Post 393712)
It is not possible to send case/dat files because their sizes is large (20MB).
forgive me
I am also working in the multiphase simulation of stirred tanks. In these images of volume fraction, impeller zone is black. How you had done this? In my case, impeller and baffle regions are also coming in the phases after patching


All times are GMT -4. The time now is 21:01.