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

Question for gas/liquid flow

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

Reply
 
LinkBack Thread Tools Display Modes
Old   July 20, 2001, 03:23
Default Question for gas/liquid flow
  #1
J.W.Ryu
Guest
 
Posts: n/a
Hi,

I am trying to solve two fluid (gas & liquid phase) at same time in Fluent 5.5. Bowl contains liquid, and is being rotated with constant angular velocity. Gas phase is passing above liquid surface with constant velocity. Cylinder type heat source provides thermal energy to liquid and gas phase, which is positioned at the outside of bowl.

I assigned natural & foced convection flow term for liquid, and tried to solve thermal and fluid flow field at same time.

But, it was not cnverged due to quite different density of gas and liquid phase.

If I assign liquid surface as wall(slip wall) instead of interior, this model can be converged. But, axial flow of gas and liquid is not allowed by wall.

Could you let me know how I can make well converged results for this model?

Thanks,
  Reply With Quote

Old   July 20, 2001, 03:50
Default Re: Question for gas/liquid flow
  #2
Alain
Guest
 
Posts: n/a
what kind of multiphase model do you tried ?

If you use VOF I think want you can't model heat transfert in FLUENT 5.5

Multiphase flow is quite always hard to converge, the reasons why depends on the model you use.

Best regards

Alain

  Reply With Quote

Old   July 20, 2001, 08:09
Default Re: Question for gas/liquid flow
  #3
J.W.Ryu
Guest
 
Posts: n/a
Thanks for your kind comment. I also considered VOF for my model. But, VOF is improper for my model because of complexity.

I have large size of tank(cooling wall) system. Some solid structure including insulation, heating source, bowl and so on are encapsuled in consant low pressure. Gas phase flows from inlet to outlet of tank, and passes on the liquid surface. Liquid is contained in bowl, which is being rotated in constant angular velocity.

I think Steady state condition is better to understand the fluid flow and thermal condition in the tank.

The main diiculties to be converged are 1. Natural convection of liquid 2. Significant density difference between liquid and gas phases.

In case of #2, Interlayer between gas phase and liquid surface is automatically assigned interior. So, density difference did not allow converging. I changed this interior to wall at boundary condition. But, wall did not permit swirl velocity of liquid. That means swirl velociy near by wall is nearly zero. So, I gave slide wall condition which has no shear stress. But, this condition does not permit axial directional flow(normal to the liquid surface).

So, I would like to know how I can converge from interior between liquid surface and gas phase instead wall condition. Would you give me good method?

Thanks,
  Reply With Quote

Old   July 25, 2001, 13:44
Default Re: Question for gas/liquid flow
  #4
Alain
Guest
 
Posts: n/a
So if you don't use VOF what kind of model do you use : the algebraic model in fluent 5.5 or the euler / euler model of fluent 4 ?

Anyway this some clues in order to have a chance to converge :

1. run in transient mode. Even if your are only interested in steady state, the steady solution is hard to obtain directly.

2. Check your discretisation order you should use 1st order at the begining of the calculation to improve stability.

3 check out your pressure/velocity coupling. Fluent recommand the body weight interpolation for multiphase flow and it is true that it improve stability.

4. If you run euler/euler model on FLUENT 4 try to converge without multigrid. It's slower but it's easier !

5. Use a step by step strategy for convergence : run your multiphase flow without heat transfert and turbulence with a low rotating velocity, increase the rotating velocity, enable turbulence, enable heat transfert,...etc

6. Underelax interphase exchange term, pressure and turbulence.

I hope this could help you.

Best regards

Alain
  Reply With Quote

Old   August 4, 2001, 04:06
Default Re: Question for gas/liquid flow
  #5
david
Guest
 
Posts: n/a
A) I am confused with ur system. B) what I understand, you have a rotary bowl rotating at x rpm, on the top there is air and bottom is filled with liquid water, now you want to model the free surface with heat transfer.. am I right? C) what's the pressure of the air? D) How did you confirm that bcos of ONLY density difference, you didn't get a converged solution ? E) I don't think you would get a steady state solution

DC
  Reply With Quote

Old   August 4, 2001, 09:34
Default Re: Question for gas/liquid flow
  #6
J.W.Ryu
Guest
 
Posts: n/a
(a) Please consider crystal crowth(Czhochoralski method) system. (b) is correct. (c) pressure is no matter. Actually 20 torr. (d) intentional wall between liquid and gas made converging. Intentionally given similar density between liquid and gas made converging, even if interface between liquid and gas phase was assigned as interior. So, I think density difference between liquid(2.52g/cc) and gas(0.014g/cc). Generally interface between liquid and gas phase was assigned as interior. With this condition, converging was not happend. (e) I think time dependence is too complicate to apply in my system.

Thanks,

JW
  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
mass flow in is not equal to mass flow out saii CFX 2 September 18, 2009 08:07
Question about Couette Flow Tiger Main CFD Forum 1 March 24, 2006 00:16
Question about flow in ducted fan in another duct Jane FLUENT 0 June 21, 2004 13:57
Question concerning about the flow simulation of a fan in an engine room. ghlee Main CFD Forum 3 October 21, 1998 07:05


All times are GMT -4. The time now is 22:44.