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

Multiphase simulation

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

Reply
 
LinkBack Thread Tools Display Modes
Old   April 8, 2010, 10:24
Default Multiphase simulation
  #1
New Member
 
Willian
Join Date: Jan 2010
Location: Brasil
Posts: 22
Rep Power: 7
100tinela is on a distinguished road
Hi,

Iīm learning using Ansys CFX 12.0 and a have a problem with multiphase simulation. My geometry is a kind of cup with an initial level of water and Iīd like simulate the flow inside it when the wall rotates at 2 rad/s, considering a steady state analysis. On CFX-Pre, I started defining in my default domain two fluids, air and water, but I didnīt know how to set this initial level of water and separate it from the air, like a two phase system. Iīve already considered no slip wall, laminal flow, buoyancy and surface tension but my results for volume fraction on CFD-Post are not what I expect, like a paraboloid shape. I couldnīt find the same situation on tutorials. Can someone help me?

Thanks,
Willian
100tinela is offline   Reply With Quote

Old   April 8, 2010, 10:53
Default
  #2
Member
 
Ciro Cannavacciuolo
Join Date: Mar 2009
Posts: 35
Rep Power: 8
mach000 is on a distinguished road
Hi, maybe I can help you but I think that the simulation is too complicated for one person that now is learning code.
So, could you send me an image of your domain?
Is it your first multiphase simulation?

Regards
mach000 is offline   Reply With Quote

Old   April 8, 2010, 16:13
Default
  #3
Member
 
Freeman Adane
Join Date: Apr 2010
Posts: 42
Rep Power: 7
freemankofi is on a distinguished road
hi mach000,
were you able to fix that? I'm having similar problems.....
freemankofi is offline   Reply With Quote

Old   April 8, 2010, 16:20
Default
  #4
New Member
 
Willian
Join Date: Jan 2010
Location: Brasil
Posts: 22
Rep Power: 7
100tinela is on a distinguished road
Hi,

Yes, itīs my first multiphase simulation and I canīt find anywhere an example for a similar simulation in Ansys CFX. As a first aproximation, I created a simple cilynder using ICEM tools and allowed an auto sizing meshing.
My parameters are basically a rotating wall, 2 rad/s, and top surface open to atmosphere and my initial condition is that 50% of cilynder volume is full of water. I think my problem is setting this initial level of water and make sure that there is a two phase situation (Air, Water). Is there any difference in results between defining a new material as a mixture and selecting two materials in domain settings?

Thanks a lot for your help,
Willian

Ps.: ICEM Mesh: http://img641.imageshack.us/i/cilindro.png/

Last edited by 100tinela; April 8, 2010 at 16:22. Reason: Icem mesh: http://img697.imageshack.us/i/cilindroy.jpg
100tinela is offline   Reply With Quote

Old   April 8, 2010, 18:17
Default
  #5
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,824
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
It is very hard to run free surface simulations steady state. You will probably have to run the simulation as a transient and wait for the surface to settle out.
ghorrocks is offline   Reply With Quote

Old   April 9, 2010, 03:34
Default
  #6
Member
 
Ciro Cannavacciuolo
Join Date: Mar 2009
Posts: 35
Rep Power: 8
mach000 is on a distinguished road
Quote:
Originally Posted by 100tinela View Post
Hi,

Yes, itīs my first multiphase simulation and I canīt find anywhere an example for a similar simulation in Ansys CFX. As a first aproximation, I created a simple cilynder using ICEM tools and allowed an auto sizing meshing.
My parameters are basically a rotating wall, 2 rad/s, and top surface open to atmosphere and my initial condition is that 50% of cilynder volume is full of water. I think my problem is setting this initial level of water and make sure that there is a two phase situation (Air, Water). Is there any difference in results between defining a new material as a mixture and selecting two materials in domain settings?

Thanks a lot for your help,
Willian

Ps.: ICEM Mesh: http://img641.imageshack.us/i/cilindro.png/
First of all i think the mesh in not the correct one for a multiphase problem. You have to create a mesh with very small elements near the position of the freesurface. The elements of your mesh are too big and they are not able to model the freesurface correctly.
Then, why don't you try to create an hexa elements mesh?
Finally, in order to simulate a multiphase simulation you need to define some expression such as Stevin Law and the initial quote of the freesurface. You will find theese expressions in some tutorials. Let me know
mach000 is offline   Reply With Quote

Old   April 9, 2010, 06:41
Default
  #7
New Member
 
Willian
Join Date: Jan 2010
Location: Brasil
Posts: 22
Rep Power: 7
100tinela is on a distinguished road
Quote:
Originally Posted by mach000 View Post
First of all i think the mesh in not the correct one for a multiphase problem. You have to create a mesh with very small elements near the position of the freesurface. The elements of your mesh are too big and they are not able to model the freesurface correctly.
Then, why don't you try to create an hexa elements mesh?
Finally, in order to simulate a multiphase simulation you need to define some expression such as Stevin Law and the initial quote of the freesurface. You will find theese expressions in some tutorials. Let me know
Ok, Iīll try that.

Thanks for your help,
Willian
100tinela is offline   Reply With Quote

Old   April 9, 2010, 07:33
Default
  #8
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,824
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Quote:
You have to create a mesh with very small elements near the position of the freesurface.
While this will increase accuracy of resolution of the free surface it will also make convergence even harder.

Quote:
create an hexa elements mesh
Yes, free surface models are typically more mesh quality sensitive than other applications.

Quote:
in order to simulate a multiphase simulation you need to define some expression such as Stevin Law and the initial quote of the freesurface.
A simple function like water up to height x and air above that is OK for an initial condition.

Don't use the surface tension model unless you need it. It makes convergence even harder and mesh quality requirements even stricter.

And as I previously said, you have little hope in getting this to work steady state. You will have to run transient and march it out until the waves die down.
ghorrocks is offline   Reply With Quote

Old   April 15, 2010, 02:09
Default
  #9
Member
 
Ali Torbaty
Join Date: Jul 2009
Location: Sydney, Australia
Posts: 71
Rep Power: 8
AliTr is on a distinguished road
Quote:
While this will increase accuracy of resolution of the free surface it will also make convergence even harder.
to help convergence on free surface models, I suggest putting a plane where your average water level is, then create inflation layers in both sides (up/down) of this plane. this method will results in much better convergence.
AliTr 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
multiphase simulation crash austin FLUENT 2 February 25, 2009 09:38
Single phase result file for multiphase simulation Kushagra CFX 2 July 8, 2008 21:14
Multiphase radiation in Ansys 10 problem Luk CFX 2 June 5, 2008 11:31
LES for multiphase simulation Kushagra CFX 0 April 24, 2008 19:51
multiphase simulation... 2D flow through an elbow Tim CFX 10 April 3, 2008 18:13


All times are GMT -4. The time now is 23:48.