Multiphase simulation

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

 April 8, 2010, 10:24 Multiphase simulation #1 New Member   Willian Join Date: Jan 2010 Location: Brasil Posts: 22 Rep Power: 8 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

 April 8, 2010, 10:53 #2 Member   Ciro Cannavacciuolo Join Date: Mar 2009 Posts: 35 Rep Power: 9 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

 April 8, 2010, 16:13 #3 Member   Freeman Adane Join Date: Apr 2010 Posts: 42 Rep Power: 8 hi mach000, were you able to fix that? I'm having similar problems.....

 April 8, 2010, 16:20 #4 New Member   Willian Join Date: Jan 2010 Location: Brasil Posts: 22 Rep Power: 8 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

 April 8, 2010, 18:17 #5 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 12,719 Rep Power: 99 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.

April 9, 2010, 03:34
#6
Member

Ciro Cannavacciuolo
Join Date: Mar 2009
Posts: 35
Rep Power: 9
Quote:
 Originally Posted by 100tinela 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

April 9, 2010, 06:41
#7
New Member

Willian
Join Date: Jan 2010
Location: Brasil
Posts: 22
Rep Power: 8
Quote:
 Originally Posted by mach000 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.

Willian

April 9, 2010, 07:33
#8
Super Moderator

Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,719
Rep Power: 99
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.

April 15, 2010, 02:09
#9
Member

Ali Torbaty
Join Date: Jul 2009
Location: Sydney, Australia
Posts: 72
Rep Power: 9
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.

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post austin FLUENT 2 February 25, 2009 09:38 Kushagra CFX 2 July 8, 2008 21:14 Luk CFX 2 June 5, 2008 11:31 Kushagra CFX 0 April 24, 2008 19:51 Tim CFX 10 April 3, 2008 18:13

All times are GMT -4. The time now is 06:08.