CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   CFX (https://www.cfd-online.com/Forums/cfx/)
-   -   Multiphase simulation (https://www.cfd-online.com/Forums/cfx/74788-multiphase-simulation.html)

 100tinela April 8, 2010 10:24

Multiphase simulation

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

 mach000 April 8, 2010 10:53

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

 freemankofi April 8, 2010 16:13

hi mach000,
were you able to fix that? I'm having similar problems.....

 100tinela April 8, 2010 16:20

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/

 ghorrocks April 8, 2010 18:17

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.

 mach000 April 9, 2010 03:34

Quote:
 Originally Posted by 100tinela (Post 253848) 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

 100tinela April 9, 2010 06:41

Quote:
 Originally Posted by mach000 (Post 253891) 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

 ghorrocks April 9, 2010 07:33

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.

 AliTr April 15, 2010 02:09

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.

 All times are GMT -4. The time now is 12:32.