[100tinela]

Hi,

I´m 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 I´d 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 didn´t know how to set this initial level of water and separate it from the air, like a two phase system. I´ve 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 couldn´t find the same situation on tutorials. Can someone help me?

Thanks,
Willian

[mach000]

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]

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

[100tinela]

Hi,

Yes, it´s my first multiphase simulation and I can´t 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]

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]

Originally Posted by 100tinela

Hi,

Yes, it´s my first multiphase simulation and I can´t 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]

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, I´ll try that.

Thanks for your help,
Willian

[ghorrocks]

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.

create an hexa elements mesh

Yes, free surface models are typically more mesh quality sensitive than other applications.

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]

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.