CFD Online Discussion Forums

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   CFX (https://www.cfd-online.com/Forums/cfx/)
-   -   How to set phases with different velocity (https://www.cfd-online.com/Forums/cfx/101350-how-set-phases-different-velocity.html)

kbaker May 2, 2012 04:42

How to set phases with different velocity
 
Hello I am want to implement stratified two-phase flow by CFX. The phases are (Oil and Water) the oil flowing at the lower part of the pipe and water at the upper part. The two phases flows at different superficial velocities I need to ask how I can set the velocity of each phase in this case in CFX-Pre?
In Bump tutorial I saw they set only one velocity for both phases? Furthermore reference to my case which it better the segregated solved or the coupled solver?

Thanks a lot
Kbaker

juliom May 2, 2012 14:01

Dear colleague,
You do this, jsut defining to phases, and using the Euler-Euler model, specifically particle model.
At the inlet you define each velocity..
Good luck!

kbaker May 2, 2012 17:11

Hi thanks for the answer. Is Euler-Euler model is same as homogeneous model with free surface model available in Multiphase menu? How can I select particle model I think it not appropriate to my case cause I have continuous fluids (not have particles anymore within the domain of solution)?

ghorrocks May 2, 2012 19:09

You cannot see the phase velocities in the bump tutorial as it is a homongenous model - both phases share a single velocity field and this is appropriate for free surface models where you have one phase or the other and they do not mix. If you run an inhomogenous model then velocities will be available for both phases.

mariam.sara May 3, 2012 07:44

?????????????????????

kbaker May 3, 2012 07:52

Thanks ghorrocks for the reply. In my case the phases not mixed (I have stratified flow case) and there is a clear interface between them. If I use in-homogeneous model I think CFX will force the phases to be mixed and I not want this occurs? I want the phases flows within the pipe with different velocities separately? so is the in-homogeneous model ensure this thing?

ghorrocks May 3, 2012 08:22

Looks like I have confused mariam. At least I have achieved something today :)

If the phases never mix then use the homogenous model. You only use inhomogenous when interphase slip happens. In your case you define a boundary with the velocity defined by its position, but still using the homogenous model.

kbaker May 3, 2012 10:04

may you clear to me pls how I can apply what mentioned in your phrase (you define a boundary with the velocity defined by its position) in CFX-Pre?

ghorrocks May 3, 2012 10:08

If the surface is at z=0, then for z<0 you define velocity=0 [m/s], and where z>0 you define velocity=1[m/s].

kbaker May 3, 2012 13:08

You mean I need write CEL expression at inlet for the velocity? if it a CEL expression may you write it for the same conditions you mentioned me above in your example with surface at z=0 ?

ghorrocks May 3, 2012 18:23

Yes, a CEL expression. Have a look inthe documentation and tutorials on CEL, it is quite a simple language.

kbaker May 4, 2012 04:17

Well in Bump tutorial at inlet boundary they set the turbulent length scale as UpH is this the value for the height above the interface or the full channel height?
Another thing in Bump tutorial too at outlet boundary they define static pressure as equation represented by DownPres ? should I set the same relation to my case? As I know from the tutorial guide this relation depends on the expected height of free surface at outlet in my simulation the height of the free surface unknown at outlet (at inlet it known and I tried CEL expression for it) and I want it computed from the downstream flow reference to the boundary at inlet?

ghorrocks May 4, 2012 07:36

You should choose your boundary conditions to match what you are modelling.

Also boundaries which only see a single phase are much simpler. If you can make use of this it will be simpler.

kbaker May 4, 2012 07:56

1) You not answer my question about UpH at inlet boundary in Bump tutorial is it represent the height above the interface (air level above the interface)?

2) Another thing what you advice me to use at the outlet boundary? pressure outlet or opening boundary?

ghorrocks May 4, 2012 09:23

I have not looked at thtat tutorial in detail for a while. But if you understand the tutorial you will be able to work it out. So you better look at it a bit closer.

Use an outlet when you do not expect back flow as it is a more numerically stable boundary. Use openings when back flow is possible, but be aware that it will be less numerically stable. If you are putting a boundary near a separation it is probably better the move the boundary down stream to avoid it.

kbaker May 4, 2012 15:27

Thanks a lot ghorrocks for the valuable information. I have some doubts hope you explain it for me:
1) Reference to my case which it is better to use the segregated solver or coupled solver?
2) When I select homogeneous model>free surface model>standard should I select interface compression level or leave it clear? If yes how many interface level should I select?

Thanks
kbaker

ghorrocks May 5, 2012 08:25

1. Depends which side of bed you got out of this morning. They both have sterngths and weaknesses and I don't have time to describe them all.
2) The default settings are usually good. But if you have some time I recommend trying all the options and seeing what ones work well for your simulation.


All times are GMT -4. The time now is 07:22.