CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   Outlet boundary condition (http://www.cfd-online.com/Forums/cfx/73376-outlet-boundary-condition.html)

 colen March 6, 2010 01:39

Outlet boundary condition

I am modelling a multiphase flow using a rectangular box. The solid inlet is on the top and gas inlet at the side.My outlet is the other side. I specified my gas inlet boundary as inlet and the normal speed. The solid inlet is based on th fluid dependent. For the outlet boundary, i specified the boundary condition as outlet and the static pressure is zero. By doing this, the turbulence energy of the air was diverging and this resulted into domain instability.

I need advise on how to resolve this problem and what outlet boundary condition is the best to use

 enr_venkat March 6, 2010 05:35

Hi,

Though i'm not an expert in CFX, i could tell you something about boundary conditions which i learnt from FLUENT presentation. But i worked in Multiphase flows using STAR CCM+. Pressure inlet / Presure outlet conditions normally leads to high fluctuations in Turbulence Kinetic energy and mass and momentum. Mass flow rate inlet / static pressure outlet is more robust than pressure inlet/outlet condition. Fluctuations would be minimal. I hope meshing wouldn't be an issue as you have a rectangular box model. Try refining the BCs. I hope this helps you.

 ghorrocks March 6, 2010 05:41

Can you describe what you are modelling a bit more?

Do you need to model the air on top of the liquid? If you use a degassing boundary at the liquid surface then you won't have to model the air and your turbulence problem disappears. But whether this is appropriate depends on what you are actually trying to model.

 colen March 8, 2010 01:17

I am modelling gas-solid interaction with the solid inlet at top of a rectangular box while the gas inlet is the side of the box. As advised, I changed the gas inlet to bulk mass flowrate with the volume fraction for air to be 1 and volume fraction for solid to be zero at the gas inlet. I maintained the outlet as outlet boundary condition but mass and momentum was modelled as static pressure. I got the notice below at each time steps but the solution didn't diverge. I don't understand what this means.
****** Notice ****** |
| A wall has been placed at portion(s) of an OUTLET |
| boundary condition (at 70.0% of the faces, 70.1% of the area) |
| to prevent fluid from flowing into the domain. |
| The boundary condition name is: Outlet. |
| The fluid name is: Sand. |
| If this situation persists, consider switching |
| to an Opening type boundary condition instead.

 enr_venkat March 8, 2010 04:10

Warning message alerts you about the outgoing flow re entering into the domain through outlet. CFX tries to close the portion of outlet face by covering the percentage of face with wall so that no re entry happens. Opening boundary condition enables the flow to interact with the atmosphere in which flow conditions at the outlet is almost exposed to atmospheric pressure and temperature. I could see that 70% face coverage with wall is higher. Face coverage upto 25 % is acceptable as suggested by CFX support engineer. Try refining the physical timescale. How is the convergence trend ? Do you see high fluctuations in the residuals ? Even i'm working on the convergence criteria as i stii didn't get smooth curve as expected. Always check the .out file for converged solution. Check whether solver has completed the run based on outer iterations reach or residual target reach. You would be aware as
proper solution is achieved only after reaching residual target no matter how the fluctuations are.

 crmorton March 8, 2010 14:53

When I come across problems like this, I usually manually stop the solution, and take a look at the results in CFX post. A velocity vector plot can usually identify the source of the problem (e.g., a stationary re-circulation zone intersecting with the outlet of the domain). If the size of the domain is not as important as the mixing characteristics near the inlet location(s), then increasing the distance between the inlet and outlet location(s) may help rectify the issue.

 enr_venkat March 8, 2010 23:49

I tried with the concept of increasing the distance between the inlet and outlet to avoid the intersection of recirculation zone with outlet during one of the simulations in automotive EGR valve application. I didn't get the proper convergence trend. Moreover convergence stability was not great. I'm aware that there could be so many other factors that affect convergence stability like mesh, y+ condition at the boundary layers, etc.,.

 All times are GMT -4. The time now is 22:33.