CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   CFX (https://www.cfd-online.com/Forums/cfx/)
-   -   Outlet/opening boundary condition (https://www.cfd-online.com/Forums/cfx/109587-outlet-opening-boundary-condition.html)

 em11g09 November 21, 2012 06:37

Outlet/opening boundary condition

Hi

I am currently trying to model 2D free surface flow through a sump. I am having issues with my outlet boundary as I want to set it so there is no defined pressure or velocity. If I do set a pressure condition then fluid wants to flow back into the system due to the head loss through the sump. If I resolve this using an open boundary it is not realistic.

I have looked at the 2d flow over bump tutorial but that sets a down stream water level which I don't want to do.

Is there any outlet boundary condition or expression I can use which does not need to have a pressure or velocity set?

Thank you

 brunoc November 21, 2012 10:04

You can set the pressure level as an explicit result of the water level calculated by the solver. For a 2D case with a rectangular outlet boundary condition and gravity in +Y, this might do it:

Code:

```LIBRARY:   CEL:     EXPRESSIONS:       DenRef = 1.185 [kg m^-3]       DenWater = 997 [kg m^-3]       DenH = (DenWater - DenRef)       areaWater = areaInt(Water.Volume Fraction)@outflow       bottomYposition = 0 [m]       domainWidth = 0.01 [m]       aveWaterHeight = bottomYposition + areaWater / domainWidth       HidPressure = DenH * g * (aveWaterHeight - y) * step( (aveWaterHeight - y)/1[m] )     END   END END```
where 'HidPressure' is the value you set at the outflow region. It will probably make convergence harder, since you're no longer tying the outlet condition.

Cheers

 em11g09 November 22, 2012 10:51

Thanks that has worked for me. I have also run the test with a long channel downstream of the sump. Both methods give roughly the same results.

Thanks again

Ed

 All times are GMT -4. The time now is 15:41.