[em11g09]

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]

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:

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]

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