[masuarez]

I am using Openfoam 1.7 chtMultiRegionSimpleFoam solver and I'm trying to get the same results as in Fluent. However, I'm getting different results (Pressure and Velocity).

My case is as follows:

Straight duct with a constant temperature bottom wall. the area of the inlet is 4x10-6 m^2. Reynolds no of 2000 (laminar flow). length of pipe is .25 m

The following are my boundary conditions

0/u:
inlet
type flowRateInletVelocity
flowRate 7.28e-5
value uniform (0 0 0)

outlet
type outletInlet
outletValue uniform(0 0 0)
value uniform(0 0 0)

0/prgh

inlet
type fixedValue
value $internalField

outlet
type outletInlet
value $internalField
outletValue $internalField

For my pressure boundary conditions I have tried several other ones such as :

fixedValue
zeroGradient
inletOutlet
etc

I have not tried freeStreamPressure because i Dont know if it applies in this case

Any help is greatly appreciated!!!! PLEASE HELP!!!!!!!!

Miguel

[Jean El-Hajal]

Hi Miguel,

is there a big difference in the results calculated with Fluent and OpenFoam ? could you give us some figures or graph.

Could you post your case ? so we can have a look at it.

Jean

[masuarez]

Jean,

the difference in the pressure and velocities between Fluent and OpenFOAM are pretty significant. as you can see in the pictures, Fluent has an outlet velocity of approx 13 m/s, however, Openfoam has a velocity of < 2.5 m/s.

Obviously there is an issue with my boundary conditions that I have not been able to solve. Any help is greatly appreciated.

I attached my case (B.C., fv, etc).

Thank you.

[Jean El-Hajal]

Hi Miguel,

Try to change the boundary condition in 0/p_rgh like that:

inlet
{
type zeroGradient;
}

outlet
{
type fixedValue;
value uniform 1.0e5;
}

Also the temperature are in Kelvin, check the temperature value !!!
jean

[masuarez]

j

Originally Posted by Jean El-Hajal

Hi Miguel,

Try to change the boundary condition in 0/p_rgh like that:

inlet
{
type zeroGradient;
}

outlet
{
type fixedValue;
value uniform 1.0e5;
}

Also the temperature are in Kelvin, check the temperature value !!!
jean

I actually used the following boundary conditions for pressure:

inlet
{
type mixed;
refValue uniform 1e5;
refGradient uniform 0;
valueFraction uniform .5;
}

outlet
{
type fixedValue;
value uniform 1e5;
}

and it is giving me better results (meaning outlet velocities higher than the ones at inlet)

regarding the Temperature... i made sure that the units were Kelvin.

as soon as I have consistent results with fluent I will post my case and my results

Thank you so much for your help.

Miguel

[maddalena]

Hello all,
I am running a chtMultiRegionSimpleFoam case on OF 1.6-x. The geometry is quite simple: a pipe flow with air, used to cool some warm surrounding solids.
BC is more or less standard, however I have some doubt about the pressure outlet BC. I used:
- inlet: U fixedValue, p buoyantPressure;
- outlet: U zeroGradient; p fixedValue;
as made on the chtMultiRegionSimpleFoam tutorial, but I have high continuity errors:

time step continuity errors : sum local = 0.2007526, global = 0.004036046, cumulative = 0.220919

and in the end the solution diverges. I guess the problem is on pressure BC. Any suggestions on the subject?

mad

[masuarez]

Mad,

I have used the following boundary conditions for my pressure and velocity:

-inlet: U flowRateInletVelocity, p_rgh mixed (with value fraction = .5)
-outlet: U inletOutlet (or fluxCorrectedVelocity), p_rgh mixed (with value fraction = .5)

I have confirmed my results with FLUENT when my flow was laminar, but when i have turbulent flow, my results differ a little than FLUENT. They are not completely off, about 5 - 10 %.

I recommend that you look at

http://www.cfd-online.com/Forums/ope...-no-catch.html

by m.nichols19. he has a pretty detailed case involving buoyantPressure boundary conditions.

Good luck and hopefully this helps.

Miguel