[Specialist]

hello guys,

right know I try to simulate a simple constant pipe flow with Open Foam. I use the solver "SimpleFoam". The pipe consisits of an an inlet on the left site and an outlet on the right site. At the cylindrical middle part friction exist.

I know the inflow velocity of 3 m/s. What about the BC?

Following BC are used in the velocity file:
Inlet

type fixed value
value uniform (3 0 0)

Outlet

zero gradient

middle part

fixed value
uniform (0 0 0)


in the Pressure file:
inlet

zero gradient

middle part

zero gradient

outlet

typ fixed value
value 0


I do not know why, but the simulation does not work. Can you give me a reason for that? Are the BC wrong?

Thanks!

Specialist

[tellico]

you might want to try specifying an inlet pressure, rather than an outlet pressure

I've encountered this problem myself and this was how I got around it,

[Specialist]

I thought about that.

Look at that example:

http://www.foamcfd.org/Nabla/guides/...Guidese13.html

The pressure at the outlet must be defined with 0. I am interested in the loss of pressure in the pipe. If I define the pressure at the inlet and at the outlet, I would definde the loss of pressure for myself.
That does not make sense?
Do I have to use other types of BC? Something like OutletInlet oder Inletoutled?
But I thought, I should be possible with the normal simple BC.

[jherb]

What does mean, your simulation does not work? Could you post the output of the solver.

[idefix]

Hello,
I am dealing with the same topic at the moment.
My aim is the calculation of the pressure drop in a pipe (diameter d=0.02m, length L=5 m).
I consider at the beginning a stationary, laminar, incompressible flow and try the simulation with simpleFoam.
To see that everything is correct I want to compare the simulation with the analytical result.

I calculate the analytical result in the following way:
velocity at the inlet: v=0.0884 m/s
viscosity: 1x10e-6 m^2/s
pressure drop : delta_p = lambda * L*density *v^2/d/2
lambda is the coefficient, defined: lambda=64/Reynolds-Number=0.0362
So the calculated pressure drop is: 35.3 Pa

Now I start the simulation:
After the calculation I´ve got a pressure-field and I used paraview to calculate the pressure drop (with the calculator: pressure * densitiy (1000 kg/m^3)
The pressure drop is 15 Pa, which is not equal to the pressure drop I calculated in the analytical way.

Does anyone know where my mistake is?

I also tried to calculate the pressure drop, when I initialized the velocity profile with u(r) = u_max (1 - (r/R)^2) , called Hagen-Poiseuille, with R=0.01 m and u_max = 0.14 m/s so that the mean velocity (integrated over the above velocity profile) is 0.0884 m/s.

Thanks a lot for your help



Here are the files I used:

the U-file is:

dimensions [0 1 -1 0 0 0 0];

internalField uniform (0 0 0);

boundaryField
{
inlet
{
type fixedValue;
value uniform (0 0.08842 0);
}

outlet
{
type zeroGradient;
//value uniform (0 0.08842 0);
}

fixedWalls
{
type fixedValue;
value uniform (0 0 0);
}

frontAndBack
{
type empty;
}
}

The p-file is:

dimensions [0 2 -2 0 0 0 0];

internalField uniform 0;

boundaryField
{
inlet
{
type zeroGradient;
}

outlet
{
type fixedValue;
value uniform 0;
}

fixedWalls
{
type zeroGradient;
}

frontAndBack
{
type empty;
}
}

my blockMesDict:

convertToMeters 1;

vertices
(
(0 0 0)
(0.01 0 0)
(0.01 5 0)
(0 5 0)
(0 0 0.02)
(0.01 0 0.02)
(0.01 5 0.02)
(0 5 0.02)
);
3
blocks
(
hex (0 1 2 3 4 5 6 7) (1 100 20) simpleGrading (1 1 1)
);

edges
(
);

boundary
(
inlet
{
type patch;
faces
(
(0 1 5 4)
);
}
fixedWalls
{
type wall;
faces
(
(0 1 2 3) //top
(6 7 4 5) //bottom
);
}
outlet
{
type patch;
faces
(
(6 2 3 7)
);
}
frontAndBack
{
type empty;
faces
(
(0 3 7 4)
(6 2 1 5)
);
}
);

mergePatchPairs
(
);

my fvSchemes:

ddtSchemes
{
default steadyState;
}

gradSchemes
{
default Gauss linear;
}

divSchemes
{
default none;
div(phi,U) Gauss linearUpwindV grad(U);
div(phi,k) Gauss upwind;
div(phi,omega) Gauss upwind;
div((nuEff*dev(T(grad(U))))) Gauss linear;
}

laplacianSchemes
{
default Gauss linear corrected;
}

interpolationSchemes
{
default linear;
}

snGradSchemes
{
default corrected;
}

fluxRequired
{
default no;
p;
}

my fvSolution-file:

solvers
{
p
{
solver GAMG;
tolerance 1e-7;
relTol 0.1;
smoother GaussSeidel;
nPreSweeps 0;
nPostSweeps 2;
cacheAgglomeration on;
agglomerator faceAreaPair;
nCellsInCoarsestLevel 10;
mergeLevels 1;
}

U
{
solver smoothSolver;
smoother GaussSeidel;
tolerance 1e-8;
relTol 0.1;
nSweeps 1;
}

}

SIMPLE
{
nNonOrthogonalCorrectors 0;
}

potentialFlow
{
nNonOrthogonalCorrectors 10;
}

relaxationFactors
{
fields
{
p 0.3;
}
equations
{
U 0.7;
}
}

cache
{
grad(U);
}

my transportPorperties-file:

transportModel Newtonian;

nu nu [0 2 -1 0 0 0 0] 0.000001;

[jherb]

@idefix: Are you using a turbulence model? Which? Your Re seems to be 1770 (calculating backward from lambda). So the flow is somewhere in the transition to a turbulent flow.

[idefix]

Hello Joachim

thanks for you answer.
I dont´use a turbulence model for this calculation, but I had the same thougth and changed the velocity to 0.265 m/s, so I am turbulent and I am using the k-epsilon-turublence model
I still have a big difference between simulation and analytical result.
But I changed the grid size to smaller cells and therefore I get closer to the real result.
As a consequence the time for othe simulation gets very big. Is there another way to get closer to the analytical result?

Thanks for your help
idefix

[jherb]

Just to be sure: Your solution is converged? The pressure difference is not oscillating between (time)steps?

[idefix]

I used simpleFoam in the steady state-modus.
It stopped when the convergence criterion is reached. Till there the pressure was not constant.
I calculated the pressure drop with the help of the following command:
patchAverage p inlet >inletAvP

because the pressure at the outlet is set to 0, the calculated pressure is the wished pressure drop -
I hope everything is correct, if not please tell me.

is there a reason why you are asking?

Thanks a lot
idefix

[jherb]

If you look at the pressure values of different steps of the simulation, do they converge (together with the residuals)?

[idefix]

I attached the residuals. Unfortunately the pressure is yello. I hope you can see it.
What do you think?

[jherb]

Do your result change, if you set the convergence criteria to 1e-4?

[idefix]

do you mean the tolerances in fvSolution-file?

[jherb]

I mean runtime control (chapter Residual/Convergence Control):
http://www.openfoam.org/version2.0.0...me-control.php

[idefix]

the calculation is still running.
the pressure residual and the residual of the velocity component in the main flow direction is not getting smaller than 10e-4

but the solution till now changes only with the first decimal place.

did you expect that?

Thanks a lot
idefix

[jherb]

Actually no. At the moment I do not have an idea what could cause this problem.

[alexeym]

Hi,

my guess is: two parallel infinite planes are rather poor model of tube

I've decided to make fully 3D simulation of the described laminar case. Pressure drop is around 40 Pa. Rather high, maybe due to rather coarse mesh in X-direction.

You can find case files (mesh is in Gmsh format) and pressure colour profile attached to the message.

Also here's simpleFoam output (at the point where I've decided to stop simulation):

...
Time = 218

DILUPBiCG:  Solving for Ux, Initial residual = 8.77581226583e-07, Final residual = 9.23550690215e-09, No Iterations 2
DILUPBiCG:  Solving for Uy, Initial residual = 3.83955671681e-05, Final residual = 1.96642296575e-07, No Iterations 2
DILUPBiCG:  Solving for Uz, Initial residual = 4.31920726089e-05, Final residual = 6.31032523367e-07, No Iterations 2
GAMG:  Solving for p, Initial residual = 3.79720211706e-06, Final residual = 3.77066594274e-07, No Iterations 141
GAMG:  Solving for p, Initial residual = 6.2556196152e-07, Final residual = 6.20062840895e-08, No Iterations 194
GAMG:  Solving for p, Initial residual = 1.54883049595e-07, Final residual = 1.52631870121e-08, No Iterations 151
time step continuity errors : sum local = 3.23088878426e-10, global = -1.41736741757e-12, cumulative = -2.60173230963e-07
ExecutionTime = 988.65 s  ClockTime = 989 s
...

[idefix]

Hello,
I tried a lot but still it doesn´t work.
Unfortunately I´ve got some "bad looking" cells at the end of the pipe and also I don´t get such a nice velocity distribution as you have.

I copied your whole case and just changed the mesh.

The picture shows the mesh cut in the middle.

Do you have any idea what I did wrong?

Thanks a lot for your help

[idefix]

here are the attached files

[alexeym]

Hi,

you should at least check your mesh before running case (and asking question ). Attached is a picture of the boundaries of the mesh in the attached case: green is outlet and red is walls. Well, at least inlet patch has correct geometry

Also to save computation time, try running simulation on 2D axisymmetric mesh (as anyway you're trying to check if simpleFoam will return pressure drop estimated from Darcy-Weisbach equation for circular tube).