CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   Pressure driven laminar flow simpleFoam pressure higher at the outlet than inlet (http://www.cfd-online.com/Forums/openfoam-solving/58888-pressure-driven-laminar-flow-simplefoam-pressure-higher-outlet-than-inlet.html)

gabriel October 23, 2007 08:04

Dear Friends, I am investi
 
Dear Friends,

I am investigating a realy difficult, scientific high demanding case :-) I have a pipe and a laminar flow. My boundary conditions are at the inlet velocity (0 0 0.1) and at the outlet pressure 0.

I start simulation with simpleFoam and the result is that the pressure at the outlet is higher than at the inlet. Nevetheless the flow streams from the inlet to the outlet.

I tried the simulation with OF 1.4 and OF 1.4.1.

What is wrong ?

And please do not write, that's an easy test case :-), it is not :-()

Thanks for any advice.

gabriel October 23, 2007 08:22

I forgot to say, Reynoldsnumbe
 
I forgot to say, Reynoldsnumber is 3.5.

mkraposhin October 23, 2007 09:53

Can you send (or post your tes
 
Can you send (or post your test case)? mkraposhin@inbox.ru

gabriel October 24, 2007 06:40

Hi, sure, do you know how i
 
Hi,

sure, do you know how i can add a .tar file on this message. So everybody can take this simple case and do his own stuff.

Best Gabriel

mkraposhin October 24, 2007 08:38

Probably, you can"t post tgz:
 
Probably, you can"t post tgz: - it will be too big.

benru October 24, 2007 08:53

Gabriel, see http://www.cfd-on
 
Gabriel, see http://www.cfd-online.com/cgi-bin/Op...ormatting#text

gabriel October 25, 2007 04:39

I put here the file. Again, it
 
I put here the file. Again, its a cylinder with a velocity inlet and a pressure outlet. Its laminar (inlet velocity 0.001 m/s) viscosity 1 and the radius is ca. 0.246 so the Reynoldsnumger is for this case is much below 1. The residuals do not converge.

If you have any suggestion, i think it would be nice for the whole community


gabriel October 25, 2007 04:39

I put here the file. Again, it
 
I put here the file. Again, its a cylinder with a velocity inlet and a pressure outlet. Its laminar (inlet velocity 0.001 m/s) viscosity 1 and the radius is ca. 0.246 so the Reynoldsnumger is for this case is much below 1. The residuals do not converge.

If you have any suggestion, i think it would be nice for the whole community


gabriel October 25, 2007 04:47

I send the file by email. It i
 
I send the file by email. It is only 1.9Mb but to large to post it.

Every one who wants this case can e-mail me.

Again, its a cylinder with a velocity inlet and a pressure outlet. Its laminar (inlet velocity 0.001 m/s) viscosity 1 and the radius is ca. 0.246 so the Reynoldsnumger is for this case is much below 1. The residuals do not converge.

If you have any suggestion, i think it would be nice for the whole community, because a flow in a pipe is quite frequent.

benru October 25, 2007 07:12

2 Gabriel I don't understan
 
2 Gabriel

I don't understand U=zeroGradient on WALL for gas laminar flow - it should be fixedValue=0.0. And (may be it's not a critical) outlet I would change on pressureOutlet. p should be defined as non-zero - uniform 1e+05 (normal atmospheric pressure) - for pressureOutlet and internalField. R - I think you should to see in the similar cases.

gabriel October 25, 2007 10:11

2 Ruben Thank you very much
 
2 Ruben

Thank you very much! U=zeroGradient on Wall is exactly the error!!! Pressure does not matter (us much Hrv writes in other sections) because the code is normalized. Pressure is always treated as a relative pressure. If I put 1e5 on the outlet then i get the absolut pressure, if i put 0 i only get the relative pressure. Adding a reference pressure (e.g. 1e5) leads again to the absolute pressure.

Again: Thank you very much! Now it looks as a very stupid error, and ... honestly ... it is :-)

Bests Gabriel

gabriel October 25, 2007 10:26

Now changing the grid and usin
 
Now changing the grid and using a more sofisticated mesh for mixing purpose, I get the following error message. I have tried to play a little around with tolerances, underrelaxation, etc. Has anybody similar experiences? Is there a solution?

Error message:

Reading field U

Reading/calculating face flux field phi

Selecting incompressible transport model Newtonian
Selecting turbulence model laminar

Starting time loop

Time = 1

DILUPBiCG: Solving for Ux, Initial residual = 1, Final residual = 0.099712, No Iterations 1
DILUPBiCG: Solving for Uy, Initial residual = 1, Final residual = 0.0148155, No Iterations 2
DILUPBiCG: Solving for Uz, Initial residual = 1, Final residual = 0.0852757, No Iterations 1
#0 Foam::error::printStack(Foam:http://www.cfd-online.com/OpenFOAM_D...part/proud.gifstream&) in "/data/home/bg/OpenFOAM/OpenFOAM-1.4.1/lib/linux64GccDPOpt/libOpenFOAM.so"
#1 Foam::sigFpe::sigFpeHandler(int) in "/data/home/bg/OpenFOAM/OpenFOAM-1.4.1/lib/linux64GccDPOpt/libOpenFOAM.so"
#2 ?? in "/lib64/libc.so.6"
#3 Foam::DICPreconditioner::calcReciprocalD(Foam::Fie ld<double>&, Foam::lduMatrix const&) in "/data/home/bg/OpenFOAM/OpenFOAM-1.
4.1/lib/linux64GccDPOpt/libOpenFOAM.so"
#4 Foam::DICPreconditioner::DICPreconditioner(Foam::l duMatrix::solver const&, Foam::Istream&) in "/data/home/bg/OpenFOAM/OpenFOA
M-1.4.1/lib/linux64GccDPOpt/libOpenFOAM.so"
#5 Foam::lduMatrix::preconditioner::addsymMatrixConst ructorToTable<foam::dicprecond itioner>::New(Foam::lduMatrix::solver const&,
Foam::Istream&) in "/data/home/bg/OpenFOAM/OpenFOAM-1.4.1/lib/linux64GccDPOpt/libOpenFOAM.so"
#6 Foam::lduMatrix::preconditioner::New(Foam::lduMatr ix::solver const&, Foam::Istream&) in "/data/home/bg/OpenFOAM/OpenFOAM-1.4.
1/lib/linux64GccDPOpt/libOpenFOAM.so"
#7 Foam::PCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/data/home/bg/OpenFOAM/OpenFOAM-1
.4.1/lib/linux64GccDPOpt/libOpenFOAM.so"
#8 Foam::fvMatrix<double>::solve(Foam::Istream&) in "/data/home/bg/OpenFOAM/OpenFOAM-1.4.1/lib/linux64GccDPOpt/libfiniteVolume.s
o"
#9 main in "/data/home/bg/OpenFOAM/OpenFOAM-1.4.1/applications/bin/linux64GccDPOpt/simpleFo am"
#10 __libc_start_main in "/lib64/libc.so.6"
#11 Foam::regIOobject::readIfModified() in "/data/home/bg/OpenFOAM/OpenFOAM-1.4.1/applications/bin/linux64GccDPOpt/simpleFo am"

[2]+ Gleitkomma-Ausnahme simpleFoam /c/home/bg FINE_nu0.007_v0.01 >log

hjasak October 25, 2007 10:35

Congratulations for getting ov
 
Congratulations for getting over the first stupid mistake. The new one looks like you've got a zero-volume cell in your mesh, which clearly is not allowed. Try running checkMesh and see what it says.

Enjoy,

Hrv

gabriel October 26, 2007 09:49

Thanks, I made a complete new
 
Thanks, I made a complete new mesh. It was a mesh with tetras, hexas and prism, and I don't know why, it was not possible to correct it, either smoothing it in ICEM. Now i use a full tetra mesh, and its fine.

Thanks,

Gabriel

yousuf May 16, 2008 05:44

Mr. Gabriel my system also giv
 
Mr. Gabriel my system also gives the same error message as yours. Can you please tell me how you resolved the problem .

I checked the mesh everything looks fine.

Thanx
Yousuf.

sarajags_89 September 30, 2009 17:43

hi to all
 
hey guys I am trying to solve a simple problem. I

---------------------------------------
____..................._______
inlet |...................| outlet
.......|.................. |
.......| ..................|
.......|. .................|
.......|___________|
acutally i modified the lid driven cavity problem to create this geometry.
i specified velocity in inlet as
movingWall (this is my inlet )
{
type fixedValue;
value uniform (10 0 0);

} movingWall1 (this is my oultet)
{

type zeroGradient;
}

and pressure values as follows

movingWall
{
type zeroGradient;
}

movingWall1
{
type fixedValue;
value uniform 2;
}


when i run icoFoam i get the following error ..
Create time

Create mesh for time = 0

Reading transportProperties

Reading field p

Reading field U

Reading/calculating face flux field phi


Starting time loop

Time = 0.001

Courant Number mean: 0 max: 1


This mesh contains patches of type empty but is not 1D or 2D
by virtue of the fact that the number of faces of this
empty patch is not divisible by the number of cells.

From function emptyFvPatchField<Type>::updateCoeffs()
in file fields/fvPatchFields/constraint/empty/emptyFvPatchField.C at line 148.

FOAM exiting

i am a beginner so sorry if i have made a silly mistake..thanks guys

sarajags_89 September 30, 2009 18:20

this is my mesh
 
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 1.6 |
| \\ / A nd | Web: http://www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

convertToMeters 0.1;


vertices

(

(0 0 0)

(2 0 0)

(-1 2 0)

(0 2 0)

(2 2 0)

(3 2 0)

(3 3 0)

(2 3 0)
(0 3 0)
(-1 3 0)
(0 0 .5 )
(2 0 .5)
(-1 2 .5)
(0 2 .5)
(2 2 .5)
(3 2 .5)
(-1 3 .5)
(0 3 .5)
(2 3 .5)
(3 3 .5)


);


blocks

(

hex (0 1 4 3 10 11 14 13) (5 5 1) simpleGrading (1 1 1)
hex (3 4 7 8 13 14 18 17) (5 5 1) simpleGrading (1 1 1)
hex (2 3 8 9 12 13 17 16) (5 5 1) simpleGrading (1 1 1)
hex (4 5 6 7 14 15 19 18) (5 5 1) simpleGrading (1 1 1)

);


edges

(

);


patches

(

wall movingWall1

(
(9 16 12 2)
)
wall movingWall

(
(6 19 15 5)
)

wall fixedWalls

(


(12 2 3 13)
(13 3 0 10)
(5 15 14 4)
(4 14 11 1)
(9 8 17 16)
(7 6 19 18)
)

empty frontAndBack

(
(18 19 15 14)
(14 11 10 13)
(13 12 16 17)
(17 18 14 13)
(7 6 5 4)
(4 1 0 3)
(3 2 9 8)
(8 7 4 3)


)

);


mergePatchPairs

(

);


// ************************************************** *********************** //


All times are GMT -4. The time now is 04:39.