I am trying to simulate a 2D impinging jet on a flat plate. I am having problems with the Boundary conditions. I have a symmetry boundary condition on the left side(west) of the 2D domain. The bottom boundary (south) is wall and is fine too. The top boundary(north) is divided into 2 parts, I(north) and B1(north). I have D/2 as inlet boundary condition at I(north)where I specify the downward jet velocity, on the top left, adjoining the symmetry boundary,and that is ok too. I am having problems with the boundary conditions at B1(north) and B2(right). I have used pressure for both B1 and B2 and the results are not good. I have used wall for B1 and outlet for B2 and then also it does not give good results.

Please let me know what boundary condition might be a realistic simulation of the Boundary conditions at B1 and B2. In Reality they are both open surfaces.

Thanks

Anindya

(1). Try to do simulation and setup boundary conditions "as if you are running the real experiment". (2). If the experimental setup is going to be in a large room with the jet and the flat wall somewhere in the center of the room, then you can include the room wall as the outer boundary. (3). If the experiment is carried out in an enclosure, then you need to simulate the enclosure wall as the boundary condition. (4). You can not set the boundary condition and location arbitrarily and hope to get the right answer.

Dear Anindya

Outlet or free BC are difficult tasks in which many CFD programmers employ a lot of time. I send you two references I used for a similar case. There you can choose among several proposals.

(1) Bruneau, CH-H and Fabrie, P. "Effective dowstream boundary conditions for incompressible Navier Stokes equations" Int. J. for Num. Methods in Fluids, Vol 19, 693-705 (1994) (2) Sani, R.L. and Gresho, P.M. "Resume and remarks on the open boundary conditions minisymposium", Int. J. for Num. Methods in Fluids, Vol 18, 983-1008, (1994)

Besides it, I would like to remark two aspects. (a) Is it a cylindrical (3D) jet simulated into 2D radial plane, or a plane 3D jet simulated into a 2D transverse plane? It could be possible you are loosing very interesting physical phenomena by imposing symmetry BC at west side. (b) What is the jet's Re?

Regards

Kike

Hi,

There are two points I know that may help you. First your boundary B2 should be sufficiently far away from the stagnation point. I used 8xD (with D the inlet diameter). Second it might be important to start the domain further upstream of the exit of the inlet pipe. This means that boundary B1 moves away from the wall and you need to simulate an extra part of the inlet pipe (hope this is clear). In my calculations the pipe exit was at 4xD from the impinged wall, but boundary B1 was at 5xD from the impinged wall.

If you have already done these two things, there is something else wrong. What do you mean with "not good results", divergence or a bad prediction of the flow field?

Regards, Luuk

For a plane jet, the "natural" solution (normalising everything) is trivial:

u = x

v = -y

p = p0 + 1/2 (x^2 + y^2)

A quick sketch will show this to have:

(1) strong varying pressure gradients along your free boundaries - precluding a constant static pressure boundary condition.

(2) significant (though constant) normal velocity components for your exit on the right - precluding the traditional "zero normal gradient" exit condition except near the bottom wall.

(3) constant normal velocity on the top half of the wall but, unfortunately, we cannot use a normal "exit" zero gradient condition here because the flow is coming in and almost all implementations are going to truncate the inflow to zero.

This is a lovely little class example! Before suggesting a solution can I ask what sets of boundary conditions your package has given you to play with?

Thanks everybody for your valuable suggestions. By not getting good results, I mean that my U (radial velocity) velocity is increasing with radial distance away from the symmetry line, instead of decreasing. Due to the effect of the bottom wall, I expect that the velocity should decrease as we go further away and that is reported in literature too.

I have tried to move the outlet further downstream, but still no effect as well as with different inlet velocity heights. Do you think it might be a problem with my grid density at specific locations or any other mistake I am making?

Thanks

Anindya

(1). The radial velocity is zero along the symmetry plane, so it should increase with r. (2). Since your jet is finite, the radial velocity will eventually decrease because of the viscous effect (the growth of the boundary layer on the bottom wall) (3). But since there is initial axial velocity (momentum) in the jet, the wall boundary layer will get thinner first and the radial velocity will increase, until the wall boundary layer start to grow again when r gets larger. (4). In any viscous calculation, you need to specify the Reynolds number(?). If the Reynolds number is high, the wall boundary layer will be thin, and the viscous effect will be slow. (5). Also you need to specify whether the flow is laminar or turbulent(?). (6). The mesh size and distribution will be a function of the Reynolds number and the turbulence model used(if required).

I agree with what John said, also tell us what kind of fluid are you using and what is the code. Generally, if you simulating liquid jet then you should simulate the FREE surface flow along the boundary B2. If you have air jet then your jet better to be confined (at B2) or so to maintain the continuity.

Before the jet hits the ground all the velocity is vertical and there is negligible horizontal or radial velocity. But after hitting the ground , it is mostly horizontal (radial) velocity U. My U profile shows increase with increasing L/r ratio. I have used values till L/r =5. L is the distance from the symmetry axis along the wall. r is 0.5 jet diameter. SHould I see if the velicty is decreasing for higher L/r ratios? my inlet jet diameter is 1 m and vel is 10m/s.

So why should my jet be confined at B2 for air? The aar has to come out of that boundary for realistic simulation.

Anindya

(1). It is important to know your Reynolds number, and the mesh size used (total number of mesh points or cells). And it is necessary to know whether you are running laminar or turbulent flow simulation.

Hi,

are you planning to publish your results? I'd be curious about that.

[jishnusoni]

Hello All,

I am trying to simulate an impingingjet using the simpleFoam in OF1.6.x. I am trying to follow the threads and tried different things. But I am still getting the same error. I am posting my error and attaching my initial bc.

Anindya, as you done a similar case before can you please help me in this matter.

Your support will be greatly appreciated.

Time = 759

DILUPBiCG: Solving for Ux, Initial residual = 0.364807, Final residual = 0.0331038, No Iterations 1
DILUPBiCG: Solving for Uy, Initial residual = 0.401396, Final residual = 0.0185339, No Iterations 1
DILUPBiCG: Solving for Uz, Initial residual = 0.439448, Final residual = 0.0046591, No Iterations 1
GAMG: Solving for p, Initial residual = 0.569614, Final residual = 0.00428777, No Iterations 66
time step continuity errors : sum local = 3.14096e+42, global = 3.09629e+39, cumulative = 6.80133e+40
DILUPBiCG: Solving for epsilon, Initial residual = 1.08298e-09, Final residual = 1.08298e-09, No Iterations 0
DILUPBiCG: Solving for k, Initial residual = 0.000115294, Final residual = 2.84805e-06, No Iterations 2
ExecutionTime = 47327.3 s ClockTime = 48069 s

Time = 760

DILUPBiCG: Solving for Ux, Initial residual = 0.506818, Final residual = 0.00973123, No Iterations 2
DILUPBiCG: Solving for Uy, Initial residual = 0.603294, Final residual = 0.0122224, No Iterations 2
DILUPBiCG: Solving for Uz, Initial residual = 0.280386, Final residual = 0.00518198, No Iterations 2
GAMG: Solving for p, Initial residual = 0.0695246, Final residual = 0.000686704, No Iterations 30
time step continuity errors : sum local = 1.41992e+43, global = 4.71133e+41, cumulative = 5.39147e+41
DILUPBiCG: Solving for epsilon, Initial residual = 3.87187e-11, Final residual = 3.87187e-11, No Iterations 0
DILUPBiCG: Solving for k, Initial residual = 1, Final residual = 0.0894909, No Iterations 1
bounding k, min: -7.27376e+51 max: 5.05817e+89 average: 5.17561e+84
ExecutionTime = 47386.5 s ClockTime = 48159 s

Time = 761

DILUPBiCG: Solving for Ux, Initial residual = 0.417362, Final residual = 0.0145424, No Iterations 1
DILUPBiCG: Solving for Uy, Initial residual = 0.51114, Final residual = 0.0224704, No Iterations 1
DILUPBiCG: Solving for Uz, Initial residual = 0.376437, Final residual = 0.0288099, No Iterations 1
GAMG: Solving for p, Initial residual = 0.629327, Final residual = 0.00528483, No Iterations 8
time step continuity errors : sum local = 1.11456e+78, global = 4.87405e+75, cumulative = 4.87405e+75
DILUPBiCG: Solving for epsilon, Initial residual = 4.23728e-09, Final residual = 4.23728e-09, No Iterations 0
#0 Foam::error:rintStack(Foam::Ostream&) in "/home/jish/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libOpenFOAM.so"
#1 Foam::sigFpe::sigFpeHandler(int) in "/home/jish/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libOpenFOAM.so"
#2 ?? in "/lib/libc.so.6"
#3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/home/jish/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libOpenFOAM.so"
#4 Foam::fvMatrix<double>::solve(Foam::dictionary const&) in "/home/jish/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libfiniteVolume.so"
#5 Foam::lduMatrix::solverPerformance Foam::solve<double>(Foam::tmp<Foam::fvMatrix<doubl e> > const&) in "/home/jish/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libincompressibleRASModels.so"
#6 Foam::incompressible::RASModels::kEpsilon::correct () in "/home/jish/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libincompressibleRASModels.so"
#7 main in "/home/jish/OpenFOAM/OpenFOAM-1.6.x/applications/bin/linux64GccDPOpt/simpleFoam"
#8 __libc_start_main in "/lib/libc.so.6"
#9 _start at /build/buildd/eglibc-2.10.1/csu/../sysdeps/x86_64/elf/start.S:116
Floating point exception




thanks

regards
jish

[elisun]

Hi.
I've got a problem with modeling an impinging jet with fluent. do i have to model the nozzle too? i mean since the flow has to be fully developed in the outlet of the nozzle, do i need to create the geometry of a pipe in gambit , or it's enough to just consider the exit of nozzle?
Tnx alot.

[romif]

Hi elisun.
For adequatre results you have to model a part of the tube (nozle) with length of about 1-2 of its diameter.
There are many literature obout jet impinging cooling (ex.1, ex.2).

jishnusoni,
do you resolve your problem? Maybe your mesh is not fine enough near the exit of inlet tube? Why do you use k-e model? It's overpredict heat transfer coefficient. I also deal with modeling of jet impinging and I use Durbin's V2F model.

Goodluck.

[Alhasan]

I'm doing impinging jet as well in open foam the problem atm is that there is flow coming in from the sides(outlet) . when i use zero gradient and when i use inletoutelt there is no flow from the sides but there is flow from the right corner ... I'm using exactly the same model which is there in the ex1 link which you have given, if you have any idea why this is happening please help me: i wanna know what boundry conditions to use fro the top patch.. the patch opposite to the impingement plate.. i cannot use wall coz its open to the atmosphere .. when i uses zero gradient I'm getting very mild flow coming in.. which is weird.????
regards
hasan.

[romif]

hasan, for the top patch I use the same BC as for the outlet patch (p=0, others=zero gradient). Try to use settings from my case

[Alhasan]

hey roman,
thanks for sharing your case i will also experiment with your boundry condition, and check with my results
-i am totally new to this openFoam and i will let you know what happens,
- why is your wall fixed value and 9.999999999e-21 for the K,
- what is this f and v2 in your 0 file
- what solver did you use for solving did u make your own solver or did you just use boutantboussisimpleFoam . . .
regards,
hasan.

[romif]

Hi hasan,
k=v2=f=0 - it's wall BC for Durbin's V2F model. Look here. I'm trying to implement it with realizable conditions for stagnation flow in OF. What turbulence model do you want to use?

Goodluck.

[Alhasan]

Hey,roman
im suposed to validate an experiment for high reynolds number and look at the results for heat transfer with different models like k-e k-w k-wsst and RSG. i had an option to choose any models under RANS and these were the ones i have chosen as of now, do you have any suggestions in OpenFoam for the models for impinging jets, you seemed to be more experienced with this particular case,
- why havnt you used Krwallfuntion in your case instead you have used fixed value
regards,
hasan

[Alhasan]

openFOAM doesn't seen to have durbin's V2F model, any suggestions how to i get this model into the openFOAM thanks