CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Main CFD Forum

Impinging Jet Boundary Conditions

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree1Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   April 24, 2001, 15:31
Default Impinging Jet Boundary Conditions
  #1
Anindya
Guest
 
Posts: n/a
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
  Reply With Quote

Old   April 24, 2001, 17:19
Default Re: Impinging Jet Boundary Conditions
  #2
John C. Chien
Guest
 
Posts: n/a
(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.
  Reply With Quote

Old   April 25, 2001, 03:43
Default Re: Impinging Jet Boundary Conditions
  #3
Kike
Guest
 
Posts: n/a
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
  Reply With Quote

Old   April 25, 2001, 03:48
Default Re: Impinging Jet Boundary Conditions
  #4
Luuk Thielen
Guest
 
Posts: n/a
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
  Reply With Quote

Old   April 25, 2001, 04:29
Default Re: Impinging Jet Boundary Conditions
  #5
andy
Guest
 
Posts: n/a
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?

  Reply With Quote

Old   April 29, 2001, 02:05
Default Re: Impinging Jet Boundary Conditions
  #6
Anindya
Guest
 
Posts: n/a
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
  Reply With Quote

Old   April 29, 2001, 02:47
Default Re: Impinging Jet Boundary Conditions
  #7
John C. Chien
Guest
 
Posts: n/a
(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).
  Reply With Quote

Old   April 29, 2001, 06:33
Default Re: Impinging Jet Boundary Conditions
  #8
A.Hassaneen
Guest
 
Posts: n/a
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.
  Reply With Quote

Old   April 29, 2001, 11:30
Default Re: Impinging Jet Boundary Conditions
  #9
Anindya
Guest
 
Posts: n/a
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
  Reply With Quote

Old   April 29, 2001, 14:00
Default Re: Impinging Jet Boundary Conditions
  #10
John C. Chien
Guest
 
Posts: n/a
(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.
  Reply With Quote

Old   May 10, 2001, 05:26
Default Re: Impinging Jet Boundary Conditions
  #11
Dzsugasvilly
Guest
 
Posts: n/a
Hi,

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

Old   April 11, 2010, 06:31
Default
  #12
New Member
 
Join Date: Feb 2010
Posts: 21
Rep Power: 7
jishnusoni is on a distinguished road
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
Attached Files
File Type: gz 0.tar.gz (1.4 KB, 63 views)
harsha_kulkarni likes this.
jishnusoni is offline   Reply With Quote

Old   May 15, 2011, 15:02
Default impinging jet
  #13
New Member
 
Join Date: Apr 2011
Posts: 5
Rep Power: 6
elisun is on a distinguished road
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.
elisun is offline   Reply With Quote

Old   November 19, 2011, 15:27
Default
  #14
New Member
 
Roman
Join Date: Mar 2009
Location: Belarus
Posts: 6
Rep Power: 8
romif is on a distinguished road
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.
romif is offline   Reply With Quote

Old   December 30, 2011, 16:15
Default
  #15
Senior Member
 
Alhasan's Avatar
 
Hasan K.J.
Join Date: Dec 2011
Location: Bristol, United Kingdom
Posts: 181
Rep Power: 5
Alhasan is on a distinguished road
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.
Alhasan is offline   Reply With Quote

Old   January 4, 2012, 08:54
Default
  #16
New Member
 
Roman
Join Date: Mar 2009
Location: Belarus
Posts: 6
Rep Power: 8
romif is on a distinguished road
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
romif is offline   Reply With Quote

Old   January 4, 2012, 13:46
Default Thanks, roman
  #17
Senior Member
 
Alhasan's Avatar
 
Hasan K.J.
Join Date: Dec 2011
Location: Bristol, United Kingdom
Posts: 181
Rep Power: 5
Alhasan is on a distinguished road
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.
Alhasan is offline   Reply With Quote

Old   January 5, 2012, 11:25
Default
  #18
New Member
 
Roman
Join Date: Mar 2009
Location: Belarus
Posts: 6
Rep Power: 8
romif is on a distinguished road
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.
romif is offline   Reply With Quote

Old   January 6, 2012, 14:13
Default
  #19
Senior Member
 
Alhasan's Avatar
 
Hasan K.J.
Join Date: Dec 2011
Location: Bristol, United Kingdom
Posts: 181
Rep Power: 5
Alhasan is on a distinguished road
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 is offline   Reply With Quote

Old   January 6, 2012, 14:15
Default
  #20
Senior Member
 
Alhasan's Avatar
 
Hasan K.J.
Join Date: Dec 2011
Location: Bristol, United Kingdom
Posts: 181
Rep Power: 5
Alhasan is on a distinguished road
openFOAM doesn't seen to have durbin's V2F model, any suggestions how to i get this model into the openFOAM thanks
Alhasan is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Water subcooled boiling Attesz CFX 7 January 5, 2013 04:32
Boundary conditions in FireFOAM 1.7.1 for Jet Fires hafiidz OpenFOAM 2 December 8, 2010 11:09
Convective Heat Transfer - Heat Exchanger Mark CFX 6 November 15, 2004 16:55
Boundary conditions? Tom Main CFD Forum 0 November 5, 2002 02:54
Boundary Conditions Jan Ramboer Main CFD Forum 11 August 16, 1999 08:59


All times are GMT -4. The time now is 18:10.