
[Sponsors] 
April 1, 2010, 12:12 
turbulent jet flow RANS validation

#1 
Senior Member
Join Date: Dec 2009
Posts: 112
Rep Power: 8 
Hey Foamers,
i have been trying to reproduce the "simplejet" from Sandia.gov ( http://www.sandia.gov/TNF/DataArch/ProJet.html ) . The results I produced so far are not matching the experimental data ! I would really appreciate some help here! I tried with 2 different Geometries. A 2D one, like a piece of paper A 3D one, like a piece of cake I have used 2 sets of boundary conditions for each Geometry Set A : zerogradient for outlet and sidewall. Set B : pressureInletOutletvelocity, pressureInletoutlet, inletoutlet (the more advanced BCs) > which gives the 4 cases of which i have the results compared with experimental data attached. For experimental data I used quads/squares. For Simulation data I used crosses/daggers. Each axial_distance/D has a certain colour (axial_distance/D=3.775 : green, axial_distance/D=15 : yellow, axial_distance/D=30: orange, axial_distance/D=50: red; so like a trafficlight: top to bottom  green, yellow, orange, red) So I would expect to have some daggers hitting the squares, in case that I have good results...but... The Results are always horrible! The axial velocity seems to be quite close to the experimental results. Radial profiles are faaaaaar away. I have massflow through the outer boundary, which should not be there. I expected this to be the cause for the bad results, but assigning phi=0 for that boundary did not fix the problem. I also tried different solvers (eg, simpleFoam, reactingFoam, rhoPisoFoam) without any success.. So I must be doing something essentially wrong here!??! Since I have figuered that some other people are having those issues it might be worth to work it out in detail. I will try to picture it in the next posts. I have:  Post with inletconditions  Post with BC and info for 2Dcase + results (using reactingFOAM)  Post with BC and info for 3Dcase + results (using reactingFOAM)  Post with 2D geometrydetails  Post with 3D geometrydetails  Post with results for 3Dgeometry with different solver Last edited by heavy_user; April 9, 2010 at 06:41. 

April 1, 2010, 12:32 
inlet Profiles

#2 
Senior Member
Join Date: Dec 2009
Posts: 112
Rep Power: 8 
I patched the inlet and the Internal field with the velocityprofile given by sandiadata (for r/R<smaller one I used a profile from a fully developed turbulent pipeflow, as stated in the sandiapaper).
I also used k and epsilon patches for the inlet an internal field.. For "k" i used k(r) = 3/2 * (factor(r) *U(r) For epsilon i used eps(r) = U(r)^(3/2)/ (0.0052 *0.1) I used the kepsilon Model for all Simulations. I used all of them for both geometries. Using reactingFoam i used: tophead for C3H8 (Y=1 for r/R<1) tophead for 02 (Y=0.21 for r/R>1) tophead for N2 (Y=0.79 for r/R>1) tophead for T (500K for r/R<1, 300K for r/R>1) Last edited by heavy_user; April 1, 2010 at 13:22. 

April 1, 2010, 12:56 

#3 
Senior Member
Join Date: Dec 2009
Posts: 112
Rep Power: 8 
The 2DGeometries flow direction is z.
I have a symmetryplane at the zaxes. I have 2 empty faces. Info and BC for case "2DA" : Code:
Geometie: block (symmetryPlane), Axial 2m , Radial 0,15m, D=5,5mm. cells (1 100 600) , Grading (1 30 40) smallest cell axial: 0,5mm , smallest cell radial 0,26mm Inlet:  vel: profile sandia  eps: profile sandia  k : profile sandia  T: Tophead (500 /300)  C3H8,O2,N2: Tophead  p: 101325; Sidewall: vel : zeroGradient; T : zeroGradient; p : zeroGradient; k: zeroGradient; eps: zeroGradient; Y,C3H8;O2 : zeroGradient; N2 : zeroGradient; Outlet: vel : zeroGradient; T : zeroGradient; p : zeroGradient; k: zeroGradient; eps: zeroGradient; Y,C3H8;O2 : zeroGradient; N2 : zeroGradient; InternalField: Profiles: U, eps, k , Tophead T, C3H8, O2,N2 uniform p 101325 timestep: 2,5e6 co(first step): Courant Number mean: 0.00744877 max: 0.342202 Mesh: hexahedra: 60000 Max cell openness = 2.21652e16 OK. Max aspect ratio = 54.1257 OK. Minumum face area = 5.49269e08. Maximum face area = 8.78116e05. Face area magnitudes OK. Min volume = 5.49269e11. Max volume = 8.78116e08. Total volume = 0.00035. Cell volumes OK. Mesh nonorthogonality Max: 1.40712 average: 0.526564 Nonorthogonality check OK. Face pyramids OK. Max skewness = 0.0624992 OK. Code:
Geometie: Schokoblock (symmetryPlane), Axial 2m , Radial 0,15m, D=5,5mm. Zellen (1 100 600) , Grading (1 30 40) Kleinste Zelle axial: 0,5mm , kleinste Zelle radial 0,26mm Inlet:  vel: profile  eps: profile sandia  k : profile sandia  T: Tophead  C3H8,O2,N2: Tophead  p: zeroGradient; Sidewall:jpg vel : type pressureInletOutletVelocity; value uniform (0 0 0); T : type inletOutlet; inletValue 380; p : type totalPressure; p0 uniform 101325; U U; phi phi; rho rho; psi none; gamma 1; value uniform 101325; k: type inletOutlet; inletValue uniform 0.001; eps: type inletOutlet; inletValue uniform 25000; Y,C3H8;O2 : type inletOutlet; inletValue uniform 0; N : type inletOutlet; inletValue uniform 1; Outlet: vel : type pressureInletOutletVelocity; value uniform (0 0 0); T: zeroGradient; p: type totalPressure; p0 uniform 101325; U U; phi phi; rho rho; psi none; gamma 1; value uniform 101325; >JanaF k: type inletOutlet; inletValue uniform 0.001; eps: type inletOutlet; inletValue uniform 25000; Y,C3H8;O2 : type inletOutlet; inletValue uniform 0; N : type inletOutlet; inletValue uniform 1; InternalField: Profiles: U, eps, k , C3H8, O2,N2 uniform p 101325, uniform T, co(first step): Courant Number mean: 0.0052683 max: 0.861124 Time = 2e06 Mesh: hexahedra: 60000 Max cell openness = 2.21652e16 OK. Max aspect ratio = 54.1257 OK. Minumum face area = 5.49269e08. Maximum face area = 8.78116e05. Face area magnitudes OK. Min volume = 5.49269e11. Max volume = 8.78116e08. Total volume = 0.00035. Cell volumes OK. Mesh nonorthogonality Max: 1.40712 average: 0.526564 Nonorthogonality check OK. Face pyramids OK. Max skewness = 0.0624992 OK. jpg I attached pictures: Results for 2DA (left) Code:
[Flowtime =1 sec !] Flux:Flux at sidewall = 0.000617497m^3/s [37.0498 l/min] Flux at outlet = 0.00181007m^3/s [108.604 l/min] Flux at inlet = 0.00117736m^3/s [70.6416 l/min] Pictures for 2DB results. A plot of velocity magnitude for 2DB @0.37 sec (which a could not attache due to a max of 5 files) would show eddies from the shearlayer in the domain. It does NOT reach a steady state with this BCs!! I guess this is the cause for the even worse profiles (high peak in radial profiles). Code:
Flowtime = 0.37 sec inlet 0.00174005m^3/s outlet 0.000597355m^3/s sidewall 0.00112035m^3/s Last edited by heavy_user; April 6, 2010 at 12:53. 

April 1, 2010, 13:15 

#4 
Senior Member
Join Date: Dec 2009
Posts: 112
Rep Power: 8 
The 3DGeometries flow direction is x.
I have 2 wedge faces Info and BC for case "3DA" : Code:
geo: piece of cake (wedge). Radial:0,15m ; Axial 1m ~ 200D. D=5,2mm. mesh (150 1 700), grading (2 1 2). > smallests cell radial:0.55mm , smalles cell axial : 0,8mm Inlet:  vel: profile  eps: profile sandia  k : profile sandia  T: Tophead  C3H8,O2,N2: Tophead  p: 101325; Sidewall: vel : zeroGradient; T : zeroGradient; p : zeroGradient; k: zeroGradient; eps: zeroGradient; Y,C3H8;O2 : zeroGradient; N : zeroGradient; Outlet: vel : zeroGradient; T : zeroGradient; p : zeroGradient; k: zeroGradient; eps: zeroGradient; Y,C3H8;O2 : zeroGradient; N : zeroGradient; InternalField: Profiles: U, eps, k , Tophead T, C3H8, O2,N2 uniform p 101325 timestep: 2,5e6 co(first step): Courant Number mean: 0.00744877 max: 0.342202 Mesh: Overall number of cells of each type: hexahedra: 104300 prisms: 700 Checking geometry... Boundary openness (2.68859e19 5.38961e16 7.2511e16) OK. Max cell openness = 2.25165e16 OK. Max aspect ratio = 65.5154 OK. Minumum face area = 2.0926e08. Maximum face area = 2.59139e05. Face area magnitudes OK. Min volume = 2.07199e11. Max volume = 3.57148e08. Total volume = 0.000980502. Cell volumes OK. Mesh nonorthogonality Max: 0 average: 0 Nonorthogonality check OK. Face pyramids OK. Max skewness = 0.330796 OK. Code:
geo: piece of cake (wedge). Radial:0,15m ; Axial 1m ~ 200D. D=5,2mm. mesh (150 1 700), grading (2 1 2). > smallests cell radial:0.55mm , smalles cell axial : 0,8mm Inlet:  vel: profile  eps: profile sandia  k : profile sandia  T: Tophead  C3H8,O2,N2: Tophead  p: zeroGradient; Sidewall: vel : type pressureInletOutletVelocity; value uniform (0 0 0); T : type inletOutlet; inletValue 380; p : type totalPressure; p0 uniform 101325; U U; phi phi; rho rho; psi none; gamma 1; value uniform 101325; k: type inletOutlet; inletValue uniform 0.001; eps: type inletOutlet; inletValue uniform 25000; Y,C3H8;O2 : type inletOutlet; inletValue uniform 0; N : type inletOutlet; inletValue uniform 1; Outlet: vel : type pressureInletOutletVelocity; value uniform (0 0 0); T: zeroGradient; p: type totalPressure; p0 uniform 101325; U U; phi phi; rho rho; psi none; gamma 1; value uniform 101325; k: type inletOutlet; inletValue uniform 0.001; eps: type inletOutlet; inletValue uniform 25000; Y,C3H8;O2 : type inletOutlet; inletValue uniform 0; N : type inletOutlet; inletValue uniform 1; InternalField: Profiles: U, eps, k , Tophead T, C3H8, O2,N2 uniform p 101325 timestep: 2,5e6 co(first step): Courant Number mean: 0.00744877 max: 0.342202 Mesh: Overall number of cells of each type: hexahedra: 104300 prisms: 700 Checking geometry... Boundary openness (2.68859e19 5.38961e16 7.2511e16) OK. Max cell openness = 2.25165e16 OK. Max aspect ratio = 65.5154 OK. Minumum face area = 2.0926e08. Maximum face area = 2.59139e05. Face area magnitudes OK. Min volume = 2.07199e11. Max volume = 3.57148e08. Total volume = 0.000980502. Cell volumes OK. Mesh nonorthogonality Max: 0 average: 0 Nonorthogonality check OK. Face pyramids OK. Max skewness = 0.330796 OK. You can see that there are still waves in the flowfield which do not show up with the setting of case 3DB. (for the 2D geometry it is vice versa ) I have allready tried to check if they dissapear with time. But another case still had those waves at flowtimes close to 1 sec. Code:
flowtime 0.11 sec massflow: inlet 0.0105862m^3/s outlet 0.00939795m^3/s sidewall 0.000142198m^3/s inlet  outlet [ 2m^3/s] = .00118825 Deviation from inflow through Inlet [%]: 11 Last edited by heavy_user; April 9, 2010 at 06:11. 

April 1, 2010, 13:20 

#5 
Senior Member
Join Date: Dec 2009
Posts: 112
Rep Power: 8 
Results for 3 DB
Code:
flowtime 0.474 sec massflow: inlet 0.00833534m^3/s outlet 0.00740893m^3/s sidewall 0.000926416m^3/s Last edited by heavy_user; April 6, 2010 at 07:59. 

April 1, 2010, 13:21 

#6 
Senior Member
Join Date: Dec 2009
Posts: 112
Rep Power: 8 
2D geometry.
Mainflow is in zDirection. Radialdirection = yDirection Code:
/** 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 1; vertices ( (0 0 0) //(0 r*cos(2.5°) r*sin(2.5°) 0) (0 0.14985723323727900000 0.00654290810480040000 ) (0 0.14985723323727900000 0.00654290810480040000 ) //some point for collapsing (0 0 0.05) (1 0 0) //(0 r*cos(2.5°) r*sin(2.5°) 0) (1 0.14985723323727900000 0.00654290810480040000 ) (1 0.14985723323727900000 0.00654290810480040000 ) //some point for collapsing (1 0 0.05) ); edges ( arc 1 2 (0 0.15 0 ) arc 5 6 (2 0.15 0) ); blocks ( hex (0 1 2 0 4 5 6 4) (150 1 700) simpleGrading (2 1 2) ); patches ( patch inlet ( (0 2 1 0) ) wall sidewall ( (2 6 5 1) ) wedge wedge ( (0 4 6 2) (1 5 4 0) ) patch outlet ( (4 5 6 4) ) ); mergePatchPairs ( ); // ************************************************************************* // Last edited by heavy_user; April 6, 2010 at 08:20. 

April 6, 2010, 08:23 

#7 
Senior Member
Join Date: Dec 2009
Posts: 112
Rep Power: 8 
3D Geometry.
Mainflow is along xAxes. Radial flow is along yaxes. Code:
/** 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 1; vertices ( (0 0 0) //(0 r*cos(2.5°) r*sin(2.5°) 0) (0 0.14985723323727900000 0.00654290810480040000 ) (0 0.14985723323727900000 0.00654290810480040000 ) //some point for collapsing (0 0 0.05) (1 0 0) //(0 r*cos(2.5°) r*sin(2.5°) 0) (1 0.14985723323727900000 0.00654290810480040000 ) (1 0.14985723323727900000 0.00654290810480040000 ) //some point for collapsing (1 0 0.05) ); edges ( arc 1 2 (0 0.15 0 ) arc 5 6 (2 0.15 0) ); blocks ( hex (0 1 2 0 4 5 6 4) (150 1 700) simpleGrading (2 1 2) ); patches ( patch inlet ( (0 2 1 0) ) wall sidewall ( (2 6 5 1) ) wedge wedge ( (0 4 6 2) (1 5 4 0) ) patch outlet ( (4 5 6 4) ) ); mergePatchPairs ( ); // ************************************************************************* // 

April 6, 2010, 08:24 

#8 
Senior Member
Join Date: Dec 2009
Posts: 112
Rep Power: 8 
Using rhoPisoFoam with the settings from case 3DB gets me the same mess.
Code:
Flowtime = 0.101 sec (intitial unsteadynes has passed the areas of sampling) This horrible values might be explained by the, not yet reached, steady state: inlet 0.0083681m^3/s outlet 0.00493538m^3/s sidewall 0.00343236m^3/s inlet  outlet [ 1m^3/s] = .00343272 deviation from flow through Inlet [%]: 41 Last edited by heavy_user; April 8, 2010 at 07:32. 

April 8, 2010, 07:33 

#9 
Senior Member
Join Date: Dec 2009
Posts: 112
Rep Power: 8 
Does anybody have ANY ideas what I could do to get results that have something in common with reality ??


April 9, 2010, 05:29 

#10 
New Member
Vadims Geza
Join Date: Apr 2010
Location: Latvia
Posts: 9
Rep Power: 7 
Hi!
Sorry, maybe I do not understand You problem well, but why You do not use at sidewalls type fixedValue in case of no slip and type slip in case of slip? In my opinion zerogradient and pressureInletOutletVelocity are more suitable for outlet. 

April 9, 2010, 06:24 

#11  
Senior Member
Join Date: Dec 2009
Posts: 112
Rep Power: 8 
Quote:
thanks for your reply! My problems are: 1.) I have flux through sidewall, where there should NOT be one. 2.) The results from Simulation do NOT match the experimental data. ( The experimental data (boxes) and the simulation data (crosses) have the same colour for different hights (eg. radial_distance/D = 30 is orange ,radial_distance/D = 50 is red), so i should have red crosses in red boxed, which i have not ) I have used 2 sets of boundary conditions for each Geometry (2dGeometry and 3Dgeometry). Set A : zerogradient for outlet and sidewall. Set B : pressureInletOutletvelocity, pressureInletoutlet, inletoutlet (the more advanced BCs) So if I understand your answer correctly, I have used everything but "type slip" which should roughly the same as setting the wallvelocity=velocity_of_coflow (right?). But i will give this version a go also and get back to you with the results. regards & nice weekend!! 

August 5, 2010, 04:52 

#12 
Senior Member
Join Date: Dec 2009
Posts: 112
Rep Power: 8 
Hi There,
by now I found some of my problems. I would like to share the solutions here. First of all "slip" did a great job! THX for that advice! Even though I still dont know why 0gradient did not work out... After that I figured that most essential Problem was a non constant massflow at the outlet. (picture attached) I tried a bunch of solvers and all of them had the nondecaying oscillation of masslfux at the outlet. The amplitude was different though. The ONLY way to have a decaying amplitude of the massflux oscillation at the outlet I found was "wavetransmissive" as BC. This was not strait forward for me, since I thought this BC was only needed for transonic or supersonic flows...However it works. Regards 

December 17, 2015, 21:35 

#13  
Member
Yan Wang
Join Date: May 2015
Location: Beijing
Posts: 30
Rep Power: 2 
Quote:
Sorry to start this old post, but I am trying to solve a jet flow too (CH4 into the air). It seems that you have solved the problem. Do you have any publications related to this? Thank you! Yan
__________________
Phd student, OpenFOAM, CFD, POD Blog: http://blog.sina.com.cn/multiphyzks RG:https://www.researchgate.net/profile/Yan_Wang154 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
simulation of a turbulent flow on airfoil  Dante  FLUENT  3  June 8, 2007 14:54 
Validation case for turbulent flow  Ratan  Main CFD Forum  0  October 4, 2005 03:03 
Validation case for turbulent flow  Ratan  Main CFD Forum  0  October 4, 2005 03:02 
Turbulent flow at walls in complex flows  Bo Jensen  Main CFD Forum  2  March 23, 2000 23:42 