
[Sponsors] 
May 8, 2008, 03:57 
Yes, LaunderSharma kepsilon m

#21 
Senior Member
Matvej Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 172
Rep Power: 8 
Yes, LaunderSharma kepsilon model is lowRe, but (on my opinion) you have fullydeveloped turbulent regime (1.0E+6 > 3.0E+5=Re_critical for sphere) and you can use kepsilon with standard wallfunctions, and y+ (for kepsilon model) should be in range 30150. May be your task is to use lowRe model in boudary layer and kepsilon in freestream...
today i'll download mesh and try it... 

May 8, 2008, 04:56 
What command line arguments ar

#22 
Senior Member
Matvej Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 172
Rep Power: 8 
What command line arguments are you using?
I use plot3dToFoam . . noBlank raetaf.x.fmt 2D 0.1 singleBlock scale 0.333 where 0.1 = 0.1ft (10% of airfoil chord length, which is 1ft, as mentioned on nasa.gov site) scale = 0.333 = convertion factor from [ft] to [m], because OpenFOAM uses metric (SI) system after conversion, i found, that: mesh has 66 high skewed faces (~12000%)  this VERY BAD and some very small edges. this is not good too. 

May 8, 2008, 05:36 
Hi there,
Doesn't "LowRe t

#23 
New Member
Steve Collie
Join Date: Mar 2009
Location: Valencia, Spain
Posts: 5
Rep Power: 8 
Hi there,
Doesn't "LowRe turbulence model" merely mean that it solves through the "lowre " (or Re_t) region of the flow, i.e. the viscous sublayer > it doesn't use wall functions. I don't think it matters what "global reynolds number" you have, it is still suitable as long as the flow isn't laminar or transitional. That said I seem to recall that it is a very stiff model (so can cause slow convergence) and has poorly defined boundary conditions at the wall (epsilon is undefined). A model like SpalartAlmaras which solves for nu_t (zero at the wall) might run better and has shown better accuracy for aerodynamic problems than kepsilon models. There is also the SST model but as far as I can see the version in openFoam 1.4.1 is not a low reynolds number implementation, you have to use wall functions and a y+>30. Does anybody know if there is a LowRe version of the SST out there?. Cheers, Steve 

May 8, 2008, 06:06 
Hi all
In the SST model the

#24 
Senior Member
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Deltares, Delft, The Netherlands
Posts: 1,608
Rep Power: 25 
Hi all
In the SST model the viscosity is the effective viscosity, thus that would make it possible to simulate all the way through the viscous sublayer, as nuEff = nuT + nuVisc. Thus it should be possible to apply kOmegaSST to your problem, as you are already having a fine resolution at the wing. The only thing which needs to be done (do not know if it is already implemented), is a boundary condition for omega. Enjoy this sunny day Niels
__________________
Please note that I do not use the Friendfeature, so do not be offended, if I do not accept a request. 

May 8, 2008, 11:02 
Leonardo Nettis, i have conver

#25 
Senior Member
Matvej Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 172
Rep Power: 8 
Leonardo Nettis, i have converted your mesh, and despite of high skewness at some faces, simpleFoam (steadystate solver) produces stable result with LaunderSharma ke model, now, i'm running LES simulation with SpalarAllmaras model, using soultion from simpleFoam. timestep is very low (5*10E7) and after first output i can send case to your email.
maybe i'm mistaken about lowre models  it seems that they are could be used with high Re numbers in freestream. however, oneeq SpalartAlmaras model is more suitable for your task 

May 8, 2008, 15:14 
ok, thank you very much krapos

#26 
Member
Leonardo Nettis
Join Date: Mar 2009
Posts: 72
Rep Power: 8 

May 12, 2008, 11:08 
Hi Matvey,
I've checked the

#27 
Member
Leonardo Nettis
Join Date: Mar 2009
Posts: 72
Rep Power: 8 
Hi Matvey,
I've checked the y+ in the LSKE steady case you sent me, with the refined grid made with salome, but its range is 625 that is not so acceptable. Anyway since I think I'm going to further reduce the cell size near the wall on your mesh, could you please tell me which utility you used in OF to achieve this purpose?? Thank you again LN 

May 12, 2008, 15:05 
O, i'm sorry, i'm keeping many

#28 
Senior Member
Matvej Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 172
Rep Power: 8 
O, i'm sorry, i'm keeping many versions at once (to reverse to old, if something goes wrong)
utility is called refineWallLayer it takes 4 parameters: case root (.) case name (.) patch name (walls) edgeWeight (0 to 1) for example, if you want nearwall distance to be twice smaller, you need to type: refineWallLayer . . walls 0.5 if you need nearwall distance to be ten times smaller, type refineWallLayer . . walls 0.1 utitlity alghorithm splits nearwall cells in patch normal direction by weighting factor and introduces new cells into the mesh, then the new mesh is written in time, one after the latest be careful, the best way  is to step by step experiment with utility and checking mesh for errors after each improvement. 

May 13, 2008, 10:16 
I've just tried to reduce the

#29 
Member
Leonardo Nettis
Join Date: Mar 2009
Posts: 72
Rep Power: 8 
I've just tried to reduce the near wall cell with an edgeweight equal to 0.5. Then I run checkMesh and the test failed for the High aspect ratio cells near the wall. Moreover I've tried to run simplefoam and the solution did not converge!
Maybe the solution could be to reduce the 3rd direction size. Did you create a 2d mesh?? Is this file located in the folders you sent me (so that I can import it in OF with a smaller zdir size)? If not could you please send me that? Thank you again LN 

May 14, 2008, 06:57 
1) contents of directory stead

#30 
Senior Member
Matvej Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 172
Rep Power: 8 
1) contents of directory steady_SAL:
0  intial values 2  mesh with refined boundaryLayer 202  values after 200 iterations with mesh, contained in 2 constant  initial mesh system  system so, may be you need to delete directory 2 and try to refine mesh again 2) the mesh is 2D (patches empty1 and empty2 are front and back planes of solution domain) 3) i think, it would be better to use next BC for variables: U inlet  fixedValue (33 0 0) walls fixedValue (33 0 0) outlet,top,bottom  pressureInletOutletVelocity (33 0 0) and internal field = (0 0 0) p inlet  zeroGradient walls  zeroGradient outlet,top,bottom  totalPressure {p0=0, gamma=0, phi=phi, U=U, rho=none, psi=none} k,epsilon inlet  fixedValue walls,outlet,top,bottom  zeroGradient epsilon should be estimated as C_mu^(0.75)*k^(1.5)/l_m where l_m can be estimated as 0.09*D, where D is airfoil chord length (25.4cm=0.254m) 

May 19, 2008, 01:17 
Hi, I'm also facing a problem

#31 
New Member
Mohd Yousuf
Join Date: Mar 2009
Location: Kharagpur
Posts: 18
Rep Power: 8 
Hi, I'm also facing a problem similar to this.
I have a mesh, while converting mesh once i did it using converttometers parameter as 1 in this case SimpleFoam is working properly but when i used converttometre as .0254 i'm facing many problems........ after 20 iterations simplefoam is giving error message ....... i tried using turbfoam but after 9 iterations suddenly courant number is increasin from 0.6 to 1800. This is the result of checkmesh Create polyMesh for time = constant Time = constant Mesh stats points: 160886 edges: 1048848 faces: 1739328 internal faces: 1666132 cells: 851365 boundary patches: 6 point zones: 0 face zones: 0 cell zones: 0 Number of cells of each type: hexahedra: 0 prisms: 0 wedges: 0 pyramids: 0 tet wedges: 0 tetrahedra: 851365 polyhedra: 0 Checking topology... Boundary definition OK. Point usage OK. Upper triangular ordering OK. Topological cell zipup check OK. Face vertices OK. Faceface connectivity OK. Number of regions: 1 (OK). Checking patch topology for multiply connected surfaces ... Patch Faces Points Surface wall1_periodic 15174 7764 ok (not multiply connected) wall2_periodic 15158 7756 ok (not multiply connected) top_wall 11701 6075 ok (not multiply connected) blade 27559 13844 ok (not multiply connected) air_inlet 1802 968 ok (not multiply connected) air_outlet 1802 968 ok (not multiply connected) Checking geometry... Domain bounding box: (0.198391 0.0421182 1.10082e08) (0.096859 0.0421504 0.123191) Boundary openness (4.82454e17 1.29423e15 1.80607e15) OK. Max cell openness = 1.83721e16 OK. Max aspect ratio = 7.81529 OK. Minumum face area = 4.58532e08. Maximum face area = 4.63974e05. Face area magnitudes OK. Min volume = 1.47244e11. Max volume = 9.59112e08. Total volume = 0.00151722. Cell volumes OK. Mesh nonorthogonality Max: 68.9708 average: 21.8092 Nonorthogonality check OK. Face pyramids OK. Max skewness = 0.955689 OK. Min/max edge length = 0.000213567 0.0119259 OK. All angles in faces OK. All face flatness OK. Mesh OK. End 

May 19, 2008, 05:00 
What BC's are you using?
Also

#32 
Senior Member
Matvej Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 172
Rep Power: 8 
What BC's are you using?
Also, write about your relaxation factors and "div" descritisation schemes 

May 19, 2008, 05:27 
wall1_periodic
{

#33 
New Member
Mohd Yousuf
Join Date: Mar 2009
Location: Kharagpur
Posts: 18
Rep Power: 8 
wall1_periodic
{ type patch; physicalType slip; } wall2_periodic { type patch; physicalType slip; } top_wall { type wall; physicalType wallFunctions; } blade { type wall; physicalType wallFunctions; } air_inlet { type patch; physicalType inlet; } air_outlet { type patch; physicalType pressureOutlet; } //div schemes divSchemes { default none; div(phi,U) Gauss upwind; div(phi,k) Gauss upwind; div(phi,epsilon) Gauss upwind; div(phi,R) Gauss upwind; div(R) Gauss linear; div(phi,nuTilda) Gauss upwind; div((nuEff*dev(grad(U).T()))) Gauss linear; } //relaxation factors relaxationFactors { p 0.3; U 0.7; k 0.7; epsilon 0.7; R 0.7; nuTilda 0.7; } basically when i import mesh with scale factor 1 it is working fine and with 25.4 this is working fine till now but i want to use for .0254(required for project) where it is not working properly..... can u suggest few changes that can help 

May 23, 2008, 22:22 
mohd yousuf,
is your case 3D

#34 
Senior Member
Matvej Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 172
Rep Power: 8 
mohd yousuf,
is your case 3D or 2D? 

May 25, 2008, 23:00 
hi matj,
Sorry for la

#35 
New Member
Mohd Yousuf
Join Date: Mar 2009
Location: Kharagpur
Posts: 18
Rep Power: 8 
hi matj,
Sorry for late reply it was weekend here. My case is a 3D case.Now i'm trying to solve the case using turbFoam. 

May 26, 2008, 10:16 
are you using tetmesh, or hex

#36 
Senior Member
Matvej Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 172
Rep Power: 8 
are you using tetmesh, or hex?
try relaxations factors 0.1 for all variables for the first 100200 iterations (in simpleFoam) can you send your case? 

May 27, 2008, 00:43 
Hi Matvej,
I'm using tetrah

#37 
New Member
Mohd Yousuf
Join Date: Mar 2009
Location: Kharagpur
Posts: 18
Rep Power: 8 
Hi Matvej,
I'm using tetrahedral mesh. Basically i somehow solved the problem for simplefoam case now i'm working in turbfoam case. In this case courant no. suddenly increases after few iterations. I have posted checkmesh results above do have a look Just now i have fired a run. Will mail you the case in nearly 8hrs from now. 

May 27, 2008, 06:21 
hey again,
Matvej......I ha

#38 
New Member
Mohd Yousuf
Join Date: Mar 2009
Location: Kharagpur
Posts: 18
Rep Power: 8 
hey again,
Matvej......I have seen that most of the times epsilon in my calculations get bounded.....and also somtimes it converges or diverges....... how can we prevent any quantity from getting bounded??? sometimes it fails when i calculate k and epsilon by formula given by few in this forum . is there any other way for calculating k and epsilon or is there any other slution 

May 28, 2008, 01:26 
if epsilon is always bounded,

#39 
Senior Member
Matvej Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 172
Rep Power: 8 
if epsilon is always bounded, than it means, that turbulence model diverges
what formula are u using? k=1.5*( (I*u_i)**2), I=0.01 (1%) epsilon=C_mu^0.75*k**(1.5)/l, l=0.07*D_c (D_c  cylinder diameter) are you using lowre model or wall functions? 

May 28, 2008, 01:37 
i'm using the same formula u m

#40 
New Member
Mohd Yousuf
Join Date: Mar 2009
Location: Kharagpur
Posts: 18
Rep Power: 8 
i'm using the same formula u mentioned
but l=.05(5%) i dont have much idea wat you mean by lowre or wallfunctions.......if you are talking of walls than i'm using wallfunctions and regarding velocity it is 73.9 and nu is 1.789e5 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Problem with turbFoam  skabilan  OpenFOAM Running, Solving & CFD  2  September 29, 2008 17:43 
Turbfoam error  danie  OpenFOAM Running, Solving & CFD  2  July 30, 2008 07:45 
TurbFoam  hsieh  OpenFOAM Running, Solving & CFD  12  July 23, 2008 07:40 
Error turbFoam  jackdaniels83  OpenFOAM Running, Solving & CFD  11  June 27, 2007 14:22 
Oodles vs turbFoam  rolando  OpenFOAM Running, Solving & CFD  9  June 4, 2007 05:42 