[mkraposhin]

Yes, LaunderSharma k-epsilon model is low-Re, but (on my opinion) you have fully-developed turbulent regime (1.0E+6 > 3.0E+5=Re_critical for sphere) and you can use k-epsilon with standard wall-functions, and y+ (for k-epsilon model) should be in range 30-150. May be your task is to use low-Re model in boudary layer and k-epsilon in freestream...

today i'll download mesh and try it...

[mkraposhin]

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.

[stevecollie]

Hi there,

Doesn't "Low-Re turbulence model" merely mean that it solves through
the "low-re " (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 Spalart-Almaras which solves
for nu_t (zero at the wall) might run better and has shown better
accuracy for aerodynamic problems than k-epsilon 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
Low-Re version of the SST out there?.

Cheers,
Steve

[ngj]

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

[mkraposhin]

Leonardo Nettis, i have converted your mesh, and despite of high skewness at some faces, simpleFoam (steady-state solver) produces stable result with Launder-Sharma k-e model, now, i'm running LES simulation with Spalar-Allmaras model, using soultion from simpleFoam. time-step is very low (5*10E-7) and after first output i can send case to your e-mail.

maybe i'm mistaken about low-re models - it seems that they are could be used with high Re numbers in freestream. however, one-eq Spalart-Almaras model is more suitable for your task

[dinonettis]

ok, thank you very much kraposhin!
my mail is nettis@imedado.poliba.it

Enjoy

LN

[dinonettis]

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 6-25 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

[mkraposhin]

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 near-wall distance to be twice smaller, you need to type:
refineWallLayer . . walls 0.5

if you need near-wall distance to be ten times smaller, type
refineWallLayer . . walls 0.1

utitlity alghorithm splits near-wall 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.

[dinonettis]

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 z-dir size)? If not could you please send me that?
Thank you again

LN

[mkraposhin]

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)

[yousuf]

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 zip-up check OK.
Face vertices OK.
Face-face 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 -1.10082e-08) (0.096859 0.0421504 0.123191)
Boundary openness (4.82454e-17 -1.29423e-15 1.80607e-15) OK.
Max cell openness = 1.83721e-16 OK.
Max aspect ratio = 7.81529 OK.
Minumum face area = 4.58532e-08. Maximum face area = 4.63974e-05. Face area magnitudes OK.
Min volume = 1.47244e-11. Max volume = 9.59112e-08. Total volume = 0.00151722. Cell volumes OK.
Mesh non-orthogonality Max: 68.9708 average: 21.8092
Non-orthogonality 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

[mkraposhin]

What BC's are you using?
Also, write about your relaxation factors and "div" descritisation schemes

[yousuf]

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

[mkraposhin]

mohd yousuf,
is your case 3D or 2D?

[yousuf]

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.

[mkraposhin]

are you using tet-mesh, or hex?

try relaxations factors 0.1 for all variables for the first 100-200 iterations (in simpleFoam)

can you send your case?

[yousuf]

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.

[yousuf]

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

[mkraposhin]

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 low-re model or wall functions?

[yousuf]

i'm using the same formula u mentioned

but l=.05(5%)

i dont have much idea wat you mean by low-re or wallfunctions.......if you are talking of walls than i'm using wall-functions and regarding velocity it is 73.9 and nu is 1.789e-5