CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

HELP NEEDED with TURBFOAM

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

Reply
 
LinkBack Thread Tools Display Modes
Old   May 8, 2008, 03:57
Default Yes, LaunderSharma k-epsilon m
  #21
Senior Member
 
mkraposhin's Avatar
 
Matvej Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 172
Rep Power: 8
mkraposhin is on a distinguished road
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 is offline   Reply With Quote

Old   May 8, 2008, 04:56
Default What command line arguments ar
  #22
Senior Member
 
mkraposhin's Avatar
 
Matvej Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 172
Rep Power: 8
mkraposhin is on a distinguished road
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.
mkraposhin is offline   Reply With Quote

Old   May 8, 2008, 05:36
Default Hi there, Doesn't "Low-Re t
  #23
New Member
 
Steve Collie
Join Date: Mar 2009
Location: Valencia, Spain
Posts: 5
Rep Power: 8
stevecollie is on a distinguished road
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
stevecollie is offline   Reply With Quote

Old   May 8, 2008, 06:06
Default Hi all In the SST model the
  #24
ngj
Senior Member
 
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Rotterdam, The Netherlands
Posts: 1,592
Rep Power: 24
ngj will become famous soon enoughngj will become famous soon enough
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 Friend-feature, so do not be offended, if I do not accept a request.
ngj is offline   Reply With Quote

Old   May 8, 2008, 11:02
Default Leonardo Nettis, i have conver
  #25
Senior Member
 
mkraposhin's Avatar
 
Matvej Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 172
Rep Power: 8
mkraposhin is on a distinguished road
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
mkraposhin is offline   Reply With Quote

Old   May 8, 2008, 15:14
Default ok, thank you very much krapos
  #26
Member
 
Leonardo Nettis
Join Date: Mar 2009
Posts: 72
Rep Power: 8
dinonettis is on a distinguished road
ok, thank you very much kraposhin!
my mail is nettis@imedado.poliba.it

Enjoy

LN
dinonettis is offline   Reply With Quote

Old   May 12, 2008, 11:08
Default Hi Matvey, I've checked the
  #27
Member
 
Leonardo Nettis
Join Date: Mar 2009
Posts: 72
Rep Power: 8
dinonettis is on a distinguished road
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
dinonettis is offline   Reply With Quote

Old   May 12, 2008, 15:05
Default O, i'm sorry, i'm keeping many
  #28
Senior Member
 
mkraposhin's Avatar
 
Matvej Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 172
Rep Power: 8
mkraposhin is on a distinguished road
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.
mkraposhin is offline   Reply With Quote

Old   May 13, 2008, 10:16
Default I've just tried to reduce the
  #29
Member
 
Leonardo Nettis
Join Date: Mar 2009
Posts: 72
Rep Power: 8
dinonettis is on a distinguished road
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
dinonettis is offline   Reply With Quote

Old   May 14, 2008, 06:57
Default 1) contents of directory stead
  #30
Senior Member
 
mkraposhin's Avatar
 
Matvej Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 172
Rep Power: 8
mkraposhin is on a distinguished road
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)
mkraposhin is offline   Reply With Quote

Old   May 19, 2008, 01:17
Default Hi, I'm also facing a problem
  #31
New Member
 
Mohd Yousuf
Join Date: Mar 2009
Location: Kharagpur
Posts: 18
Rep Power: 8
yousuf is on a distinguished road
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
yousuf is offline   Reply With Quote

Old   May 19, 2008, 05:00
Default What BC's are you using? Also
  #32
Senior Member
 
mkraposhin's Avatar
 
Matvej Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 172
Rep Power: 8
mkraposhin is on a distinguished road
What BC's are you using?
Also, write about your relaxation factors and "div" descritisation schemes
mkraposhin is offline   Reply With Quote

Old   May 19, 2008, 05:27
Default wall1_periodic {
  #33
New Member
 
Mohd Yousuf
Join Date: Mar 2009
Location: Kharagpur
Posts: 18
Rep Power: 8
yousuf is on a distinguished road
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
yousuf is offline   Reply With Quote

Old   May 23, 2008, 22:22
Default mohd yousuf, is your case 3D
  #34
Senior Member
 
mkraposhin's Avatar
 
Matvej Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 172
Rep Power: 8
mkraposhin is on a distinguished road
mohd yousuf,
is your case 3D or 2D?
mkraposhin is offline   Reply With Quote

Old   May 25, 2008, 23:00
Default hi matj, Sorry for la
  #35
New Member
 
Mohd Yousuf
Join Date: Mar 2009
Location: Kharagpur
Posts: 18
Rep Power: 8
yousuf is on a distinguished road
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.
yousuf is offline   Reply With Quote

Old   May 26, 2008, 10:16
Default are you using tet-mesh, or hex
  #36
Senior Member
 
mkraposhin's Avatar
 
Matvej Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 172
Rep Power: 8
mkraposhin is on a distinguished road
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?
mkraposhin is offline   Reply With Quote

Old   May 27, 2008, 00:43
Default Hi Matvej, I'm using tetrah
  #37
New Member
 
Mohd Yousuf
Join Date: Mar 2009
Location: Kharagpur
Posts: 18
Rep Power: 8
yousuf is on a distinguished road
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 is offline   Reply With Quote

Old   May 27, 2008, 06:21
Default hey again, Matvej......I ha
  #38
New Member
 
Mohd Yousuf
Join Date: Mar 2009
Location: Kharagpur
Posts: 18
Rep Power: 8
yousuf is on a distinguished road
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
yousuf is offline   Reply With Quote

Old   May 28, 2008, 01:26
Default if epsilon is always bounded,
  #39
Senior Member
 
mkraposhin's Avatar
 
Matvej Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 172
Rep Power: 8
mkraposhin is on a distinguished road
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?
mkraposhin is offline   Reply With Quote

Old   May 28, 2008, 01:37
Default i'm using the same formula u m
  #40
New Member
 
Mohd Yousuf
Join Date: Mar 2009
Location: Kharagpur
Posts: 18
Rep Power: 8
yousuf is on a distinguished road
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
yousuf 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
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


All times are GMT -4. The time now is 18:23.