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

Missing separation

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

Reply
 
LinkBack Thread Tools Display Modes
Old   July 31, 2009, 05:19
Default Missing separation
  #1
New Member
 
Marcin Hinz
Join Date: May 2009
Location: Monheim am Rhein, Germany
Posts: 24
Rep Power: 8
Marcin is on a distinguished road
Hi All,

I try to simulate and compare the results in OF and CFX of blades in a gas turbine. The problem is, I don't get separation in OF in a rotor blade on the pressure side. This occurs in CFX and as the experience of my company shows it is the right solution. Of course I use the same meshes and I hope I use the same alignments in both codes. Any ideas what coul'd be the reason for this?

Best regards,

Marcin

Last edited by Marcin; August 6, 2009 at 07:14.
Marcin is offline   Reply With Quote

Old   August 4, 2009, 10:07
Default
  #2
Member
 
Join Date: Jun 2009
Posts: 36
Rep Power: 8
dipling is on a distinguished road
I think one reason is that nobody can really reconstruct your exact problem. Your description is..let me say "short"
dipling is offline   Reply With Quote

Old   August 6, 2009, 05:45
Default
  #3
New Member
 
Marcin Hinz
Join Date: May 2009
Location: Monheim am Rhein, Germany
Posts: 24
Rep Power: 8
Marcin is on a distinguished road
Yes well, I just tought there is a magic button 'turn the separation on'

I'm not quite sure what I should write over here to make it entire and undersandable, but I try to do my best.

Like I sad it is a simulation of a rotor blade of a gas turbine. (By the way, the next step of my work is to test the GGI or mixing-planes. Does anybody have some expierence with these interfaces in steam or gas turbines?) The mesh was made with Turbogrid and imported over Icem using .msh to Foam. I have tried different meshes of the same geometry with a nuber of elemenst between 90000 and 350000. In all cases checkMesh sad mesh ok. The yPlus values are between 30 and 180 on average in depend of the grid.

The boudary conditions are total pressure and total or static temperature at inlet and a static pressure at outlet. The Mach number computated with these boudaries equals about 0.95. I have used k-epsilon and SST turbulence models (I have made a special mesh for the SST model with smaller yPlus values). Medium of my simulation is air pureMixture with constTransport. All the thermophysical values have been took out of thermodynamics tabels.

Because of the fact that there is no compressible solver to simulate rotor blades I made a new one by oneself. I took the rhoSimpleFoam, added the SRFModel and made small changes in the equations.

The schemes I simulate with are:


ddtSchemes
{
default steadyState;
}
gradSchemes
{
default Gauss linear;
grad(p) Gauss linear;
}
divSchemes
{
default none;
div(phi,U) Gauss upwind;
div(phid,p) Gauss linearUpwind;
div(phiU,p) Gauss linearUpwind;
div(phi,h) Gauss upwind;
div(phi,k) Gauss upwind;
div(phi,epsilon) Gauss upwind;
div(phi,R) Gauss linearUpwind;
div(phi,omega) Gauss linearUpwind;
div((rho*R)) Gauss linearUpwind;
div(R) Gauss linearUpwind;
div(U) Gauss linearUpwind;
div((muEff*dev2(grad(U).T()))) Gauss linear;
div(phi,(0.5*magSqr(Usrf))) Gauss upwind;
div(phi,(0.5*magSqr(U))) Gauss upwind;
}
laplacianSchemes
{
default none;
laplacian(muEff,U) Gauss linear corrected;
laplacian(mut,U) Gauss linear corrected;
laplacian(DkEff,k) Gauss linear corrected;
laplacian(DepsilonEff,epsilon) Gauss linear corrected;
laplacian(DREff,R) Gauss linear corrected;
laplacian(DomegaEff,omega) Gauss linear corrected;
laplacian((rho|A(U)),p) Gauss linear corrected;
laplacian(alphaEff,h) Gauss linear corrected;
}
interpolationSchemes
{
default linear;
}
snGradSchemes
{
default corrected;
}



As and when required I will paste also my solution file. I will also try to paste today some screenshots of my geometry. Of course I'm happy to answer any other questions about my case.

Thank you in advance for any reply,

Marcin

Last edited by Marcin; August 6, 2009 at 07:14.
Marcin is offline   Reply With Quote

Old   August 17, 2009, 02:37
Default
  #4
Senior Member
 
Henrik Rusche
Join Date: Mar 2009
Location: Braunschweig, Niedersachsen, Germany
Posts: 275
Rep Power: 9
henrik is on a distinguished road
Marcin,

I have a few questions/guesses for you:

Since the solver is new - did you validate it on something simple?

I think CFX has special compressible wall boundary conditions - Are you sure that you are running the same wall boundary conditions?

Henrik
henrik is offline   Reply With Quote

Old   August 19, 2009, 08:52
Default Check the schemes
  #5
New Member
 
Oscar
Join Date: Jun 2009
Location: Murcia, Spain
Posts: 14
Rep Power: 8
Zowie is on a distinguished road
If you are using CFX, probably your divergence scheme is High Resolution (or maybe a specified blend factor), am I right? In OpenFOAM you are using first order upwind... well, following my experience, this has an important effect on the solution.

Try to use Gamma or limited linear for OpenFoam or maybe upwind for CFX and compare again... maybe it helps a little bit.
Zowie is offline   Reply With Quote

Old   August 19, 2009, 10:43
Default
  #6
Administrator
 
jola's Avatar
 
Jonas Larsson
Join Date: Jan 2009
Location: Gothenburg, Sweden
Posts: 162
Rep Power: 10
jola is on a distinguished road
Send a message via MSN to jola Send a message via Skype™ to jola
My experience is that CFX with their default SST k-omega model using resolved walls is one of the most separation sensitive models available (among commercial eddy-viscosity based solvers). Sometimes this is good, but often it will give you overly conservative designs. What turbulence model and what kind of wall treatment are you using?
jola is offline   Reply With Quote

Old   August 25, 2009, 03:46
Default
  #7
New Member
 
Marcin Hinz
Join Date: May 2009
Location: Monheim am Rhein, Germany
Posts: 24
Rep Power: 8
Marcin is on a distinguished road
Hello,

first to all I would like to thank you all for replies. It took some time to check and validate ones more my test cases.

The problem was, that one force therme was lost as I derived the energy equation with the total enthalpy. After I found it I have started some simulations once more and got quite good results. However the situation of both codes has changed

OpenFOAM shows little bit wider separation and wake than CFX. I suppose that it is the couse of different wall functions in both codes. Another reason for it could be the Mach number, which is greater than 1. Could it?

Like I sad the results are not bad. When I compare the results with ParaView there are only small differences in the outlines of some quantities and when I plot the results over different lines.
Also by patch averaged values there are diffrences of 1 - 3 %. The only big difference at the outflow is the Mach number with 12 %.

Just to anwser your questions ...

henrik CFX uses compressible wall boundary conditions only for Mach numbers greater than 3, so this couldn't be the reason for this

Zowie I was using the same (upwind) schemes in both codes

jola I have used and comared k-epsilon and SST models in both codes. You can see the results above. I must admit, I don't know how I can compare the wall treatment of OF and CFX. Where can I check it?

Best Regards
Marcin is offline   Reply With Quote

Old   September 30, 2009, 07:09
Default
  #8
Senior Member
 
Ivan Flaminio Cozza
Join Date: Mar 2009
Location: Torino, Piemonte, Italia
Posts: 207
Rep Power: 9
ivan_cozza is on a distinguished road
Send a message via MSN to ivan_cozza
Hi Foamers,
I'm facing a similar problem. I'm solving a steady state turbine blade with simpleFoam, as the max Mach in the domain is 0.3. My turbulence model is k-Omega SST, with full resolved walls (y+ less than one in the whole domain), and fixedValue 1e-12 bc for k.
Schemes for div are all limitedLinear.
The AoA is 0, at this AoA there must be a separation in the pressure side, but my results are an attached flow.
Someone have any experience on simpleFoam behavior with separation bubble? Could it be a problem with the turbulence model?
Thanks!
ivan_cozza 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
separation Dougal Main CFD Forum 2 November 8, 2007 03:27
Separation Point over a NACA 0012 Franny Main CFD Forum 3 March 22, 2007 15:49
Separation prediction over a 2d cylinder.... Kyle FLUENT 2 December 9, 2005 05:17
Separation An Modh Coinniolach FLUENT 4 April 1, 2002 11:31
Euler + separation again Oliver Main CFD Forum 23 June 19, 2001 12:47


All times are GMT -4. The time now is 17:23.