I have a simple question for
I have a simple question for the board.
Which solver applies best for a turbulent, compressible and subsonic (0.4<M<1.0) flow? I have tried setting up a calculation using sonicTurbFoam, inspired by the prismtutorial, but when I go down in Machs, I find it hard to make succesful calculations. Thanks in advance. 
coodles the compressible LES
coodles the compressible LES solver works very well for unsteady 3D flows at all kinds of Mach numbers.

coodles, is that a new solver
coodles, is that a new solver included in the new openFoamversion? I am currently using foam2.3 from the old days.
Thanks for the help! 
Yes.
Yes.

I have now succesfully update
I have now succesfully updated my computers to OpenFOAM1.0.
I have found the coodlessolver, but I cannot find the configuration files for FoamX. Would it be possible to get the FoamX configurationfiles for coodles from you guys, in case you have them? Thanks again for all your help! 
Guess that one hasn't been do
Guess that one hasn't been done yet. Probably it takes the same setup (apart from boundary conditions) as oodles. Have a look at the oodles tutorial.
Mattijs 
But what should I do, if I on
But what should I do, if I only want a normal turbulence model together with an incompressible flow (Ma < 0.5) (like starcd with ideal gas)?

turbFoam = incompressible + t
turbFoam = incompressible + turbulence model.
Mattijs 
Sorry, I mean compressible wi
Sorry, I mean compressible with standard KEpsilon ;)

We have not written a basic c
We have not written a basic compressible turbulent flow solver because it has not been needed although this functinality does form the basis of all the combustion codes. If you take XiFoam for example and strip out all the combustion modelling you will end up with a basic compressible turbulent flow solver which should suit your needs. If you would like OpenCFD write one for you let us know and we can discuss a small contract to cover this application development and associated documentation and FoamX preprocessor support.

I am using rhoTurbFoam for an
I am using rhoTurbFoam for an exhaust manifold simulation on a high quality hex mesh. It appears to be running fine with Co<=0.3. Initialisation is from a reasonably converged simpleFoam simulation (with no problems of turbulence bounding). I've made some modifications to achieve an adaptive number of piso and nonorthogonal corrections at each timestep (I can share these modifications if people are interested).
I have some problems though that people may have some experience with: 1) After quite some time of steady timestep advancement, the enthalpy correction blows up and gives the following error... BICCG: Solving for h, Initial residual = 0.00719075, Final residual = 2.63587e05, No Iterations 1 > FOAM FATAL ERROR : Maximum number of iterations exceeded Function: specieThermo<thermo>::T(scalar f, scalar T0, scalar (specieThermo<thermo>::*F)(const scalar) const, scalar (specieThermo<thermo>::*dFdT)(const scalar) const) const in file: /home/dm2/henry/OpenFOAM/OpenFOAM1.1/src/thermophysicalModels/specie/lnInclude/ specieThermoI.H at line: 83. Although, it appears that the enthalpy equation has converged (shown above). The error is caused when it is exceeding the 100 iterations to obtain a temperature value. This problem persists even when turbulence is switched off. 2) Like with enthalpy, sometimes the k and epsilon fields need to be bounded after some time of well behaved timesteps (~1000 timesteps). bounding epsilon, min: 5.3484e+07 max: 5.80694e+10 average: 3.62477e+06 I am using the Gamma2 scheme for k and epsilon convection with a value of 1. Does anyone have any tips with this? Thanks for the help! 
Not sure about 1 but I can tel
Not sure about 1 but I can tell you about 2.
The problem with bounding means that your setup of differencing schemes may be problematic. The convection differencing is OK, even a bit too conservative  you should not need to use the factor greater than about 0.5. The problem may be in the laplacian  could you please try to run checkMesh and tell me what the nonorthogonality angles are. If they are bigish, try the laplacian scheme like this (for k and epsilon, and maybe for the enthalpy as well) laplacian(thingy,thingy) Gauss linear limited 0.5; This is interesting, please keep me posted (you can fiddle the last number, 0.7 or 1 should work as well), Hrv 
Hi Hrvoje,
I am currently r
Hi Hrvoje,
I am currently running a kEpsilon case with the changes to the laplacian scheme you suggest (k, epsilon and enthalpy). Will let you know of the result. As for the checkMesh nonorthogonality angles, some key measures are... Mesh nonorthogonality Max: 52.5196 average: 11.7172 Nonorthogonality check OK. Max skewness = 27.6894 percent. Face skewness OK. Minumum edge length = 0.000309256. Maximum edge length = 0.00480689. All angles in faces are convex or less than 10 degrees concave. Number of cells by type: hexahedra: 169024 Mesh OK. ...etc... 
Hrvoje,
I have tried differ
Hrvoje,
I have tried different variants of limited (0.333, 0.5, 0.7), corrected and uncorrected on the k, epsilon and enthalpy Laplacians. Bounding on both k and epsilon still occurs at various stages, then crashes due to enthalpy (temperature) exceeding maximum number of iterations. 
Hmm, I was afraid of that when
Hmm, I was afraid of that when I saw the max nonorthogonality angle  this really is a good mesh.
Sorry to waste your time, but I've got a couple more ideas to try:  if you are using partial convergence in the solver, try converging all the way  the final thing I do in such cases is to switch the convection discretisation to upwind. If there are still problems with bounding k and epsilon, this would indicate serious problems with the solver (or a nasty bug). If all that fails (this is now pretty conservative discretisation and foam is certainly able of doing better) and the geometry is not confidential (and below a million cells), I'd like to have a look at it. Sorry for the trouble, I am running out of easy ideas. Please let me know. Regards, Hrv 
Jarrod,
There may be some i
Jarrod,
There may be some issues with the JANAF thermodynamics/heattransfer due to some developments I made to the thermo library to handle complex boundary conditions. I am not sure if these problems might relate to your case failing but you could try using constant coefficient termodynamics and/or adiabatic walls. 
I have the same problems as Ja
I have the same problems as Jarrod,
I am trying to simulate a channel flow with constant wall heat flux. I cannot use adiabatic walls so what should I do? Should I use another solver? Daniele 
Constant wall heat flux is eqi
Constant wall heat flux is eqivalent to a fixed gradient boundary condition on energy/temperature.

Yes, I am using fixed gradient
Yes, I am using fixed gradient boundary condition on temperature and I get the same error message as Jarrod.
It is related to the boundary condition I am giving or something else? 
What OpenFOAM version are you
What OpenFOAM version are you running?
What solver? What thermodynamics package? Have you tried changing the gradient? Does it run if the gradient is small enough? Have you tried changing the sign of the gradient? 
All times are GMT 4. The time now is 04:55. 