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

Turbulent compressible and subsonic gas flow

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

Reply
 
LinkBack Thread Tools Display Modes
Old   December 15, 2004, 11:47
Default I have a simple question for
  #1
Rasmus Gjesing (Gjesing)
Guest
 
Posts: n/a
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 prism-tutorial, but when I go down in Machs, I find it hard to make succesful calculations.

Thanks in advance.
  Reply With Quote

Old   December 16, 2004, 07:08
Default coodles the compressible LES
  #2
Eugene de Villiers (Eugene)
Guest
 
Posts: n/a
coodles the compressible LES solver works very well for unsteady 3D flows at all kinds of Mach numbers.
  Reply With Quote

Old   December 16, 2004, 08:51
Default coodles, is that a new solver
  #3
Rasmus Gjesing (Gjesing)
Guest
 
Posts: n/a
coodles, is that a new solver included in the new openFoam-version? I am currently using foam2.3 from the old days.

Thanks for the help!
  Reply With Quote

Old   December 16, 2004, 10:04
Default Yes.
  #4
Eugene de Villiers (Eugene)
Guest
 
Posts: n/a
Yes.
  Reply With Quote

Old   December 16, 2004, 12:35
Default I have now succesfully update
  #5
Rasmus Gjesing (Gjesing)
Guest
 
Posts: n/a
I have now succesfully updated my computers to OpenFOAM-1.0.

I have found the coodles-solver, but I cannot find the configuration files for FoamX.

Would it be possible to get the FoamX configuration-files for coodles from you guys, in case you have them?

Thanks again for all your help!
  Reply With Quote

Old   December 16, 2004, 12:42
Default Guess that one hasn't been do
  #6
Mattijs Janssens (Mattijs)
Guest
 
Posts: n/a
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
  Reply With Quote

Old   December 20, 2004, 14:34
Default But what should I do, if I on
  #7
Joern Beilke (Beilke)
Guest
 
Posts: n/a
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)?
  Reply With Quote

Old   December 20, 2004, 14:45
Default turbFoam = incompressible + t
  #8
Mattijs Janssens (Mattijs)
Guest
 
Posts: n/a
turbFoam = incompressible + turbulence model.

Mattijs
  Reply With Quote

Old   December 20, 2004, 16:11
Default Sorry, I mean compressible wi
  #9
Joern Beilke (Beilke)
Guest
 
Posts: n/a
Sorry, I mean compressible with standard KEpsilon ;-)
  Reply With Quote

Old   December 21, 2004, 18:36
Default We have not written a basic c
  #10
Henry Weller (Henry)
Guest
 
Posts: n/a
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.
  Reply With Quote

Old   March 16, 2005, 21:01
Default I am using rhoTurbFoam for an
  #11
New Member
 
Jarrod Sinclair
Join Date: Mar 2009
Posts: 6
Rep Power: 8
sinclair is on a distinguished road
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 non-orthogonal 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 = 2.63587e-05, 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/OpenFOAM-1.1/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!
sinclair is offline   Reply With Quote

Old   March 17, 2005, 04:11
Default Not sure about 1 but I can tel
  #12
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,758
Rep Power: 21
hjasak will become famous soon enough
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 non-orthogonality angles are. If they are big-ish, 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
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   March 17, 2005, 08:56
Default Hi Hrvoje, I am currently r
  #13
New Member
 
Jarrod Sinclair
Join Date: Mar 2009
Posts: 6
Rep Power: 8
sinclair is on a distinguished road
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 non-orthogonality angles, some key measures are...

Mesh non-orthogonality Max: 52.5196 average: 11.7172
Non-orthogonality 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...
sinclair is offline   Reply With Quote

Old   March 18, 2005, 02:49
Default Hrvoje, I have tried differ
  #14
New Member
 
Jarrod Sinclair
Join Date: Mar 2009
Posts: 6
Rep Power: 8
sinclair is on a distinguished road
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.
sinclair is offline   Reply With Quote

Old   March 18, 2005, 03:41
Default Hmm, I was afraid of that when
  #15
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,758
Rep Power: 21
hjasak will become famous soon enough
Hmm, I was afraid of that when I saw the max non-orthogonality 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
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   March 18, 2005, 04:40
Default Jarrod, There may be some i
  #16
Senior Member
 
Join Date: Mar 2009
Posts: 854
Rep Power: 13
henry is on a distinguished road
Jarrod,

There may be some issues with the JANAF thermodynamics/heat-transfer 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.
henry is offline   Reply With Quote

Old   April 21, 2005, 07:11
Default I have the same problems as Ja
  #17
Senior Member
 
Daniele Panara
Join Date: Mar 2009
Posts: 101
Rep Power: 8
panara is on a distinguished road
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
panara is offline   Reply With Quote

Old   April 21, 2005, 07:15
Default Constant wall heat flux is eqi
  #18
Senior Member
 
Join Date: Mar 2009
Posts: 854
Rep Power: 13
henry is on a distinguished road
Constant wall heat flux is eqivalent to a fixed gradient boundary condition on energy/temperature.
henry is offline   Reply With Quote

Old   April 21, 2005, 07:19
Default Yes, I am using fixed gradient
  #19
Senior Member
 
Daniele Panara
Join Date: Mar 2009
Posts: 101
Rep Power: 8
panara is on a distinguished road
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?
panara is offline   Reply With Quote

Old   April 21, 2005, 07:26
Default What OpenFOAM version are you
  #20
Senior Member
 
Join Date: Mar 2009
Posts: 854
Rep Power: 13
henry is on a distinguished road
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?
henry 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
Compressible Turbulent Flow CFDtoy Main CFD Forum 5 January 19, 2005 05:41
bench mark for subsonic compressible turbulent fl javadi Main CFD Forum 0 June 14, 2004 08:40
need tubulence compressible subsonic benchmark javadi Main CFD Forum 1 June 14, 2004 08:36
compressible subsonic flow Joel CD-adapco 2 April 24, 2003 08:18
Compressible turbulent flow FVS Main CFD Forum 0 April 13, 2002 17:07


All times are GMT -4. The time now is 22:31.