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

Low Mach Number for Combustion

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

Reply
 
LinkBack Thread Tools Display Modes
Old   January 18, 2011, 02:02
Default Low Mach Number for Combustion
  #1
Member
 
sahm's Avatar
 
S. Ali H.M.
Join Date: Nov 2009
Location: Chicago
Posts: 69
Rep Power: 7
sahm is on a distinguished road
Send a message via Yahoo to sahm
Hi everyone, Especially Foamers.
I want to know if anybody tried to simulate combustion using low mach number model in OpenFOAM. I would really appreciate if anybody can help as I have some problems.
Mostly the problem is with the pressures.
__________________
SAHM
sahm is offline   Reply With Quote

Old   January 18, 2011, 03:12
Default
  #2
Senior Member
 
Karl-Johan Nogenmyr
Join Date: Mar 2009
Location: Linköping
Posts: 252
Rep Power: 12
kalle is on a distinguished road
Hi!

I and a friend did some work on that starting from the reactingFoam solver in OF1.5. I do not have the solver ready right now, but I can upload if you want. Anyway, if you are using newer version of OF you are probably better off rewriting their reactingFoam solvers, as the thermodynamics implementation is different. All the neccessary info is available here:

http://web.student.chalmers.se/group...SlidesOFW5.pdf

If you use the XiFoam solver, I would guess that cancelling the dpdt term and implementing the pressure eq as above should work.

This is for constant pressure environment. If you are working with, for instance, piston engines, you need to rewrite.

/Kalle
kalle is offline   Reply With Quote

Old   January 18, 2011, 03:34
Default Thanksb
  #3
Member
 
sahm's Avatar
 
S. Ali H.M.
Join Date: Nov 2009
Location: Chicago
Posts: 69
Rep Power: 7
sahm is on a distinguished road
Send a message via Yahoo to sahm
Hi, thank for your link. I'll try to use that.
I`m working with OF1.7 and am trying to use reactingFoam and K-Epsilon Model. the thermophysical models are a little complicated, but I know what is the difference between the two codes.
I think the pressure equation should be the same, but let me see first. My application is constant pressure too.
Can I contact you later, if I have more questions?
__________________
SAHM
sahm is offline   Reply With Quote

Old   January 18, 2011, 08:53
Default
  #4
Senior Member
 
Karl-Johan Nogenmyr
Join Date: Mar 2009
Location: Linköping
Posts: 252
Rep Power: 12
kalle is on a distinguished road
Sure, of course. Good luck implementing!

K
kalle is offline   Reply With Quote

Old   January 19, 2011, 22:17
Default Detailed
  #5
Member
 
sahm's Avatar
 
S. Ali H.M.
Join Date: Nov 2009
Location: Chicago
Posts: 69
Rep Power: 7
sahm is on a distinguished road
Send a message via Yahoo to sahm
Hi Karl
Right now, I'm trying to use the equations from the paper below:
"Numerical Simulation of Low Mach Number Reactive Flows" Toboulides Et all.
Journal of scientific computing V12 N2 1997
The Equation set 1.1 in that paper, is very similar to what you have used in your project,
but my problem is with the pressure definition:
I can add two pressure terms in createFields.h to be used for dynamic pressure and hydrostatic ( thermodynamic ) pressure.
But in openfoam 1.7 there's class thermo that does all the definitions and calculations for pressure and rho, T, h .... I do not want to get into this class to change its source, do you have any idea how I can feed the pressure into it? I think if I change the pEqn file to calculate for dynamic pressure and try to fix the pressure in that class with my value, that should work.
another question: what is dpdt term?
SAHM.
__________________
SAHM
sahm is offline   Reply With Quote

Old   January 20, 2011, 03:46
Default
  #6
Senior Member
 
Karl-Johan Nogenmyr
Join Date: Mar 2009
Location: Linköping
Posts: 252
Rep Power: 12
kalle is on a distinguished road
Hi again,

I am not sure how things are done in 1.7, but what I did in 1.5 was to leave the p-field as it was, and initialize it with the global thermodynamic pressure. Then I introduced a new volScalarField, pd. That scalar I used as (dynamic) pressure in the momentum equation and in pEqn.H, the pressure correction.

The dpdt term is a source/sink term for enthalpy, which should be removed completely. If you keep it you will find pseudo pressure waves bouncing around in your domain.

Leaving the p field untouched, it will remain a constant uniform value throughout the simulation, and it will assist in calculating density. By this way you do not need to enter into the thermodynamics code.

Regards,
Kalle
kalle is offline   Reply With Quote

Old   January 20, 2011, 20:12
Default
  #7
Member
 
sahm's Avatar
 
S. Ali H.M.
Join Date: Nov 2009
Location: Chicago
Posts: 69
Rep Power: 7
sahm is on a distinguished road
Send a message via Yahoo to sahm
Hi
I totally omitted the dpdt term in all files, and had to do some changes for the fluxes, so that they use pHydro for pressure. Also I put a p=p_Operational Term in the code, to keep the p fixed. this one is feeding this pressure into termodynamics.
My question is do I have to change the compressibleCourantNo into CourantNo so that the code uses larger time steps ( DeltaT) or it does'nt change at all?
I`m trying what I said above to see what it will be like.
__________________
SAHM
sahm is offline   Reply With Quote

Old   January 21, 2011, 03:06
Default
  #8
Senior Member
 
Karl-Johan Nogenmyr
Join Date: Mar 2009
Location: Linköping
Posts: 252
Rep Power: 12
kalle is on a distinguished road
Hi!

Continue using the compressible version, as your flux, phi, is still including density.

In some sense, one would like the compressibleCoNo to be based on sound speed to correctly capture the evolution of pressure waves... this is however not the case in OF.

Regards,
Kalle
kalle is offline   Reply With Quote

Old   January 28, 2011, 02:59
Default
  #9
Member
 
sahm's Avatar
 
S. Ali H.M.
Join Date: Nov 2009
Location: Chicago
Posts: 69
Rep Power: 7
sahm is on a distinguished road
Send a message via Yahoo to sahm
Hi, Sorry for updating this thread late.
My Question is If I use compressible courant number, then how does openfoam calculate the time steps for the case, shouldn't the time steps be bigger?
__________________
SAHM
sahm is offline   Reply With Quote

Old   May 5, 2011, 08:12
Default
  #10
Senior Member
 
Karl-Johan Nogenmyr
Join Date: Mar 2009
Location: Linköping
Posts: 252
Rep Power: 12
kalle is on a distinguished road
Please let me correct myself. Some solvers in OF, like rhoCentralFoam, do determine the Co-number from wave speed rather than convective velocity. This is implemented in a solver-specific compressibleCourantNo.H.

Sorry for the misinfo.
K
kalle is offline   Reply With Quote

Old   October 11, 2013, 20:43
Default Pressure solver for low mach number solver
  #11
New Member
 
Join Date: Sep 2013
Posts: 8
Rep Power: 3
menonshyam is on a distinguished road
Hi All,

I have two questions following up on this low mach number solver thread:

I have changed the pressure equation to look as below to use the dynamic pressure "pd":

fvScalarMatrix pdEqn
(
fvc::ddt(psi, p)
+ fvc::div(phi)
- fvm::laplacian(rho*rUA, pd)
);

pdEqn.solve();

if (nonOrth == nNonOrthCorr)
{
phi += pdEqn.flux();
}
But if i start with a zero initial velocity field and impose a flame (density jump), it does not produce any velocity field nor any changes in dynamic pressure. On the other hand if i change the line "fvc::ddt(psi, p)" to "fvc::ddt(rho)", I do see a velocity field and changes in dynamic pressure. Does this mean that my "psi" implementation has something wrong with it? I do try to update the "psi" field to reflect changes in temperature due to the the flame.

The second question is after implementing "fvc::ddt(rho)", the solution diverges quickly and crashes. I have tried different pressure solvers (GAMG,PCG,ICCG) with and without pre-conditioners. Any ideas on getting this to run in a stable manner!?

Thanks in advance!
menonshyam 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
Exporting results and Mach number calculation pawan1989 CFX 0 July 14, 2010 13:05
Strong oscillation at transonic mach number martingariepy FLUENT 2 May 12, 2009 11:40
BlockMeshmergePatchPairs hjasak OpenFOAM Native Meshers: blockMesh 11 August 15, 2008 07:36
acoustics and low mach number George Main CFD Forum 42 November 3, 2005 07:05
compressible at low Mach number with uniteration ricklee Main CFD Forum 2 October 20, 2005 23:15


All times are GMT -4. The time now is 16:47.