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

Pressure waves bouncing around in the domain

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

Reply
 
LinkBack Thread Tools Display Modes
Old   October 14, 2010, 13:42
Default Pressure waves bouncing around in the domain
  #1
Senior Member
 
Nilesh Rane
Join Date: Apr 2010
Posts: 122
Rep Power: 7
nileshjrane is on a distinguished road
Hi folks,

I am trying to solve mixing of air and fuel jets in a combustor. PFA the case dict.

When i solve the case with rhoPisoFoam, the case diverges after some time. but till that time, when opened in paraview, i noticed that pressure wave is stating from inlet and it goes on reflection from walls and the inlets and outlets. The wave keeps moving in the domain. I searched on the forum for such problem. i couldn't find the solution for this. I have never done much of subsonic compressible simulations and i never saw such issue before.

I tried changing numerical schemes and relax. factors. but all in vein.

Anyone has any solution any info for this??
Attached Files
File Type: gz test_dict_2.tar.gz (4.2 KB, 3 views)
__________________
Imagination is more important than knowledge..
nileshjrane is offline   Reply With Quote

Old   October 14, 2010, 14:26
Default
  #2
Senior Member
 
Nilesh Rane
Join Date: Apr 2010
Posts: 122
Rep Power: 7
nileshjrane is on a distinguished road
some more info:

The solution always end with same error:

Quote:
--> FOAM FATAL ERROR:
Maximum number of iterations exceeded

From 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/opencfd/OpenFOAM/OpenFOAM-1.7.0/src/thermophysicalModels/specie/lnInclude/specieThermoI.H at line 67.

FOAM aborting

#0 Foam::error:rintStack(Foam::Ostream&) in "/opt/openfoam170/lib/linux64GccDPOpt/libOpenFOAM.so"
#1 Foam::error::abort() in "/opt/openfoam170/lib/linux64GccDPOpt/libOpenFOAM.so"
#2 Foam::hPsiThermo<Foam:ureMixture<Foam::constTran sport<Foam::specieThermo<Foam::hConstThermo<Foam:: perfectGas> > > > >::calculate() in "/opt/openfoam170/lib/linux64GccDPOpt/libbasicThermophysicalModels.so"
#3 Foam::hPsiThermo<Foam:ureMixture<Foam::constTran sport<Foam::specieThermo<Foam::hConstThermo<Foam:: perfectGas> > > > >::correct() in "/opt/openfoam170/lib/linux64GccDPOpt/libbasicThermophysicalModels.so"
#4
in "/opt/openfoam170/applications/bin/linux64GccDPOpt/rhoPisoFoam"
#5 __libc_start_main in "/lib/libc.so.6"
#6
in "/opt/openfoam170/applications/bin/linux64GccDPOpt/rhoPisoFoam"
Aborted
This happens sooner or later depending on the change in BC. I think i might get correct solution if i can make it to run for long enough. But i just can't.
__________________
Imagination is more important than knowledge..
nileshjrane is offline   Reply With Quote

Old   October 15, 2010, 00:29
Default
  #3
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,894
Rep Power: 26
alberto will become famous soon enoughalberto will become famous soon enough
Mach number?
__________________
Alberto Passalacqua

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as live DVD/USB, hard drive image and virtual image.
OpenQBMM - An open-source implementation of quadrature-based moment methods
alberto is offline   Reply With Quote

Old   October 15, 2010, 02:49
Default
  #4
Senior Member
 
Nilesh Rane
Join Date: Apr 2010
Posts: 122
Rep Power: 7
nileshjrane is on a distinguished road
Hi Alberto,

The mach number is 0.3 at air inlet (the pipe attaching from side) and 1 at fuel stream (chocked nozzle).

I suspect the pressures are not appropriate. (the values i have got are from my counter parts who r designing other components. Its a ducted rocket basically). As after doing some runs i saw that the air stream actually goes supersonic and a normal shock is forming. But as the shock tries to go out of the air inlet pipe the solution blows. PFA the pic of the last time step where it diverges.

Somewhere on the forum someone suggested that one can modify the max number of iterations for the solver in "/home/opencfd/OpenFOAM/OpenFOAM-1.7.0/src/thermophysicalModels/specie/lnInclude/specieThermoI.H", but i didn't like the idea as i suppose the physics need some check. I tried many things but numerics seem fine as it does make much difference. So i am currently trying with pressure BC.
Attached Images
File Type: jpg normalshk.jpg (96.8 KB, 55 views)
__________________
Imagination is more important than knowledge..
nileshjrane is offline   Reply With Quote

Old   October 17, 2010, 16:44
Default
  #5
Senior Member
 
Nilesh Rane
Join Date: Apr 2010
Posts: 122
Rep Power: 7
nileshjrane is on a distinguished road
updates:

I figured out that the pressure BC are unrealistic. There is huge pressure jump at inlets and thus flow goes supersonic. And a normal shock is the ultimate fate.

So i reduced the pressure jump to zero with many intermediate permutations. Now i am using these pressure BCs:

Air inlet : 2358000Pa
Fuel inlet: 2400000Pa
Outlet: 2358000Pa
Initialisation of P: 2358000Pa

Now this is very much physical situation. But still i am getting tha pressure wave moving back and forth like a shock in a shock tube. and my solution meets same fate as i said in earlier posts sooner or later.

I think zeroGradient BC is prone to pressure wave relections ,please correct me if m wrong. So i tried with fixedValue or waveTransmissive BC as well but all in vein..


My problem is similar to this one: Pressure instability with rhoSimpleFoam
__________________
Imagination is more important than knowledge..

Last edited by nileshjrane; October 17, 2010 at 17:11.
nileshjrane is offline   Reply With Quote

Old   October 18, 2010, 03:47
Default
  #6
Senior Member
 
Christian Lucas
Join Date: Aug 2009
Location: Braunschweig, Germany
Posts: 198
Rep Power: 7
Chris Lucas is on a distinguished road
Hi,

at this high velocities, you should modify the solver a little bit. First of all, are you using the transonic setting for the pressure equation? Otherwise, the pressure equation is (more or less) for an incompressible flow (at least this is what I think). Secondly, a might want to implement a total energy equation instead of the thermal energy equation used in rhoPisoFoam.

Solving the total energy equation

About the reflection outlet BC, there is no simple solution so far. You could program a new non reflection BC (would be great ). The Other possibility might be to place the outlet BC far away from the area of interest. This away, the dissipation might dissipate all pressure waves in the system (at least it helped me).

Regards,
Christian





Chris Lucas is offline   Reply With Quote

Old   October 21, 2010, 09:20
Default
  #7
Senior Member
 
Nilesh Rane
Join Date: Apr 2010
Posts: 122
Rep Power: 7
nileshjrane is on a distinguished road
Thanx for reply Chris,

I am surprized to know that rhoPisoFoam does not solve energy equation. I never thought about it.

I have got only 3weeks to finish the simulations and its not possible to modify anything in the solver for me now. I have never used c++ before, neither i have enough knowledge of numerical schemes i feel.

I am thinking of writing a density based solver after this task is over.
__________________
Imagination is more important than knowledge..
nileshjrane is offline   Reply With Quote

Old   October 21, 2010, 09:27
Default
  #8
Senior Member
 
Christian Lucas
Join Date: Aug 2009
Location: Braunschweig, Germany
Posts: 198
Rep Power: 7
Chris Lucas is on a distinguished road
Hi,

either I misunderstand you or you misunderstood me. rhoPisoFoam solves the thermal energy equation, which is fine for low speed flows. The total energy equation is more correct for high speed flows (link above).

About the transonic setting. Add "transonic true" in the fvSolution file under Piso.

Use low Co numbers. The BC should be far away from the area of interest.
Use limitedLinear Schemes for div. at least this works for me.


Regards,
Christian
Chris Lucas is offline   Reply With Quote

Old   October 21, 2010, 10:41
Default
  #9
Senior Member
 
Nilesh Rane
Join Date: Apr 2010
Posts: 122
Rep Power: 7
nileshjrane is on a distinguished road
I made a boo boo..Sorry..i missed "total" word before energy equation. it should have been total energy equation rather than just energy equation. Sorry, my bad.
__________________
Imagination is more important than knowledge..
nileshjrane is offline   Reply With Quote

Old   October 21, 2010, 11:19
Default
  #10
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,894
Rep Power: 26
alberto will become famous soon enoughalberto will become famous soon enough
Have you ever considered rhoCentralFoam?
__________________
Alberto Passalacqua

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as live DVD/USB, hard drive image and virtual image.
OpenQBMM - An open-source implementation of quadrature-based moment methods
alberto is offline   Reply With Quote

Old   October 21, 2010, 12:27
Default
  #11
Senior Member
 
Nilesh Rane
Join Date: Apr 2010
Posts: 122
Rep Power: 7
nileshjrane is on a distinguished road
Hello Alberto,

I did have a look at all the available solvers. rhoCentralFoam isn't meant for turbulent flows thats the problem. But it does solve total energy (rhoE) i suppose rather than enthalpy (h).
__________________
Imagination is more important than knowledge..
nileshjrane is offline   Reply With Quote

Old   October 21, 2010, 14:43
Default
  #12
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,894
Rep Power: 26
alberto will become famous soon enoughalberto will become famous soon enough
Well, if that's the solver that works in your case, adding turbulence means coding a bit... Probably better than trying to make a solver work at the limit of its capabilities.
__________________
Alberto Passalacqua

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as live DVD/USB, hard drive image and virtual image.
OpenQBMM - An open-source implementation of quadrature-based moment methods
alberto 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
Fluent natural ventilation pressure boundary condition pierresandre FLUENT 24 November 8, 2011 15:32
RPM in Wind Turbine Pankaj CFX 9 November 23, 2009 05:05
CFX Solver Memory Error mike CFX 1 March 19, 2008 08:22
How to apply negtive pressure to outlet bioman66 CFX 5 June 3, 2006 01:40
pressure waves Antonio Main CFD Forum 3 February 17, 2006 21:53


All times are GMT -4. The time now is 10:34.