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

Aeroacoustics with coodles

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

Reply
 
LinkBack Thread Tools Display Modes
Old   January 15, 2010, 04:59
Default Aeroacoustics with coodles
  #1
Member
 
Kapa Lilla
Join Date: Mar 2009
Location: Bruxelles, Belgium
Posts: 45
Rep Power: 8
klilla is on a distinguished road
Dear All,

I would like to open a thread dedicated for aeroacoustics, since such kind of problems is a bit different from general cfd. I saw some threads about it, but all were rather old ones, I hope still someone working on this direction.

Yesterday I already posted this, but I think on a wrong thread (it was about pre-processing as I later realized, sorry posting it twice, but I would like to bring my problem front of the right community).

So, I tried to simulate an acoustic pulse placed in the middle of a rectangular domain. The pulse should spread with the speed of sound unidirectionally. This happens well, BUT, in the density field there remains a smaller pulse constantly. This I do not understand, it seams that there and entropy pulse created, due to I do not know what.

My initial problem:

velocity is zero everywhere
gaussian pulse of pressure at the center of the domain (set by funkySet Field)
Op. 1: constant temperature, hoping that the "thermo" package will set the density well
Op. 2: set the density too as a gauss pressure rho = 1/(c*c)*p

Both initializations give back exactly the same results.

I normalized the pressure by pNorm = p/(c*c) +0.327 where the correction is exactly the same as the amplitude of the remaining pulse. In this case the density and normP plots are the same (except that in the density there is the extra bump )

have you any idea where I introduce this additional pulse?

Thanks,

Lilla
klilla is offline   Reply With Quote

Old   January 15, 2010, 06:35
Default
  #2
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 Lilla,
post some pictures of your calculations, it could be easier to help you with them. Moreover, put attention in normalizing variables in OF, as the solvers work with dimensional variables!
ivan_cozza is offline   Reply With Quote

Old   January 15, 2010, 10:05
Default
  #3
Member
 
Kapa Lilla
Join Date: Mar 2009
Location: Bruxelles, Belgium
Posts: 45
Rep Power: 8
klilla is on a distinguished road
Dear Ivan,

I used dimensional values.

p_0 = 10000Pa
U_0 = (0 0 0) - no background flow
T_0= 300K

and superimposed to them the pulse (maximum amplitude of 1 kg/m^3, ok this could be a bit high...), namely the pressure or the pressure and density.

Well, I would upload image, but when I click to the icon it is asking an url address and from there I'm lost.

So I created an album, it is in


well, here, if I write it:
http://www.cfd-online.com/Forums/mem...++coodles.html


Lilla
klilla is offline   Reply With Quote

Old   January 18, 2010, 01:07
Default
  #4
Senior Member
 
Fabian Braennstroem
Join Date: Mar 2009
Posts: 407
Rep Power: 10
braennstroem is on a distinguished road
Hi Lilla,

I wonder, how you set the gaussian pulse with funkySetFields... do you have a hint!?

Fabian
braennstroem is offline   Reply With Quote

Old   January 18, 2010, 05:57
Default gaussian pulse
  #5
Member
 
Kapa Lilla
Join Date: Mar 2009
Location: Bruxelles, Belgium
Posts: 45
Rep Power: 8
klilla is on a distinguished road
Like that:

expressions
(
benchP
{
field p;
expression "100000+0.1*340*340*exp(-log(2.)/9.*(pos().x*pos().x+pos().y*pos().y))";
}
/* benchR
{
field rho;
expression "1.163+exp(-log(2.)/9.*(pos().x*pos().x+pos().y*pos().y))";

//+0.1*exp(-log(2.)/25.*((pos().x-67.)*(pos().x-67.)+(pos().y-67.)*(pos().y-67.)))";
}
benchU
{
field U;
expression "U+vector(0.04*(pos().y-67.)*exp(-log(2.)/25.*((pos().x-67.)*(pos().x-67.)+(pos().y-67.)*(pos().y-67))),-0.04*(pos().x-67.)*exp(-log(2.)/25.*((pos().x-67.)*(pos().x-67.)+(pos().y-67.)*(pos().y-67.))), 0.0)";
}
*/
);

This is a benchmark problem from the ICASE/LaRC Workshop... from NASA (NASA CP-3300). Here an acoustic and a entropy/shear pulse are defined. I deleted the later one, so just the acoustic pulse remained. The adventage of the testcase, that it has analytical solution.

Lilla

Lilla
klilla is offline   Reply With Quote

Old   January 20, 2010, 06:44
Default localising the problem
  #6
Member
 
Kapa Lilla
Join Date: Mar 2009
Location: Bruxelles, Belgium
Posts: 45
Rep Power: 8
klilla is on a distinguished road
I found out where the simulation is going wrong, now I just do not know exactly why.

In the initialization we have due to the perfect gas law:

rhomax=pmax/(R*T)=1.2933, which should be equal in isentropic flow rho=c^2*p as c=sqrt(gamma/(R*T))=const as T =const., however in this way with gamma = 1.4 rhomax = 1.2586. So seems gamma do not fit.

The difference between the two remains in the computational domain as an entropy wave.

Unfortunatelly here a 3% of error is introduced which is not that much, I know, but in the present case more than annoying.

I do not know how to overcome this problem. Any suggestion is very wllcomed!

Lilla
klilla is offline   Reply With Quote

Old   January 20, 2010, 07:55
Default correction
  #7
Member
 
Kapa Lilla
Join Date: Mar 2009
Location: Bruxelles, Belgium
Posts: 45
Rep Power: 8
klilla is on a distinguished road
Sorry, I was a bit too fast:

p=rho0+c^2*(rho-rho0)

But the numbers are ok.
klilla is offline   Reply With Quote

Old   February 5, 2010, 04:26
Default
  #8
Member
 
Kapa Lilla
Join Date: Mar 2009
Location: Bruxelles, Belgium
Posts: 45
Rep Power: 8
klilla is on a distinguished road
Dear,

I realised my mistake, so to complete this tread:

The perturbations do not satisfy by themselves the perfect gas law, the instantaneous quantities do (like p=p0+p', etc.). So where I computed T'=m/R*p'/rho'=const. is not valid. Instead T=m/R*(p0+p')/(rho0+rho'). This is the closure of the initial value problem of an acoustic pulse.

Best regards,

Lilla
klilla is offline   Reply With Quote

Old   April 29, 2014, 08:49
Default
  #9
New Member
 
J.S.
Join Date: Jul 2012
Location: Germany
Posts: 4
Rep Power: 5
JS-UDE is on a distinguished road
Dear Lilla,

I know this is a quit old thread, but nevertheless thanks for opening it. I had implemented acoustic analogies in Openfoam and I wanted to verify my results by running the NASA Benchmark Test case. I have been successful in running my OF-case but now I stuck in generating/plotting the analytical solution to compare my numerical results with the exact one. Do you (or anybody else) have any helping hint? Do I have to solve the Integral of the analytical solution manually to get values along the x-axis for a specific time-step? Thanks a lot in advance?
JS
JS-UDE is offline   Reply With Quote

Old   April 29, 2014, 10:59
Default
  #10
Member
 
Kapa Lilla
Join Date: Mar 2009
Location: Bruxelles, Belgium
Posts: 45
Rep Power: 8
klilla is on a distinguished road
Hi,

yes, you need to integrate numerically (I've used matlab fort he pulse) to get the solution. There is not closed solution for such problems.
Best,
Lilla
klilla is offline   Reply With Quote

Old   April 29, 2014, 13:06
Default
  #11
New Member
 
J.S.
Join Date: Jul 2012
Location: Germany
Posts: 4
Rep Power: 5
JS-UDE is on a distinguished road
Hi Lilla,

thank you very much for your quick reply. And as I understand correctly, I was on the right path ;-). Hope the matlab-coding is not that much work... is the there a kind of usefull "hidden" function in Matlab/Octave for it?
Best regards,
Jan
JS-UDE is offline   Reply With Quote

Reply

Tags
acoustic, coodles

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
Nonphysical flow field while using coodles solver ankgupta8um OpenFOAM Running, Solving & CFD 5 January 26, 2008 17:54
Startingsetting coodles on an academic case melanie OpenFOAM Running, Solving & CFD 5 March 30, 2006 04:00
aeroacoustics Constantinos Main CFD Forum 1 March 22, 2004 14:32
Aeroacoustics - Flow over Cylinder Axel Rohde Main CFD Forum 2 August 17, 2002 12:18
aeroacoustics jonathan Main CFD Forum 2 February 4, 2002 09:14


All times are GMT -4. The time now is 20:36.