
[Sponsors] 
February 25, 2013, 19:21 
decay 2d turbulence  the initial field

#1 
New Member

I've seen some videos that demonstrates the process of 2d turbulence decay. Here are some of them:
http://www.youtube.com/watch?v=boWeyfYs2EQ http://www.youtube.com/watch?v=pNCst5zPEQ http://www.youtube.com/watch?v=fDwnyi_EkM I want to simulate this process by using the Euler system of equations. For this goal, I must have the initial field (rho, u, w, p). Does anyone give me some ideas about this? Thanks for helping! 

February 26, 2013, 04:45 

#2  
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 1,645
Rep Power: 23 
Quote:
just to say that if you use the inviscid flow equation, you have no decay due to dissipation. Furthermore, in 2D you can have some inverse cascade as well as you can see small vortical structures forming bigger ones (e.g., the vortex merging) 

February 26, 2013, 05:12 

#3 
New Member

Can you give me the link to that book you sad?
I know that there is no decay due to physical dissipation in inviscid flow, but it's impossible to neglect the grid viscosity which is meshdependent factor. I don't know what kind of the final field will be, I'm interested in generating the initial field to initialize the test case. Thanks for replying! 

February 26, 2013, 05:22 

#4 
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 1,645
Rep Power: 23 

February 26, 2013, 06:29 

#5 
New Member

OK, that book explains the theory of turbulence very good and fully. But I still need particular specifically formulas for generating the initial field to initialize a simulation case. In the book I can't find out them.


February 26, 2013, 06:34 

#6 
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 1,645
Rep Power: 23 
see also:
http://onlinelibrary.wiley.com/doi/1...d.613/abstract in the references you will find a paper of Lesiuer describing the details 

February 26, 2013, 06:57 

#7 
New Member

Can you tell the name of Lesiuer's paper describing the details of turbulence initial field for numerical simulations?
I couldn't download the journal. 

February 26, 2013, 07:05 

#8 
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 1,645
Rep Power: 23 
Lesieur, M. Staquet C, Le Roy P, Comte P. The mixing layer and its coherence examined from the point of
view of twodimensional turbulence. Journal of Fluid Mechanics 1986; 192:511–534. you cna find the case of the initialization for a 2D micing layer 

February 26, 2013, 07:59 

#9 
New Member

Do you know that I don't need an initial field for 2D shear layer. I need an initial field for the exactly given above examples: decay of 2D turbulence flow with vortices. I've found out some articles, which describe the initial field for some different kind of Euler equations. They used the vortexvelocity transport equations to solve the problem. With that kind of Euler equations it's possible to define the exact field for all the vortices. I use the Euler equations in FV method to solve the problem, I need the initial state for all components of the velocity. This is my problem!
Thanks for helping! 

February 26, 2013, 09:14 

#10  
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 1,645
Rep Power: 23 
Quote:
if you want to simulate only the homogeneous/isotropic decay, you can simply work in the x,y plane by using the initial 1D distribution (extended in the homogeneous 2D meaning and adjusting the coefficients to satisfy the continuity contraint) described here: On the application of congruent upwind discretizations for large eddy simulations Authors Andrea Aprovitola, Filippo Maria Denaro Publication date 2004/2/10 Journal name Journal of Computational Physics Volume 194 Issue 1 Pages 329343 Publisher Academic Press 

February 26, 2013, 17:25 

#11 
New Member

I want to solve the problem in the x,y plane, with the limited space [LxL] and periodic boundary conditions. I need the initial with vorticies like in the above videos. But I can't find out some formulas for this purpose. I've read the article you sad, but it didn't help me.
I think that in the videos, the vortexvelocity form of the Euler equations was used. It's possible to give the exact values of vorticies at the cell centers. I use the FV approach to solve the the Euler system of equations. It's no need to have a vorticity field at the beginning time. But I need the beginning values for the velocity components. I have read many works, but I can't find out some of them helpful for me! 

May 7, 2013, 00:39 

#12 
New Member
Angus Hutchison
Join Date: May 2013
Posts: 6
Rep Power: 4 
@mp121209 did you have any luck with your simulation?


May 7, 2013, 10:36 

#13 
Member
Reza
Join Date: Mar 2009
Location: Appleton, WI
Posts: 99
Rep Power: 8 
I don't know if you are still interested in this or not, but you can find an initial velocity field for homogenous turbulence in the following paper:
Numerical Experiments in Homogeneous Turbulence, by Robert S. Rogallo It is a very old NASA report and a very good reference for DNS codes, so it is available on many sites. Just google the title and you should be able to get it. I can't remember which page :p but it was near the end of the paper. It uses Fourier transform though, so you should be prepared to take inverse FFT of a spectral distribution, just a heads up :) Good luck. 

October 16, 2013, 07:45 

#14 
New Member
Dhruv Mehta
Join Date: Jun 2012
Posts: 22
Rep Power: 5 
Hello
Thank you for the information on Rogallo's code. I would be thankful if you could tell me how can I modify the code to generate a 2D field instead of the 3D field that the code is supposed to generate. Thank you ! 

October 16, 2013, 09:53 

#15 
Member
Reza
Join Date: Mar 2009
Location: Appleton, WI
Posts: 99
Rep Power: 8 
Why twodimensional? Turbulence is intrinsically threedimensional.
Anyhow, if you want a 2D initial field, you can either generate a 3D field and apply any averaging operator on the third dimension, or just generate the 2D spectral distribution first (Rogallo's distribution makes sure, for example, continuity is satisfied, so when modifying the equations, do not just remove the third component. You'll probably need to change the remaining two components as well) and then perform a twodimensional IFFT. It has been very long since last I saw that paper. Let us know if you have any specific problems converting it to 2D and I might be able to help. At the end, again, I have to emphasize the inherent threedimensionality of turbulence. 

October 16, 2013, 10:18 

#16 
New Member
Dhruv Mehta
Join Date: Jun 2012
Posts: 22
Rep Power: 5 
Thank you for your response.
I agree that turbulence is 3D in nature. However, there are few numerical tests conducted on the decay of 2D turbulence. I just wanted to verify a 2D code and thus required the field. I will try what you suggested and would let you know in case it works. Thank you again for your prompt response. Best ! 

October 18, 2013, 09:47 

#17 
New Member
Dhruv Mehta
Join Date: Jun 2012
Posts: 22
Rep Power: 5 
Hello Reza
I modified the code to generate a 2D field that satisfies the continuity equation in wavenumber space, i.e. kx*ux + ky*uy = 0; The field is indeed isotropic and divergence free (to machine precision, set to 108) in this case. However, on taking the inverse FFT of this field, the physical fields that results is not divergence free at all. I am making a mistake in using the inverse FFT (I use MATLAB's iffn(symmetric) ). I would be thankful if you could help me with this. To generate the 2D field I used: u = a*ky*(1/k) i  a*kx*(1/k) j where, sqrt( kx^2 + ky^2 ) = k, i and j are the x and y unit vectors, u here is defined in wavenumber space. This definition of u satisfies continuity as ux/uy = ky/kx. Also, a is a function of the desired energy spectrum as used by Rogallo. I use a = ( E(k) / 2*pi*k)^(0.5) * e^(iota*phi) Thank you. Regards Dhruv 

October 18, 2013, 10:07 

#18 
Member
Reza
Join Date: Mar 2009
Location: Appleton, WI
Posts: 99
Rep Power: 8 
Hi,
Multidimensional IFFT can be a real headache sometimes, specially when you are generating values in frequency domain and you are hoping to get a realvalued function in physical space. I'm not familiar with MATLAB's ifftn function, so I'll take a look at that as soon as a license becomes available for me to use :) However, by then, are you taking care of the wraparound? Also, if you have to give MATLAB the whole spectral response, you need to make sure it satisfies the symmetry rules to guarantee a real function in the physical domain. These symmetries mainly come from the fact that: where is the Fourier transform of and is the conjugate of a complex number . Because of this symmetry and wraparound, some on the values have to be real, for example: and you can get some specific relations for where and are equal to , where is the size of the grid that you are using. Last edited by triple_r; October 18, 2013 at 10:08. Reason: LATEX Error 

October 18, 2013, 10:17 

#19 
New Member
Dhruv Mehta
Join Date: Jun 2012
Posts: 22
Rep Power: 5 
Hello
Thank you for the explanation. As advised, I will go through some notes on FFT. Regards 

October 18, 2013, 10:44 

#20 
Member
Reza
Join Date: Mar 2009
Location: Appleton, WI
Posts: 99
Rep Power: 8 
Yeah, as I mentioned, you need to make sure the frequencydomain field that you are generating is as MATLAB describes it "conjugate symmetric". Here is an octave code that I was able to dig from my archives that makes sure the field is symmetric:
Code:
for i = 1:M for j = 2:N/2 E(i, j) = temp(i, j); E(mod(Mi+1, M)+1, mod(Nj+1, N)+1) = conj(temp(i, j)); end end for i = 2:M/2 E(i, 1) = temp(i, 1); E(mod(Mi+1, M)+1, 1) = conj(temp(i, 1)); end for i = 2:M/2 E(i, N/2+1) = temp(i, N/2+1); E(mod(Mi+1, M)+1, N/2+1) = conj(temp(i, N/2+1)); end E(1,1) = real(temp(1,1)); E(M/2+1,1) = real(temp(M/2+1,1)); E(1,N/2+1) = real(temp(1,N/2+1)); E(M/2+1,N/2+1) = real(temp(M/2+1,N/2+1)); Hope this helps. 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
pisoFoam  unstable pressure residual  Industrial_CFD  OpenFOAM Running, Solving & CFD  21  February 24, 2013 16:39 
problem with Min/max rho  tH3f0rC3  OpenFOAM  7  February 23, 2013 06:37 
Error while running rhoPisoFoam..  nileshjrane  OpenFOAM Running, Solving & CFD  8  August 26, 2010 12:50 
lift and drag on ship superstructures  vaina74  OpenFOAM Running, Solving & CFD  3  June 8, 2010 12:30 
ForcesCoeffs  ronaldo  OpenFOAM  4  September 14, 2009 07:11 