CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Paraview & paraFoam (http://www.cfd-online.com/Forums/openfoam-paraview/)
-   -   StreamFunction (http://www.cfd-online.com/Forums/openfoam-paraview/120197-streamfunction.html)

 Luis Batista July 2, 2013 10:00

StreamFunction

Hello Forum,

I am doing an analysis to a cavity flow using SimpleFoam....:)

Is there any known issue/error with the OF(2.1.2) function StreamFunction ?

Apparently, I am having proper results within my vorticity vector field but when I plot the point field resulting from the streamFunction in Paraview, it seems that the results are 10 times smaller....I also see that the units of the streamfunction scalar field are L3 T-1.

How are these units being derived?

Regards,
Luis

 wyldckat July 7, 2013 05:57

Hi Luis,

Can you provide a simple test case?

Best regards,
Bruno

 chl August 19, 2013 13:37

1 Attachment(s)
Dear Bruno and Luis,

I find the same with version 1.6-ext: the stream function seems to be too small by a factor of 10 and has dimensions length^3/time.

I attach a case of a linear shear flow, U = (y/H)*V, with H the height of the domain, and V the velocity at the upper boundary.

The stream function should be: \Psi = 0.5*((y/H)^2 -1)*V*H

best regards,
Christiane

 chl August 20, 2013 05:34

Hi,

the factor 0.1 seems to stem from the cell width in the empty direction, which is \Delta z = 0.1 in the above example. Reducing \Delta z to 0.01 also reduces the streamFunction by another factor of 10.

So it seems, that the streamFunction utility computes
\Psi*\Delta z, not \Psi. This would also explain the dimensions length^3/time.

Do you agree?

best regards,
Christiane

 wyldckat August 21, 2013 09:32

Greetings Christiane,

Many thanks for the test case, but I haven't yet managed to look into it.
But I've taken a quick look into the source code of "streamFunction" on both 2.2.x and 1.6-ext:
And both calculations seem to be done in the same. I can't find any indication of an explicit scaling factor, which leads me to believe that the phi field that OpenFOAM is using already includes the scale of each cell or face. Because the sign function only gives us "+1" or "-1".

Another indication is that it doesn't seem to work for 3D simulations, because it assumes that Z is the empty orientation.

I'll try to look at the test case later today.

Best regards,
Bruno

 chl August 22, 2013 12:28

Hi Bruno,

yes, the face flux field phi is
phi = U_f & S_f, with S_f the area of the face.

For the computation of the stream function U_f & S_f/\Delta z would be

best regards,
Christiane

 wyldckat August 22, 2013 12:59

Hi Christiane,

Of course! Why didn't I visualize that... the face area still depends on Z, even though the flow is only over X-Y.

OK, then there are 2 immediate solutions:
1. Use 1.0 for the width of the empty direction, in order to avoid the distortion of the "phi" and "psi" calculation.
• This reminds me of a 2D tutorial in OpenFOAM that uses the thickness of 1.0m and I didn't understand why... until now. The tutorial is the "combustion/XiFoam/ras/moriyoshiHomogeneous".
2. Request a bug fix for this at the respective bug trackers:
1. Official OpenFOAM: http://www.openfoam.org/bugs/
2. Extend Project's bug tracker: http://sourceforge.net/apps/mantisbt/openfoam-extend/
Best regards,
Bruno

 chl August 26, 2013 04:29

Hi Bruno,

thanks!

I requested bug fixes at both sites:
http://www.openfoam.org/mantisbt/view.php?id=976
http://sourceforge.net/apps/mantisbt...iew.php?id=185

best regards,
Christiane

 All times are GMT -4. The time now is 11:26.