CFD Online Discussion Forums

CFD Online Discussion Forums (
-   OpenFOAM Post-Processing (
-   -   Average velocity of two different planes (

niqbal April 19, 2010 10:34

Average velocity of two different planes
3 Attachment(s)
Hi Foam Users,
I have done some MD simulations in OpenFOAM.The simulation is of water flow in a nanoChannel. At the center of the channel I had taken a slice along the z-axis and draw a velocity profile along the vertical line (y-axis). The velocity profile is atomistic. I want to take a couple of slices and want to take the profile of average velocity at those planes. Is there some way to combine the the velocity profiles and take the average of these profiles in paraview directly? or is there any other suitable way to do it? I am attaching screen shots also. The velocity profiles are at the same vertical line but at two different slices along the z-axis. I want to have the average of these velocity profiles.
Thanks in Advance.

Attachment 3031

Attachment 3032

Attachment 3033

chegdan October 22, 2010 16:35

average velocity profile in 3D space
I'm curious about this one as well. I would like to either obtain and average velocity profile from many slices or over a whole 3d domain. Anyone do this before?

Tobi December 20, 2010 07:59

What do the same with my temperatur profil.

I just can average my Inlet and outlet with "patchAverage T inlet/outlet" but i want to get the average temperature in some other planes. I heard that it is possible to make that with paraview but i don 't know how this works and which filter i have to use.

Some ideas ?

misge98 December 28, 2010 02:14

hi friends
I am trying to simulate twin screw pump by using ANSYS-FLUENT and I used dynamic mesh but I have a problem when I preview mesh motion and I got negative volume. before that I used ANSA for intial meshing of the model I think I have to smoothing the mesh but I couldn't, please can you suggest me how can I have to solve it and if you know any other refference on screw pump simulation please tell me.

Thank you!!!

Tobi January 3, 2011 16:02

I solved it.

You have to do the following steps:

1. open paraview
2. load your file or paraFoam etc.

3. set a slice and apply
4. use the filter -> integrateVariables and apply
5. use the filter -> calculator and apply
6. attribute mode: cell data
7. set a name and then use U/Area for average the velocity over that area ... T/Area for temperatur and so on and apply
8. activate integrateVariables and use "showing -> calculator" and change it to cell data.

The name "result" is the average velocity or so on... you can change the name "result" in the calculator...

thats it ...

bye tobi

shadabdyn June 17, 2017 16:12

Dear Tobi,

I have followed the above steps to calculate the average velocity on the slice but I have one confusion i.e by dividing the velocity by area the result will be of dimension [LT]^-1 which clearly is not the dimension of velocity but according to you the result is giving average velocity.
How is that possible?

Thanks & Regards
Shadab Mohammed

Tobi June 19, 2017 06:08

IntegrateVariable will multiply the quantity by the area or volume of the face/cell. Thats why you have to divide by the complete area/volume at the end again.
You can also make some simple tests to see that this holds or not. E.g. hotRoom tutorial -> uniform field (like T) at time = 0 - slice it, integrateVariable -> T gets 15000 K which could not be correct. Using caluclator filter and divide by the area lead to the average temperature of 300 K again (of course it is the new field).

Hope that it gets clear now. The evaluation should be like (for integrated values):
\phi_A = \sum_i^n \phi_i A_i
\phi_V = \sum_i^n \phi_i V_i

All times are GMT -4. The time now is 21:09.