CFD Online Discussion Forums

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   OpenFOAM Post-Processing (https://www.cfd-online.com/Forums/openfoam-post-processing/)
-   -   plot probe data (https://www.cfd-online.com/Forums/openfoam-post-processing/93794-plot-probe-data.html)

ehsanshams October 26, 2011 15:15

plot probe data
 
hi,

I have probe data from my simulation. Does anyone know what application opens the vector data (U)? or any application that can convert it to tecplot format?
here is the format of the data:

# x -3.5 -2 -1
# y 0.0333 0.0333 0.0333
# z 0 0 0
# Time
1000.1 (0.0346853 0.00264113 -0.00438583) (0.045667 -0.0254756 -0.00883625) (0.0479257 -0.00194718 -0.00995854)
1000.2 (0.0346853 0.002646 -0.00437969) (0.0461788 -0.0248685 -0.00900286) (0.0482703 -0.00188878 -0.0105974)
...


Thank you

fs82 November 25, 2011 09:33

You found a solution for your problem? If not I wrote a pyhton script which reformats the probes of openfoam and write a tecplot file. It is not very handy and fast, because it was my first experience with pyhton but it works. So if you need it, I could provide it to you.

kind regards,
Fabian

owayz January 9, 2012 21:37

Hi Fabian,
Can you send me that code.
Would I be able to extract the data over time for specified point from the techplot file? (I have no previous experince with techplot file thats why I ask it)

Regards,
Awais

fs82 January 10, 2012 03:57

1 Attachment(s)
Hi Awais,

no problem, here it is :)

fs82 April 5, 2012 07:38

1 Attachment(s)
I found a big bug in my python script. I don't no if you experience it but if you have time values twice in your probe data the script fails. I tried to fix the bug, but the source code of the script was to creepy. I decided to wrote it completely new.

kind regards,
Fabian

ehsanshams April 5, 2012 14:12

hey Fabian
thanks for updating the file, I'll check it out

palmerlee February 17, 2014 22:33

Hi, Fabian!

Could you please give more details about how to use this script? That'll be very helpful for learners like me.

Quote:

hpc@node12:~/OpenFOAM/lyp/rD5Re4400_7h$ python newFoamProbeToTecplot
Traceback (most recent call last):
File "newFoamProbeToTecplot", line 7, in <module>
import numpy
ImportError: No module named numpy
kind regards,
Peter

linyanx July 18, 2017 21:56

Quote:

Originally Posted by palmerlee (Post 475421)
Hi, Fabian!

Could you please give more details about how to use this script? That'll be very helpful for learners like me.



kind regards,
Peter

Hi Peter,

I wonder have you figured this code out, I'm also curious about the utilization of this code but find hard time understand this.

Best,
Linyan:)

fs82 July 20, 2017 06:21

To be honest I do not use this script anymore, since I discovered, that it is possible to use gnuplot to plot the probes
Code:

plot <file> u 1:2 " %lf (%*lf %*lf %*lf)" w l title 'your title'
Nevertheless, a word on this question
Quote:

hpc@node12:~/OpenFOAM/lyp/rD5Re4400_7h$ python newFoamProbeToTecplot
Traceback (most recent call last):
File "newFoamProbeToTecplot", line 7, in <module>
import numpy
ImportError: No module named numpy
This is very simple. You have to install a add-on for python called numpy http://www.numpy.org which includes various functionality for scientific usage. If you are using ubuntu it is just "apt-get install python-numpy" and your done.

Best regards
Fabian

linyanx July 20, 2017 09:28

postProcess -func probes problem
 
Quote:

Originally Posted by fs82 (Post 657760)
To be honest I do not use this script anymore, since I discovered, that it is possible to use gnuplot to plot the probes
Code:

plot <file> u 1:2 " %lf (%*lf %*lf %*lf)" w l title 'your title'
Nevertheless, a word on this question

This is very simple. You have to install a add-on for python called numpy http://www.numpy.org which includes various functionality for scientific usage. If you are using ubuntu it is just "apt-get install python-numpy" and your done.

Best regards
Fabian

Hi Fabian,

Thanks for your information, it works!

However, I have a confusing question about the function of the probe in the postProcess package. How to specify the probeLocations while using 'postProcess -func probes' command?

I want to probe a specific point after simulation. The problem is the system/probesDict which contains specified location and fields information cannot be recognized by the system while I command 'postProcess -func probes'. Instead, it just probes out the point (0,0,0) and field p and U which is by default. I know it must be some tiny points that I've ignored. I haven't either found by google or by the forum post about the specific procedures regarding using the 'postProcess -func probes'.

Could you see what's wrong with the way I did with the probe function?

Best,
Linyan

fs82 July 20, 2017 09:44

I tried it and it worked well. Just add a probe to your controlDict
Code:

functions
{
    probes
    {
        type            probes;
        libs ("libsampling.so");
        writeControl    timeStep;
        probeLocations
        (
            (x y z)
        );
        fields
        (
            U
        );
    }
}

and execute
Code:

postProcess -func probes
.
Works perfectly and gives you the result in postProcessing/probes/<time>.

fs82 July 20, 2017 09:50

Ok sorry it is not working. I was too fast. However, check the information on the CFDDirect Homepage https://cfd.direct/openfoam/user-gui...hs-monitoring/ this works fine.

linyanx July 20, 2017 10:05

Quote:

Originally Posted by fs82 (Post 657804)
Ok sorry it is not working. I was too fast. However, check the information on the CFDDirect Homepage https://cfd.direct/openfoam/user-gui...hs-monitoring/ this works fine.

Fabian,

You made my day! It works. This link illustrates the exact way to probe at the specific location.

Thanks,
Linyan

sitajeje August 9, 2017 07:00

Hi Fabian,

Perhaps I made some basic mistakes. I followed the link you posted by copying the "probes" file into "system" folder, and add functions {#includeFunc probes} into "controlDict". After I ran the postProcess -func probes, one "postProcessing/probes" folder was created. However the data was not saved in one single file, but different time folders were created, where the "U" file with one single data for the corresponding time was saved. I ran also pimpleDyMFoam -postProcess, but nothing happened, the #includeFunc seemed to be absent.

I would appreciate if you could give me some suggestions, thank you very much in advance!

Best regards,

sitajeje

fs82 August 10, 2017 03:01

The instruction at this page https://cfd.direct/openfoam/user-gui...hs-monitoring/ are really good and work perfectly, as long as you are using the Foundation Release (no + and no extend) greater than 4.0.

Best regards
Fabian

sitajeje August 10, 2017 06:00

Dear Fabian,

I tried with tutorial cases, and found that the "probes" works as the user guide describes for "cavity" and "pitzDaily". For "mixerVesselAMI2D" it functioned as in my case. This problem might be related to the *DyM* solver.

sitajeje


All times are GMT -4. The time now is 11:56.