[sachinthakre]

Hello,
I am running a transient case (of course in OpenFoam) and I wish to plot average pressure on one of the boundaries with the time. Can anybody suggest me how to do it?

I tried PatchAverage p boundaryname. But I can't see anything either in paraview or something in post-processing folder (Or, I don't know how to see it).

Any help or suggestion is highly appreciated.

regards,
Naive user

[jherb]

If you install swak4foam you can use this:
https://openfoamwiki.net/index.php/C...unctionObjects

[Jason_Duguay]

Hi Sachin,

This is a way to do it without having to install swak4Foam:

averagePressure
{
type faceSource;
functionObjectLibs ("libfieldFunctionObjects.so");
outputControl timeStep;
log true;
valueOutput true;
source patch;
surfaceFormat off;
verbose true;
sourceName upstream; // replace this with your boundary patch name
operation areaAverage;

fields
(
p
);
}

Add the code above within the functions subdictionary in your controlDict file and change the sourceName to the boundary patch name that you want to calculate the average pressure over. The average pressure along the boundary will be printed out in a text file in the postProcessing folder in your case. To plot the pressure data you can easily do it with gnuplot (have a look online for a simple tutorial). Also, most solvers in OpenFOAM give pressure as the kinematic pressure (p/rho), so if you end up getting what look to be very small pressure values try multiplying them by your fluid density.

Hope that helps.

[sachinthakre]

Many thanks, Jason and Joachim, for your solutions.

Best,
Sachin

[otaolafr]

Originally Posted by Jason_Duguay

Hi Sachin,

This is a way to do it without having to install swak4Foam:

averagePressure
{
type faceSource;
functionObjectLibs ("libfieldFunctionObjects.so");
outputControl timeStep;
log true;
valueOutput true;
source patch;
surfaceFormat off;
verbose true;
sourceName upstream; // replace this with your boundary patch name
operation areaAverage;

fields
(
p
);
}

Add the code above within the functions subdictionary in your controlDict file and change the sourceName to the boundary patch name that you want to calculate the average pressure over. The average pressure along the boundary will be printed out in a text file in the postProcessing folder in your case. To plot the pressure data you can easily do it with gnuplot (have a look online for a simple tutorial). Also, most solvers in OpenFOAM give pressure as the kinematic pressure (p/rho), so if you end up getting what look to be very small pressure values try multiplying them by your fluid density.

Hope that helps.

thanks it was excatly what i was looking for!
small question, I am in a steadystate simulation (simpleFoam) so i would like to extract the averagePressure at the inlet but only for the last time, is it possible?
also when i continued my old simulation for the next time (I added the function to the controlDict) it have not created a postProssesing folder, should i do something extra to the run of the application so OF adds it?
thanks

[HPE]

Hi,

>> small question, I am in a steadystate simulation (simpleFoam) so i would like to extract the averagePressure at the inlet but only for the last time, is it possible?

- Adding the following entry to your function object may help in this regard: `writeTime onEnd;`.


>> also when i continued my old simulation for the next time (I added the function to the controlDict) it have not created a postProssesing folder, should i do something extra to the run of the application so OF adds it?

- Could you please elaborate this question, if possible? The `postProcessing` folder should be created when the function object writes out the relevant information.

[otaolafr]

Originally Posted by HPE

Hi,

>> small question, I am in a steadystate simulation (simpleFoam) so i would like to extract the averagePressure at the inlet but only for the last time, is it possible?

- Adding the following entry to your function object may help in this regard: `writeTime onEnd;`.


>> also when i continued my old simulation for the next time (I added the function to the controlDict) it have not created a postProssesing folder, should i do something extra to the run of the application so OF adds it?

- Could you please elaborate this question, if possible? The `postProcessing` folder should be created when the function object writes out the relevant information.

hello thanks for the help!
>>- Adding the following entry to your function object may help in this regard: `writeTime onEnd;`.
thanks a lot!

>>- Could you please elaborate this question, if possible? The `postProcessing` folder should be created when the function object writes out the relevant information.
I have my case already run it (it achieved the minimum residuals I gave in fvSolutions, so to see if this was functional, I added to the functions in the controlDict file, and then change the minimum residuals (to a lower level so the simulation could continue from the lastestTime) and run de solver, but there were no postProcessing folder created ( I changed as mentioned "sourceName upstream; // replace this with your boundary patch name" for "sourceName inlet" that is the name of my patch that i want to investigate.
EDIT: it shows as openFOAM (at least the version (vr7) i have does not have the same functions?) I did not saw this in the log file as it was at the beginning of the log and i though that if there was an error it would not continue at all...
first it does not recognise the function faceSource:

--> FOAM Warning :
From function void Foam::timeControl::read(const Foam::dictionary&)
in file db/functionObjects/timeControl/timeControl.C at line 89
Reading "/mnt/c/Users/Microreactors/Documents/OpenFOAM_Simulations/crearMeshWithPatches/Simulation_block_snap_topo_creat_simpleF/system/controlDict.functions.averagePressure" from line 52 to line 66
Using deprecated 'outputControl'
Please use 'writeControl' with 'writeInterval'
--> FOAM Warning :
From function bool Foam::functionObjectList::read()
in file db/functionObjects/functionObjectList/functionObjectList.C at line 746
Caught FatalError
--> FOAM FATAL ERROR:
Unknown function type faceSource

ps. it was the same proyect you helped me but i corrected the issue with the patches
franco

[HPE]

Hi,

I lost track of things, and lost entries where I promised to help. Can you poke me within few weeks time if I don't come back to your problem, and you would still need something. Thanks.