Monitor Total Pressure in a running simulation using functionobjects
 

Hi,
I'm new to Open Foam, so probably the solution of my problem will be really simple for other user but I couldn't find anything about this in the forum.
I'm running a simulation of something similar to a pipe in simpleFoam ( OpenFoam 2.2.0). I'd like to monitor the areaAverage of the total pressure on the outlet boundary as a parameter to judge when the simulation reaches a good convergence. I'm doing the same for the massflowrate with a functionobject and it works fine but when I try to do it using the new pressureTools I got this warning:


The simulation runs fine and it saves a folder total(p) every iterations but it doesn't calculate the areaAverage at Outlet.



this is my control dictionary function:

Thank you in advance for your help!



Ale

anybody can help me?

Did I do something wrong?

Greetings CFD-Cat,

Mmm... this looks sort-of familiar... OK, 2 details:

1. In this part of the code:
   
   Code:

   ---

   TotalPressureAveOutlet
{
type patchAverage;
functionObjectLibs ("libsimpleFunctionObjects.so");
verbose true;
patches (outlet);
factor 1;
fields (
total(p)
);
outputControl  timeStep;
outputInterval  1;
outputControlMode timestep;
}

   ---

   You should use quotes:
   
   Code:

   ---

   fields (
"total(p)"
);

   ---

   This is to avoid any other kind of interpretation.
2. Secondly, the file name depends on several factors, as described on the Doxygen documentation: http://foam.sourceforge.net/docs/cpp...4.html#details

More specifically, I wrote about this here: http://www.cfd-online.com/Forums/ope...tml#post430031 post #4


Beyond this, I need an example case to test this for myself.

Best regards,
Bruno

I added the quote but it gives the same error. :-(

Hi CFD-Cat,

I finally managed to have a look into the case you sent me and it was fortunately rather simple!
A bit of a introduction - the idea behind "()" and "{}" is this:

• The brackets "{}" are for gathering blocks of options, such as this:
  
  Code:

  ---

  {
a 123;
b 4564;
c "word";
}

  ---

• The parenthesis "()" are for lists of values, such as:
  • Code:

    ---

    (1 2 3)

    ---

  • Code:

    ---

    ((0 1 2) (3 4 5))

    ---

    Which is the same as:
    
    Code:

    ---

    ((0 1 2) (3 4 5))

    ---

  • And the ultimate kind of list:
    Code:

    ---

    (
{
a 123;
b 4564;
c "word";
}

{
a 534;
b 57467;
c "another word";
}
)

    ---

The reason why this didn't work:
Is because lists with parenthesis cannot have a name or title. This is why "functions" should be a block list of blocks:
Best regards,
Bruno

Hi CFD-Cat,

To answer the question you've asked via private message, the full "functions" entry should look something like this:
Notice that brackets "{}" are used for the "functions" block, and not parenthesis "()".

Best regards,
Bruno

Hi,
I'm sorry to restart this old discussion but since when I installed OF2.2.2 instead of OF2.2.0 I'm facing a new problem with pressureTools function object.

I can't understand the reason why when i try to calculate the total(p) the output reports only the BC like if no internal field has been calculated. It I try to calculate the static(p) I got the same problem, while for the total(p)_coeff I got a field distribution(maybe wrong) even setting the pInf =0.

I check if someone else found a similar problem but I wasn't able to find anything useful.

Except for this sentence that sincerely I don't understand completely:

"Where the function generates a field, e.g. wallShearStress, pressureTools, yPlusRAS, etc., the field is now stored on the mesh database so that it is available for further post-processing. " from http://www.openfoam.org/version2.2.2/

Hi CFD-Cat,

I need more information in order to be able to help you, namely:

1. How exactly did you configure the function objects section at "controlDict"?
2. What type of simulation are you performing?
3. Are you able to reproduce the error with a tutorial from OpenFOAM?

Best regards,
Bruno

I'm out of office. On monday I'll try the tutorial and I'll send you the file.thank you for your help

Hi wyldckat,

I reproduced it with the tutorial Tjunction. This is my controlDict

and this is the output :

while the total(p)_coeff is like this:

I run my case with simpleFoam too and I got the same result.

Best regards,

Ale

Hi Ale,

I finally managed to look into this. This should work:
The missing details were these:
"rhoRef" doesn't exist, it's "rhoInf" that should be used. And we have to indicated that the name of the field to be used for "rho" is "rhoInf", so that it knows that it should use the constant value, as there is no "rho" field.

Although a bit cryptic, this can be spotted if we look at the source code: https://github.com/OpenFOAM/OpenFOAM...reTools.C#L263
Best regards,
Bruno

Thank you very much Bruno. Now it works! I really appreciate your help.

I didn't check it because in OF2.2.0 it works fine without

Monitor Total Pressure in a running simulation using functionobjects
 

For people looking for the same functionality in OpenFOAM version 6

Does anybody know how to do that in OpenFOAM-1906 and 1912? Does not seem to accept "pressure" as a function type. "unknown function type pressure"

Solved: needed to add "libfieldFunctionObjects.so" in the libs-section on top of "controlDict" to make it work.