Can someone please share with
 

Can someone please share with me the code to monitor velocity (either U or V) as the solution progresses. I know this is done using the probe utility. However, I would prefer if someone can show me the code. I'm using the incompressible icoFoam solver.

Thanks a lot!

That depends on whether you wa
 

That depends on whether you want the data to be written to screen or to a file. If you want it written to file, check the implementation in oodles. If you want it written to the standard out, see below.

Put this before your time loop:

/******************************************/
IOdictionary pLocs
(
IOobject
(
"probeLocations",
runTime.constant(),
mesh,
IOobject::MUST_READ,
IOobject::NO_WRITE
)
);
const pointField& probeLocations(pLocs.lookup("probeLocations"));

labelList probeCells(probeLocations.size(), -1);

forAll(probeLocations, pI)
{
probeCells[pI] = mesh.findCell(probeLocations[pI]);
}
/******************************************/

And then put the following at the end inside your time loop:

/*******************************************/
forAll(probeCells, pI)
{
if(probeCells[pI] != -1)
{
label cellNo = probeCells[pI];
Pout << pI << ". Location: "
<< probeLocations[pI]
<< ", cell no.: " << cellNo
<< ", U: " << U[cellNo]
<< ", p: " << p[cellNo]
//add any other fields here
<< endl;
}
}

/*******************************************/

Put the probe locations in the constant/probeLocations dictionary as per usual.

Note the code hasn't been tested so there might be bugs.

Thanks very much Eugene. I fee
 

Thanks very much Eugene. I feel ashamed. I just went and included Probe.H and createProbes.H in my icoFoam.C followed by a reference to writeprobes.H after the runTime.write(); (i.e. # include "writeProbes.H"). Then I created a probeLocations inside the constant sub-directory. That was all. Follow that with a wclean && wmake to rebuild icoFoam and when I run my case, it neatly creates a probes subdirectory with velocity and pressure data at my selected point.

I thank you guys a lot for being so patient with n00bs. Thanks and keep up the good work!

Eugene, Many thanks for your
 

Eugene,
Many thanks for your code. I have successfully compiled my code. For some reason, I got this error while I tried to run the application.


--> FOAM FATAL IO ERROR : problem while reading header for object probeLocations

file: /home/qtian/OpenFOAM/qtian-1.4/run/tutorials/simpleFoam/bumpkom2/constant/probeL ocations at line 1.

From function regIOobject::readStream(const word&)
in file db/regIOobject/regIOobjectRead.C at line 75.

FOAM exiting

I know it must be something wrong with the probeLocations file format.

Here is probeLocations file format.

(
0.01 0.10 0.000
0.01 0.15 0.000
0.01 0.2 0.000
)

Is there any other way to read the probe points location? Thanks for your help.
Best

QT

OpenFOAM 1.4 has probe functio
 

OpenFOAM 1.4 has probe functionality inbuilt. Define your probe points in controlDict.

Dear Srinath, Could you tel
 

Dear Srinath,

Could you tell what are the keywords one have to write to the controlDict to activate the inbuilt probe functionality?

Thanks

Please use the 'Search' option
 

Please use the 'Search' option in future. Thanks!

Quoting Eugene from an eariler post:

Activate probes by adding the following to the end of your controlDict:

functions
(
probes1
{
type probes;

functionObjectLibs ("libsampling.so");

//dictionary probesDict;

region region0;

probeLocations
(
(0.710 -0.730 0.829)
(0.710 -0.757 0.763)
(0.855 -0.714 0.881)
(0.855 -0.748 0.805)
(0.855 -0.774 0.735)
(1.000 -0.695 0.932)
(1.000 -0.754 0.805)
(1.000 -0.779 0.735)
(1.350 -0.651 1.030)
(1.350 -0.740 0.862)
);

fields
(
p
U
);
}
)

Reference: http://www.cfd-online.com/OpenFOAM_D...es/1/4350.html

Dear Srinath, Thank you for
 

Dear Srinath,

Thank you for the prompt reply.

Just a correction. The last parenthesis have to be followed by a ";", or the function doesn't work.

flga

surface patch instead of probelocations
 

Hi,

Can we use any surface patch instead of writing probeLocation explicitly. I need this to calculate surface averaged quantity(vertex averaged) at the outlet patch in case of RTD calculations.

The following is not working.

functions
(
RTD
{
type probes;
functionObjectLibs ("libsampling.so");
setFormat gnuplot;
surfaceFormat raw;

probeLocations
(
patches (outflow)
);
fields (T);
}
);

Thanks
Santhosh..

patchAverage
 

I started again looking at the answer for the above problem.

Finally I could find that patchAverage utility can do the required operation.

Now the problem is patchAverage cannot be used for runTime calucation, i.e., patchAverage cannot write the output at each time step similar to probes utility. I am trying to modify it so that it will output average of a patch at each time step.

If anybody already done that please reply.

Regards
santhosh

Yes. It has been done. Have a look at http://openfoamwiki.net/index.php/Co...unctionObjects and the (note the original name) patchAverage-functionObject

Bernhard

Thanks Bernhard,

That is exactly what I want. Actually I was able to change the solver to do the required operation. But this utility is much more robust and generic.

Thanks a lot

--santoo..

Bernhard

Little help, May be I am doing simple mistake.

I successfully compiled simpleFunctionObject and could able to see it in USER_LIBBIN.

But, when I included function object in system dictionary as following,

functions
(
RTD
{
type patchAverage ;
functionObjectsLibs ("libsimpleFunctionObjects.so");
verbose true;
patches
(
outflow
);
factor 1;
}
);


I got following error,

Unknown function type patchAverage

Table of functionObjects is empty


From function functionObject::New(const word& name, const Time&, const dictionary&)
in file db/functionObjects/functionObject/functionObject.C at line 74.

FOAM exiting

--santosh

It is working now,

I added following in controlDict (change is addition of fields to it)

functions
(
RTD
{
type patchAverage;
functionObjectLibs ("libsimpleFunctionObjects.so");
fields ( T );
patches ( outflow );
verbose true;
factor 1;
}
);

-santhosh

Strange. Your previous example should have failed with an error about that missing (not with an empty table)

I too felt the same.

I came to know about adding field after running in openFOAM 1.5 version. I feel the problem is with 1.6 version. It may be printing wrong error messages/Error messages are misplaced in code.

-santhosh

Confused...
 

:o:D There is always different response ...

Question: You used different sources for 1.5 and 1.6 (the 1.5 version of the simpleFunctionObjects will not compile on 1.6 so this leads me to the suspicion that they were not there at all)

Bernhard

I have two machines one with 1.5 version and another 1.6 version..

I have compiled respective simpleObjects on different machines as given at
http://openfoamwiki.net/index.php/Co...unctionObjects.

(there both simpleObject utility for 1.5 and 1.6 versions are available)

The error I got in 1.6 machine is regarding "Table Empty"
The error I got in 1.5 machine is regarding "missing field"

hope I am clean now.

--santoo..

If it is not in the table, then the problem is that OpenFOAM can't find it. So do a wclean on the 1.6-version of the sources (I can't stress enough that the 1.5-version won't compile on 1.6) and make a "wmake libso" on them again. Lookout for an error. If there is
- no error
- it still doesn't work
- the library is found in $FOAM_USER_LIBBIN
try using another functionObject (probe for instance) with that case (because I only take responsibility after the simpleFunctionObjects are loaded into the runtime-selection-table ;) )

Bernhard

Thanks for constant help, I could able to use in OF 1.6 as well now.

someone used the probes in OF 1.6. An example can be found in
\incompressible\pimpleFoam\t-junction\system

// Write at same frequency as fields
outputControl outputTime;
outputInterval 1;

there is new keyword word for the output control.

nishant

Hello,

does anybody know, how I can redirect the data from a probe also directly to the screen, so that I can plot them with the pyFoam utility? Is there any option to be switched on like "log = true" or something like that?

For any help thank you in advance

Kind regards,
Toni

What you want is the value at one place on the standard-output so that a customRegexp can pick it up and plot it, right?

I'm afraid the probe-functionObject doesn't offer this (but I didn't research it too much)

What would be possible is to use (sorry) swak4Foam: generate a sampledSet of type cloud with one point. Use a functionObject swakExpression on it, set that to verbose and get that value. Maybe there is a simpler way.

To see how sampledSets are used in swak4Foam browse through the Examples that come with swak4Foam or look at my presentation from this years workshop

Bernhard

Problem using multiple probe locations
 

Hi all,

When I use multiple probe locations, only the data from the first location makes any sense, the rest gives values like -1e300. Does anyone have any experience with this? Ever seen this before?

My code looks like this:

functions
{
probes1
{
type probes;

functionObjectLibs ("libsampling.so");

region region0;

probeLocations
(
(1.3e-2 -2e-4 0)
(1.3e-2 0 0)
(1.3e-2 2e-4 0)
);

fields
(
U
);

outputControl timeStep;
outputInterval 100;
}
}


And I run the solver in parallel, on 4 cores (1 machine).

Thanks in advance for any help,

Sita

Additional info:
OpenFOAM gives warnings about these probe locations, it cannot find them:

--> FOAM Warning :
From function probes::read()
in file probes/probes.C at line 72
Did not find location (0.013 0 0) in any cell. Skipping location.
--> FOAM Warning :
From function probes::read()
in file probes/probes.C at line 72
Did not find location (0.013 0.0002 0) in any cell. Skipping location.

Strange, because both points are really present in my mesh...

-1e300 is the usual response if the probe is outside the mesh .... which OF very clearly points out to you in the warnings you quoted ("did not find in any cell")

Yeah, I know, that's pretty clear indeed. The only problem is, as I pointed out, that these points are really present in my mesh. In fact, they are in the list of vertices in blockMeshDict.

So maybe I should rephrase my question: why is OF unable to find these points? Is there something wrong with my syntax? Or does it have to do with the parallel solving? Or…?

Edges and corners are not a good idea. Testing for them is like dropping a ball onto a fence: you never know on which side it will fall (in your case: outside). Put the probe points SLIGHTLY inside (instead of 3 use 2.99999 for instance).

Thanks, that works!

Hello everyone,

I have a question regarding the probes function.

I'm modelling a wave flume with monochormatic waves propagating over it and i have applied the probes function to a series of points in the mesh to calculate velocity.

My question is: when i get the results ate the end of the run, those values of velocity are instantaneous velocity or are they phase averaged values?

I've been strugling with this for some time and maybe someone has the answer,

Thanks!

António