CFD Online Discussion Forums - Probe Warning, Probe Does Not Work

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)

- OpenFOAM Pre-Processing (https://www.cfd-online.com/Forums/openfoam-pre-processing/)

- - Probe Warning, Probe Does Not Work (https://www.cfd-online.com/Forums/openfoam-pre-processing/124412-probe-warning-probe-does-not-work.html)

Probe Warning, Probe Does Not Work

Greetings people,

I am running a case, with parallel computing, and before the computations I got this warning message:

Code:

--> FOAM Warning :

    From function probes::read()

    in file probes/probes.C at line 71

    Did not find location (0.03 0.11 0) in any cell. Skipping location.

--> FOAM Warning :

    From function probes::read()

    in file probes/probes.C at line 71

    Did not find location (0.03 0.11125 0) in any cell. Skipping location.

--> FOAM Warning :

    From function probes::read()

    in file probes/probes.C at line 71

    Did not find location (0.03 0.1125 0) in any cell. Skipping location.

--> FOAM Warning :

    From function probes::read()

    in file probes/probes.C at line 71

    Did not find location (0.03 0.1225 0) in any cell. Skipping location.

--> FOAM Warning :

    From function probes::read()

    in file probes/probes.C at line 71

    Did not find location (0.04 0.12375 0) in any cell. Skipping location.

--> FOAM Warning :

    From function probes::read()

    in file probes/probes.C at line 71

    Did not find location (0.0475 0.1275 0) in any cell. Skipping location.

I did not got any error with the checkMesh, and as I checked the probes are not outside the domain. I read on other thread (I do not remember the link) that while decomposing it might appear some problems. So I run the case in a single processor, and got the same warning, but only in one probe, the warning message is:

Code:

--> FOAM Warning : 

    From function probes::read()

    in file probes/probes.C at line 71

    Did not find location (0.0475 0.1275 0) in any cell. Skipping location.

So, does anyone know what is the problem ?

checkMesh and see whether your mesh is in domain or not

As I said (and confirmed), the probes are in the domain. If I DO NOT decompose the problem, i. e. run the simulation in only one processor, OpenFOAM still gives me one warning. Is there any problems between decomposing the mesh and probe locations ? And why I get the warning, if the probe is in the domain ?

rather than using a probe functionObject try a polyLine set where the original probeLocations are now the points.

Hi,

actually warning are self-explanatory

Code:

Did not find location (0.03 0.1225 0) in any cell. Skipping location.

For example in the warning it tries to tell you that a probe (0.03 0.1225 0) is outside of the mesh. And surely if a probe is outside of the mesh, there's nothing to probe.

Check dimensions of the mesh, check where you put your probes. Try to put all the probes inside the mesh.

sure alexeym, but I have noticed the probe functionObject having trouble locating points that are inside a mesh when running in parallel. There are slight differences in the implementation of the particular findCell() function for probes, polyLines, clouds, etc. and in my experience, there are some bugs.

Oh, sorry, missed several messages.

Does the number of warnings depend on the decomposition (number of subdomains, decomposition method)? Maybe probes are on processor boundaries (though in this case another warning should be issued)?

I've looked though the implementation of findCell method and wasn't able to find anything that won't be working in parallel cases.

I've attached a case where I noticed this happening. The controlDict has functionObjects that write out velocity and pressure at 120 locations inside the domain at each iteration, once using type probes from libsampling and once using type sets with polyLine. The polyLine method works fine, but the probes approach skips four locations. Just use Allrun - hopefully it's self-explanatory.

If you get to the bottom of that and are still motivated, check out http://www.openfoam.org/mantisbt/view.php?id=0001147 for a another sampling peculiarity.

Hi,

unfortunately I wasn't able to reproduce the error, here is the output of the solver for the attached case:

Code:

Build  : 2.2.2-9739c53ec43f

Exec   : simpleFoam -parallel

...

SIMPLE: convergence criteria

    field p      tolerance 0.001

    field U      tolerance 0.0001

    field "(k|epsilon)"  tolerance 0.0001





Starting time loop



Reading set description:

    polyLine



Time = 1



smoothSolver:  Solving for Ux, Initial residual = 1, Final residual = 0.0762530558, No Iterations 1

smoothSolver:  Solving for Uy, Initial residual = 0.69705505, Final residual = 0.651831039, No Iterations 1000

smoothSolver:  Solving for Uz, Initial residual = 1, Final residual = 0.0752473553, No Iterations 1

GAMG:  Solving for p, Initial residual = 1, Final residual = 0.0835314711, No Iterations 2

time step continuity errors : sum local = 1.10938559e-16, global = -3.04128912e-18, cumulative = -3.04128912e-18

smoothSolver:  Solving for epsilon, Initial residual = 0.999999992, Final residual = 0.0309136051, No Iterations 2

smoothSolver:  Solving for k, Initial residual = 0.999999991, Final residual = 0.0339960612, No Iterations 2

...

thanks for trying that out. I noticed from your output log that you are running 2.2.2. I had been running 2.3.x. I've built 2.2.x again and tested the same case - my output is now just like yours - no errors. If you (or anyone else) have 2.3.x available, I'd be interested in how that works for you. In the meantime though, I'll submit a bug report when I have an opportunity.

I'd like to confirm that bug can be reproduced with 2.3.x.

There was certain changes in findCell algorithm between 2.2.2 and 2.3.x though I wasn't able yet to determine the reason why everything is OK under 2.2.2 and not OK under 2.3.x (though I guess the reason is tetrahedral cells near the probes as mainly the algorithm was changed for tetrahedral mesh).

hello!

I can also confirm the bug. I'm using version 2.3.0 and for a list of 45 points which clearly ly within the domain 8 are not found. If I use the sample application the same error accures. Did somebody find a solution for the problem?

Hi, I'm facing a similar issue in OpenFOAM 4.1. Did someone file a bug report?

Hei hei I used also version 3.0+ and there I do not have any problems to find the probes