CFD Online Discussion Forums
Page 2 of 3 1 2 3
Show 40 post(s) from this thread on one page

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (https://www.cfd-online.com/Forums/openfoam-solving/)
-   -   Foam fatal io error: cannot find file (https://www.cfd-online.com/Forums/openfoam-solving/134568-foam-fatal-io-error-cannot-find-file.html)

sihaqqi June 1, 2014 10:41
1 Attachment(s)
Dear Bruno

Many thanks for your efforts. I removed last time step to check again at 0.1008569 and same thin happened. Also I tried with 0.1008569 and 0.100857 and I got the error as double scalar. I have attached the file you asked for. Log file is 203MB so after compression, it is still big enough and cannot be attached. However tomorrow I shall try to see in my Uni what other compression software we have. If I have something which can compress more, I shall reattach.

Best Regards
Imad

wyldckat June 2, 2014 15:52
Hi Imad,

Hopefully I've figured out what the problem is! And it's one of those really annoying ones at that...

OK, in post #16 you have this:
Code:
Time = 0.1011976
It has 7 significant digits.

Then in post #18 you have the following details:
  1. Quote:
    Originally Posted by sihaqqi (Post 494427)
    No such time step as 0.101057 exists anywhere. Last time step I have in all processors is 0.1010569.
    The solver is asking for a time folder with 6 significant digits. But the existing folder has got 7 digits.
  2. Quote:
    Originally Posted by sihaqqi (Post 494427)
    Controldict contents are

    Code:
    //...
    deltaT          1e-7;
    //...
    timePrecision  6;
    //...
    The defined precision in "controlDict" is 6 digits.
In the file list you attached in the previous folder you also have a lot of time folders with 7 digits. This apparently is because you have a deltaT of 1e-7, which means that sooner or later you're going to at least need 7 significant digits.

In addition, the file list you provided does not follow to a fixed deltaT, which I assume is because you used "writeControl clockTime" in the first run, which lead to the time folders you have at this moment.


The solution should be crazy simple: edit the file "system/controlDict" and change the timePrecision entry to 7 or 8 or even 9.


I do write every once in a while here on the forum that every single detail, no matter how insignificant if may seem, is a lot more important to OpenFOAM than we might want to believe!

Best regards,
Bruno

sihaqqi June 4, 2014 22:59
Dear Bruno
I did not come back earlier because I have modified my controlDict and am waiting for simulations to run so that I can give you some sort of feedback. Still I am waiting. As soon as I see everything is okay which I expect it to be like you do, I shall advise.
Thanks again

Best Regards
Imad

sihaqqi June 5, 2014 01:05
Hi Bruno

I am experiencing same error.
Code:
cannot find file
[210]
[210] file: /scratch/director674/shaqqi/tee/LES/75_original/processor210/0.100857/p at line 0.
[210]
[210]    From function regIOobject::readStream()
error continues for many processors like this

Also, log file ends in
Code:
"e533.27255"
"e541.5558"
"e548.5864"
)

Pstream initialized with:
    floatTransfer    : 0
    nProcsSimpleSum  : 0
    commsType        : nonBlocking
sigFpe : Floating point exception trapping - not supported on this platform
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create mesh for time = 0.100857

Reading field p

wyldckat June 6, 2014 15:02
Hi Imad,

A few questions:
  1. What is the content of the "system/controlDict" file you used for this latest output?
  2. Which are the latest time folders that are present in the "processor*" folders?
  3. What is the content of the file "uniform/time" that is in the latest time folder, in "processor0"?
    For example, if the latest time folder is "0.1008569", then what's inside the file "processor0/0.1008569/uniform/time"?
By the way, when posting code, file contents and so on, please use the "[CODE]" markers, as explained here: Posting code and output with [CODE]

Best regards,
Bruno

sihaqqi June 8, 2014 07:19
Hi Bruno

controlDict contents are

Code:
application    pisoFoam;

startFrom      latestTime;

stopAt          endTime;
//stopAt          nextWrite;

endTime        5e-1;

deltaT          1e-7;

writeControl    timeStep;
//writeControl    clockTime;

writeInterval  2000;

purgeWrite      10;

writeFormat    ascii;

writePrecision  8;

writeCompression off;

timeFormat      general;

timePrecision  6;

runTimeModifiable true;

functions
{
    probes
    {
        type            probes;
        functionObjectLibs ("libsampling.so");
        enabled        true;
        outputControl  timeStep;
        outputInterval  1;

        fields
        (
            p
        );

        probeLocations
        (
        (0.036 2.000 0)
        (0.036 2.400 0)
            (0.036 2.600 0)
            (0.036 2.700 0)
            (0.036 2.798 0)
        (0.100 2.798 0)
        (0.300 2.798 0)
        (0.500 2.798 0)
        (1.000 2.798 0)
            (1.500 2.798 0)
        (2.000 2.798 0)
        (2.500 2.798 0) 
        (3.000 2.798 0)
        (3.500 2.798 0)
        (4.000 2.798 0)
        (4.500 2.798 0)
        (-0.100 2.798 0)
        (-0.300 2.798 0)
        (-0.500 2.798 0)
        (-1.000 2.798 0)
            (-1.500 2.798 0)
        (-2.000 2.798 0)
        (-2.500 2.798 0) 
        (-3.000 2.798 0)
        (-3.500 2.798 0)
        (-4.000 2.798 0)
        (-4.500 2.798 0)     
        );

    }

    fieldAverage1
    {
        type            fieldAverage;
        functionObjectLibs ("libfieldFunctionObjects.so");
        enabled        true;
        outputControl  outputTime;

        fields
        (
            U
            {
                mean        on;
                prime2Mean  on;
                base        time;
            }

            p
            {
                mean        on;
                prime2Mean  on;
                base        time;
            }
        );
    }

    surfaceSampling
    {
        // Sample near-wall velocity

        type surfaces;

        // Where to load it from (if not already in solver)
        functionObjectLibs ("libsampling.so");
        enabled        true;
        outputControl  outputTime;

        interpolationScheme cellPoint;

        surfaceFormat vtk;

        // Fields to be sampled
        fields
        (
            U
        );

        surfaces
        (
            nearWall
            {
                type            patchInternalField;
                patches        ( lowerWall );
                distance        1E-6;
                interpolate    true;
                triangulate    false;
            }
        );
    }
Answer 2: Latest time step is 0.1008569

Answer 3:
Last time step uniform/time contents are below


Code:
FoamFile
{
    version    2.0;
    format      ascii;
    class      dictionary;
    location    "0.1008569/uniform";
    object      time;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

value          0.100857;

name            "0.1008569";

index          182000;

deltaT          1e-07;

deltaT0        1e-07;


// ************************************************************************* //
Do you think if I change all time files manually and write value as 0.1008569 instead of 0.100857, should it work. Is there any command in linux which can change all these files with this value simultaneously as there are 1200 processors i.e., if it is going to be of help.

Thanks for your efforts and time.
Regards
Imad

wyldckat June 8, 2014 08:03
Hi Imad,

I strongly advise you not to manually modify the time information in the time-related folders and files. Specially because you're using the time averaging procedure.

Edit the file "system/controlDict" and change this line:
Code:
timePrecision  6;
To this:
Code:
timePrecision 8;
or to this:
Code:
timePrecision 9;
Best regards,
Bruno

sihaqqi June 8, 2014 09:03
Thanks Bruno

I apologize, I made writePrecision as 8 but not timePrecision by mistake. Anyways, I have corrected it. Hopefully it should work. I shall update you as soon as simulations run.

Best Regards
Imad

sihaqqi June 8, 2014 22:37
Dear Bruno

Thanks, it has worked.

Best Regards
Imad

sihaqqi July 29, 2014 09:44
Quote:
Originally Posted by sihaqqi (Post 496167)
Dear Bruno

Thanks, it has worked.

Best Regards
Imad
Dear Bruno,
With reference to my question at link at
http://www.openfoam.org/mantisbt/view.php?id=1355#c3178

I will let that question at openfoam.org stay because I need to know why the software does not write more time steps after deleting the different time step. If we together figure out a way to solve it, I shall close the query myself. I know that solving all my questions is not your responsibility but in fact people like you take out your time to guide us.
I have posted the same question with more description at the link
http://www.cfd-online.com/Forums/ope...tml#post503586

If you can just go through it and advise, it would be great as it can save a lot of time. For your information, my job scheduler does not provide any warning as you mentioned. I use OpenFOAM 2.1.1. I cannot find "adjustTimeStep".

Regards
Imad

wyldckat August 16, 2014 12:50
Hi Imad,

I've answered your question in the other thread. As for the last statement on this post above:
Quote:
Originally Posted by sihaqqi (Post 503589)
I cannot find "adjustTimeStep".
It's explained in the User Guide: http://www.openfoam.org/docs/user/controlDict.php - and demonstrated in several tutorials.
You can find all tutorials that use this feature by running this command:
Code:
find $FOAM_TUTORIALS -name controlDict | xargs grep -sl "adjustTimeStep"
For more information on how to search for more information in files present in OpenFOAM: http://openfoamwiki.net/index.php/In...hing_for_files

Best regards,
Bruno

diananilminikumari March 20, 2015 03:43
cannot find file ....buoyantBoussinesqPimpleFoam/hotcy/hotcylinderm/0/T at line 0
 
Dear all,
I was trying to simulate flow through a cylinder.
After run the blockMesh , I have run buoyantBoussinesqPimpleFoam.
but it gave the error,

-> FOAM FATAL IO ERROR:
cannot find file

file: /home/diana/OpenFOAM/diana-2.3.0/run/tutorials/heatTransfer/buoyantBoussinesqPimpleFoam/hotcylinderm/0/T at line 0.

From function regIOobject::readStream()
in file db/regIOobject/regIOobjectRead.C at line 73.

FOAM exiting

Since I'm new in OpenFoam it is difficult to find why this is happening . please kind to help me

franjo_j March 20, 2015 04:05
Hello,

It looks the T file does not exist in the 0 folder of your case. This is file needed to read the boundary conditions for the temperature fields and the values of temperature. Some tutorials in OpenFOAM-2.3.0 contain T.org which you can use a template for your problem.

Regards,

Franjo

Quote:
Originally Posted by diananilminikumari (Post 537341)
Dear all,
I was trying to simulate flow through a cylinder.
After run the blockMesh , I have run buoyantBoussinesqPimpleFoam.
but it gave the error,

-> FOAM FATAL IO ERROR:
cannot find file

file: /home/diana/OpenFOAM/diana-2.3.0/run/tutorials/heatTransfer/buoyantBoussinesqPimpleFoam/hotcylinderm/0/T at line 0.

From function regIOobject::readStream()
in file db/regIOobject/regIOobjectRead.C at line 73.

FOAM exiting

Since I'm new in OpenFoam it is difficult to find why this is happening . please kind to help me

diananilminikumari March 23, 2015 23:59
Quote:
Originally Posted by franjo_j (Post 537345)
Hello,

It looks the T file does not exist in the 0 folder of your case. This is file needed to read the boundary conditions for the temperature fields and the values of temperature. Some tutorials in OpenFOAM-2.3.0 contain T.org which you can use a template for your problem.

Regards,

Franjo
Thank you very much, for your information and I got it .:)

sumo793 July 3, 2016 22:16
--> FOAM FATAL IO ERROR:
Cannot find patchField entry for rotatingWall1

file: /home/sumit/OpenFOAM/sumit-3.0.1/run/tutorials/incompressible/simpleFoam/generator/0/U.boundaryField from line 26 to line 75.

From function GeometricField<Type, PatchField, GeoMesh>::GeometricBoundaryField::readField(const DimensionedField<Type, GeoMesh>&, const dictionary&)
in file /home/openfoam/OpenFOAM/OpenFOAM-3.0.1/src/OpenFOAM/lnInclude/GeometricBoundaryField.C at line 209.

FOAM exiting



rotatingWall2
{
type fixedValue;
value uniform (0 0 0);
origin (0 0 0);
axis (1 0 0);
omega 83.73;
}

rotatingWall3
{
type fixedValue;
value uniform (0 0 0);
origin (0 0 0);
axis (1 0 0);
omega 83.73;
}

rotatingWall1
{
type fixedValue;
value uniform (0 0 0);
origin (0 0 0);
axis (1 0 0);
omega 83.73;

}



stuck at this error from few days....any solution:confused:

Antimony July 4, 2016 04:43
Hi,

My guess, without looking at the entire U file, is that you are missing a ; and/or a } somewhere.

Cheers,
Antimony

sumo793 July 4, 2016 04:51
i will check....thanks

niran November 24, 2016 03:09
i am facing the same problem

Reading waveProperties


--> FOAM FATAL IO ERROR:
cannot find file

file: /home/user/OpenFOAM/user-2.4.0/run/waveFlume2/constant/waveProperties at line 0.

From function regIOobject::readStream()
in file db/regIOobject/regIOobjectRead.C at line 73

how to slove this problem

i am running wave2foam tutorial waveFlume

Aditya Patil January 5, 2017 13:14
OpenFOAM for Windows 16.06 (v2)

Aadhi@Aditya /cygdrive/c/OpenFOAM/Aadhi-3.0.x/run
$ tutorials/incompressible/icoFoam/elbow_tri
-bash: tutorials/incompressible/icoFoam/elbow_tri: Is a directory

Aadhi@Aditya /cygdrive/c/OpenFOAM/Aadhi-3.0.x/run
$ fluentMeshToFoam.exe elbow.msh
/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 3.0.x |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
|*---------------------------------------------------------------------------*|
|* OpenFOAM for Windows 16.06 (v1) *|
|* Built by CFD Support, www.cfdsupport.com (based on Symscape). *|
\*---------------------------------------------------------------------------*/
Build : 3.0.x-ac3f6c67e02f
Exec : C:\OpenFOAM\cygwin64\opt\OpenFOAM\OpenFOAM-3.0.x\platforms\cygwin64mingw-w64DPInt32Opt\bin\fluentMeshToFoam.exe elbow.msh
Date : Jan 05 2017
Time : 18:11:14
Host : "ADITYA"
PID : 3904
Case : C:/OpenFOAM/Aadhi-3.0.x/run
nProcs : 1
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Allowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time



--> FOAM FATAL IO ERROR:
cannot find file

file: C:/OpenFOAM/Aadhi-3.0.x/run/system/controlDict at line 0.

From function regIOobject::readStream()
in file db/regIOobject/regIOobjectRead.C at line 73.

FOAM exiting


Aadhi@Aditya /cygdrive/c/OpenFOAM/Aadhi-3.0.x/run
$

alixcattermole December 14, 2017 17:17
Hello,

I am trying to import a mesh from netgen to openfoam and getting the same problem you had when i use the command netgenNeutralToFoam.
How did you manage to get around this error?
My error -->FOAM FATAL IO ERROR
cannot find file

file: /home/ofuser/workingDir/openfoam-v1706/system/controlDict at line 0

I am in the openfoam-v1706 working directory when i do this.

Thanks.


All times are GMT -4. The time now is 17:16.
Page 2 of 3 1 2 3
Show 40 post(s) from this thread on one page