[alimansouri]

Hi guys

I am working on my first tutorial (lidcavity) and I changed the mesh density from 20*20 to 41*41
and I got this error


size 400 is not equal to the given value of 1681


could you help and let me know what I am missing?

thank you!

[sachin]

Hi ,
I m not sure just delete all other files other than blockMeshdict from polyMesh folder and again run blockMesh...
i hope u ran blockMesh command after editing meshdict

[sega]

The initialization of gamma is done in a list containing 20*20 values. If you change the cell to 41*41 there are more cells than values for gamma.

You have to set the gamma field to the new mesh using setFields or funkySetFields.

Tell me if this works out.

[idrama]

Thanks a lot!

It had worked.

cheers

[A H Gazi]

Originally Posted by idrama

Thanks a lot!

It had worked.

cheers

Hi sir i am facing same error in twoPhaseEulerFoam.how did you solve your problem ?please help. i am very new in openfoam. where to change gamma value i am not able to find out.i am using openFoam 5.0.
....size 6000 is not equal to the given value of 49600
Thanks and please reply .

[RobertHB]

As Sebastian wrote in 2009, your gamma file contains less values than you have grid points. This is most likely because you changed the mesh of the case that you are using. Create a "empty" gamma file in your 0 folder. Similar to the other variables there, with only your boundaries. If you need a patch value or internal field, define it there. But dont use the gamma file with a list of values that dont match your mesh.
Alternatively, you can try mapping the lower resolution list onto your new mesh using map fields.

[A H Gazi]

Originally Posted by RobertHB

As Sebastian wrote in 2009, your gamma file contains less values than you have grid points. This is most likely because you changed the mesh of the case that you are using. Create a "empty" gamma file in your 0 folder. Similar to the other variables there, with only your boundaries. If you need a patch value or internal field, define it there. But dont use the gamma file with a list of values that dont match your mesh.
Alternatively, you can try mapping the lower resolution list onto your new mesh using map fields.

Thank you very much sir, for your quick reply.As i said i am very new in openFoam.Will you please give me a example. after making gamma file and putting my boundary condition what will be the gamma value??sorry for my little knowledge.
Regard

[RobertHB]

Originally Posted by A H Gazi

Thank you very much sir, for your quick reply.As i said i am very new in openFoam.Will you please give me a example. after making gamma file and putting my boundary condition what will be the gamma value??sorry for my little knowledge.
Regard

Is it really a file named "gamma" giving you problems? Your error code should tell you which files are not matching you mesh. Anyhow, here is an example from a case of mine (variable and size will not match yours). I'm pretty sure that the file giving you trouble will look something like this

FoamFile
{
    version     2.0;
    format      ascii;
    class       volVectorField;
    location    "686";
    object      U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 1 -1 0 0 0 0];

internalField   nonuniform List<vector> 
40707
(
(5.75351e-08 1.78608e-13 -1.29983e-08)
(4.34756e-08 -1.68768e-11 1.1458e-08)
(6.87797e-08 -1.31685e-11 -1.64066e-08)
(1.26222e-07 1.20794e-11 -2.15262e-09)
(8.19207e-08 6.92902e-12 1.65675e-08)
(3.25676e-08 -2.42031e-11 -9.9565e-10)
(3.88896e-07 -1.56001e-11 3.71109e-08)
(3.39852e-07 7.24725e-12 1.21746e-08)
(3.42452e-07 1.10985e-11 7.22658e-09)
[...]
(1.25084e-06 -1.60452e-10 1.37135e-09)
(1.16599e-06 6.83278e-11 -6.65523e-09)
(1.25118e-06 1.34288e-10 1.54835e-09)
(1.16659e-06 -2.39878e-11 2.30208e-09)
)
;

boundaryField
{
    front
    {
        type            slip;
    }
    back
    {
        type            slip;
    }
    inlet
    {
        type            fixedValue;
        value           nonuniform List<vector> 
            92
            (
            (3.9921e-07 9.41269e-12 3.60087e-08)
            (9.47981e-07 -1.95452e-12 4.31057e-08)
            (1.35416e-06 -1.04229e-11 3.00812e-08)
            [...]
            (1.16941e-06 -5.50304e-11 4.28134e-08)
            (1.2247e-06 -3.0136e-10 4.27937e-08)
            );
    }
    
    outlet
    {
        type            inletOutlet;
        inletValue      uniform (0 0 0);
        value           nonuniform List<vector> 
            74
            (
            (4.53798e-07 -2.58165e-10 4.07981e-08)
            (9.47981e-07 -1.95452e-12 4.31057e-08)
            [...]
            (1.58258e-06 -1.05756e-14 4.61522e-09)
            (1.05566e-06 2.77257e-11 4.06847e-08)
            (1.05562e-06 5.70094e-11 4.06854e-08)
            (9.4798e-07 7.00389e-12 4.30221e-08)
            );
    }
    
    top
    {
        type            slip;
    }
    
    lowerWall
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }
}

It contains data from a previous run or timestep. In total my file contains 40707 points for the internal field and a few points for a patch called inlet and outlet. If i would copy this file into a different case where the internal mesh does not have 40707 points in the internalField i would get an error like you. It might read "size 40707 is not equal to the given value of 4096" or something like that. If i remove all data points from my file i get a variable file containing only the bounary conditions. Like this:

FoamFile
{
    version     2.0;
    format      ascii;
    class       volVectorField;
    location    "1";
    object      U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 1 -1 0 0 0 0];

internalField   uniform (0.000625 0 0);

boundaryField
{
    bottom
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }
    top
    {
        type            slip;
    }
    inlet
    {
        type            cyclic;
    }
    outlet
    {
        type            cyclic;
    }
    front
    {
        type            slip;
    }
    back
    {
        type            slip;
    }
    lowerWall
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }
 }

Try it for your own files and boundary conditions. I'd be surprised if it doesnt fix your problems.

If you need further help,dont hesitate to ask, but provide more detail. For example post the error OpenFoam gives you. Or post the file that gives your problems.

[A H Gazi]

Originally Posted by RobertHB

Is it really a file named "gamma" giving you problems? Your error code should tell you which files are not matching you mesh. Anyhow, here is an example from a case of mine (variable and size will not match yours). I'm pretty sure that the file giving you trouble will look something like this

FoamFile
{
    version     2.0;
    format      ascii;
    class       volVectorField;
    location    "686";
    object      U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 1 -1 0 0 0 0];

internalField   nonuniform List<vector> 
40707
(
(5.75351e-08 1.78608e-13 -1.29983e-08)
(4.34756e-08 -1.68768e-11 1.1458e-08)
(6.87797e-08 -1.31685e-11 -1.64066e-08)
(1.26222e-07 1.20794e-11 -2.15262e-09)
(8.19207e-08 6.92902e-12 1.65675e-08)
(3.25676e-08 -2.42031e-11 -9.9565e-10)
(3.88896e-07 -1.56001e-11 3.71109e-08)
(3.39852e-07 7.24725e-12 1.21746e-08)
(3.42452e-07 1.10985e-11 7.22658e-09)
[...]
(1.25084e-06 -1.60452e-10 1.37135e-09)
(1.16599e-06 6.83278e-11 -6.65523e-09)
(1.25118e-06 1.34288e-10 1.54835e-09)
(1.16659e-06 -2.39878e-11 2.30208e-09)
)
;

boundaryField
{
    front
    {
        type            slip;
    }
    back
    {
        type            slip;
    }
    inlet
    {
        type            fixedValue;
        value           nonuniform List<vector> 
            92
            (
            (3.9921e-07 9.41269e-12 3.60087e-08)
            (9.47981e-07 -1.95452e-12 4.31057e-08)
            (1.35416e-06 -1.04229e-11 3.00812e-08)
            [...]
            (1.16941e-06 -5.50304e-11 4.28134e-08)
            (1.2247e-06 -3.0136e-10 4.27937e-08)
            );
    }
    
    outlet
    {
        type            inletOutlet;
        inletValue      uniform (0 0 0);
        value           nonuniform List<vector> 
            74
            (
            (4.53798e-07 -2.58165e-10 4.07981e-08)
            (9.47981e-07 -1.95452e-12 4.31057e-08)
            [...]
            (1.58258e-06 -1.05756e-14 4.61522e-09)
            (1.05566e-06 2.77257e-11 4.06847e-08)
            (1.05562e-06 5.70094e-11 4.06854e-08)
            (9.4798e-07 7.00389e-12 4.30221e-08)
            );
    }
    
    top
    {
        type            slip;
    }
    
    lowerWall
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }
}

It contains data from a previous run or timestep. In total my file contains 40707 points for the internal field and a few points for a patch called inlet and outlet. If i would copy this file into a different case where the internal mesh does not have 40707 points in the internalField i would get an error like you. It might read "size 40707 is not equal to the given value of 4096" or something like that. If i remove all data points from my file i get a variable file containing only the bounary conditions. Like this:

FoamFile
{
    version     2.0;
    format      ascii;
    class       volVectorField;
    location    "1";
    object      U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 1 -1 0 0 0 0];

internalField   uniform (0.000625 0 0);

boundaryField
{
    bottom
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }
    top
    {
        type            slip;
    }
    inlet
    {
        type            cyclic;
    }
    outlet
    {
        type            cyclic;
    }
    front
    {
        type            slip;
    }
    back
    {
        type            slip;
    }
    lowerWall
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }
 }

Try it for your own files and boundary conditions. I'd be surprised if it doesnt fix your problems.

If you need further help,dont hesitate to ask, but provide more detail. For example post the error OpenFoam gives you. Or post the file that gives your problems.

I got it, the error has gone now.Thank you very much for your detail explanation,I really appreciate.