[AJAY BHANDARI]

Hi all,

I think my problem is similar as described above. I have to input a time varying variable Cp whose value is changing with time not space. I have 32 time points and 32 values of Cp. these values are listed in a text file and i have to read it from there..

Basically i am simulating a convection diffusion equation . I am pasting the code for better understanding...

solve
(
fvm::ddt(C)
+ (1/por)*fvm::div(phi, C)
- fvm::laplacian(D, C)
+ fvm::Sp((ktrans/por), C)
+ fvm::Sp((lfc/por)*(p-lp), C)
==
(ktrans*Cp)

);

In here Cp term (basically its concentration in moles) on RHS is time varying and changing for 32 time points.
My problem is how i enter the time varying values of Cp as i am simulating this eqn for 32 time points to get C at each time point (total time 128 seconds with time difference of 4 sec so total 32 time points). I have list of 32 values of Cp for 32 time points... How I enter them for each time point?? or how i read my text file. I am pasting my text file also for better understanding..
time(sec) concentration(moles)
4 0.0
8 0.0
12 0.0
16 0.0
20 0.0
24 0.10108117
28 1.0127527
32 2.0
36 1.557599
40 1.131114
44 1.1927048
48 1.289628
52 1.295573
56 1.140025
60 1.038649
64 1.0607834
68 1.1071031
72 1.0575966
76 1.0918694
80 1.0274673
84 1.005336
88 0.9897777
92 0.93968034
96 0.932393
100 0.8909937
104 0.93785316
108 0.8845323
112 0.91211754
116 1.0066646
120 0.92081094

Any help will be appreciated...

Regards
Ajay

[wyldckat]

Greetings Ajay,

I've moved your post from the other thread: http://www.cfd-online.com/Forums/ope...ampledict.html - to this new one, since the problems are somewhat different.

The first problem is determining if you are solving a 0D or a 1D equation. I ask this because this affects how the "Cp" field is provided, as well as the other fields, such as C and D.

Therefore, please provide more details about the case set-up you have. I ask this because the "Cp" field should either be:

1. Using a boundary condition that allows for this field change;
2. or perhaps it's best to use a "swakExpression" (you will need to install swak4Foam for this) to modify the field based on the txt file.

Best regards,
Bruno

[AJAY BHANDARI]

Hi,

Thanks bruno for your quick reply.. Regarding your questions..

I am simulating a body tissue which is basically porous media. The above equation is basically a 3D equation means i am simulating C (concentration in tissue) in 3D. It is a volScalarField.

D is diffusion constant and its value is 1e-09 and is uniform all over the mesh.
ktrans and por are permeability coefficient and porosity which is non uniform and has been input on each cell in mesh.
Mesh is rectangular with 45,30,10 cells in x,y,z directions respectively.
pressure and velocity have been solved earlier by continuity and momentum equations.
Now problem is that i am simulating the above equation for 30 time steps starting from 0 to 120 sec at interval of 4 sec. And at each time step Cp(concentration in capillaries) term is changing and i have a list of values which i have already mentioned above. I just want to read this text file and update Cp term at each time step to calculate C at each time step.

Hope you understand

Regards
Ajay

[wyldckat]

Hi Ajay,

Without a working code to work on, I'll have to rely on a few quick notes:

1. Based on the code from the boundary condition "uniformFixedValueFvPatchField" ("src/finiteVolume/fields/fvPatchFields/derived/uniformFixedValue"), the following chunks of code will be needed:
   

   autoPtr<DataEntry<Type> > uniformValue_;
   
   uniformValue_(DataEntry<Type>::New("uniformValue", dict))
   {
       const scalar t = this->db().time().timeOutputValue();
       fvPatchField<Type>::operator==(uniformValue_->value(t));

2. From "applications/utilities/preProcessing/dsmcInitialise/dsmcInitialise.C":
   

       IOdictionary dsmcInitialiseDict
       (
           IOobject
           (
               "dsmcInitialiseDict",
               mesh.time().system(),
               mesh,
               IOobject::MUST_READ_IF_MODIFIED,
               IOobject::NO_WRITE
           )
       );

3. Putting things together in code:
   1. In the creation section:
      

      IOdictionary cpDict
      (
          IOobject
          (
              "cpDict",
              mesh.time().constant(),
              mesh,
              IOobject::MUST_READ,
              IOobject::NO_WRITE
          )
      );
      
      
      autoPtr<DataEntry<scalar> > cpValue(DataEntry<scalar>::New("cpValue", cpDict));

   2. In the calculation section, before using "Cp":
      

      Cp = cpValue->value(mesh.time().timeOutputValue()));

4. The following files are examples that this code should be able to process:
   1. The dictionary file "constant/cpDict" with the data settings:
      

      cpValue     tableFile;       
      cpValueCoeffs       
      {       
          fileName     "$FOAM_CASE/myDataFile"
          outOfBounds  clamp;       
      }

      Note: The solver will complain about the missing header in this file, which is just a matter of copy-pasting the stuff it tells you into the beginning of this file.
   2. The file "myDataFile" should be placed in the base case folder and is based on your text file, but reformatted like this:
      

      (
        (4 0.0)
        (8 0.0)
        (12 0.0)
        (16 0.0)
        (20 0.0)
        (24 0.10108117)
        (28 1.0127527)
        (32 2.0)
        (36 1.557599)
        (40 1.131114)
        (44 1.1927048)
        (48 1.289628)
        (52 1.295573)
        (56 1.140025)
        (60 1.038649)
        (64 1.0607834)
        (68 1.1071031)
        (72 1.0575966)
        (76 1.0918694)
        (80 1.0274673)
        (84 1.005336)
        (88 0.9897777)
        (92 0.93968034)
        (96 0.932393)
        (100 0.8909937)
        (104 0.93785316)
        (108 0.8845323)
        (112 0.91211754)
        (116 1.0066646)
        (120 0.92081094)
      );

      Source: http://www.cfd-online.com/Forums/ope...tml#post350763 post #2

Don't forget to build the solver again. With any luck, this works at first try... but I doubt it, since I didn't have a base work code to work with.


Best regards,
Bruno

[AJAY BHANDARI]

Hi bruno,

Thanks for your help. I did exactly as you have mentioned. I built the solver again. Solver was compiled succesfully. But when i am running the case Its giving following error..

    
--> FOAM FATAL ERROR: 
Different dimensions for =
     dimensions : [0 0 0 0 1 0 0] = [0 0 0 0 0 0 0]


    From function dimensionSet::operator=(const dimensionSet&) const
    in file dimensionSet/dimensionSet.C at line 171.

FOAM aborting

#0  Foam::error::printStack(Foam::Ostream&) at ??:?
#1  Foam::error::abort() at ??:?
#2  Foam::dimensionSet::operator=(Foam::dimensionSet const&) const at ??:?
#3  ? at ??:?
#4  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#5  ? at ??:?
Aborted (core dumped)

I have checked all the dimensions twice.. I don't know where is the error now. But i think error is in this line

              
Cp = cpValue->value(mesh.time().timeOutputValue()));

Because It compiled succesfully without any dimension error when i was doing it previously without this method but obviously results were not correct.. Please suggest...

Regards
Ajay

[wyldckat]

Hi Ajay,

Originally Posted by AJAY BHANDARI

Because It compiled succesfully without any dimension error when i was doing it previously without this method but obviously results were not correct.. Please suggest...

Even if it compiles, it doesn't mean it will run properly .

Knowing how you defined the Cp variable would make it easier to give a proper solution.
Either way, the problem is that it cannot be a "scalar", it has to be "dimensionedScalar"... let me see if I can find an example in OpenFOAM's code... here's a command that helps find several examples:

find $FOAM_UTILITIES $FOAM_SOLVERS -name "*.[CH]" -type f | xargs grep dimensionedScalar

Drawing from a few files, something like this might work:

dimensionedScalar Cp("Cp", dimEnergy/dimTemperature, 0.0);
dimensionedScalar Cp("Cp", dimensionSet(0, 2, -1 , 0, 0), 0.0);

Note: These are just examples. I didn't go check what units are "Cp" meant to be .

Best regards,
Bruno

[AJAY BHANDARI]

Hi bruno,

I didn't get it means you are saying that in createfields.h file i replace this

    Info<< "Reading field Cp\n" << endl;
    volScalarField Cp
    (
        IOobject
        (
            "Cp",
            runTime.timeName(),
            mesh,
            IOobject::MUST_READ,
            IOobject::AUTO_WRITE
        ),
        mesh
    );

by this

dimensionedScalar Cp("Cp", dimensionSet(0 0 0 0 1 0 0), 0.0);

or where i should put the above line of code in my case??

[AJAY BHANDARI]

Hi bruno,

I have done the following changes in createFields,h

   IOdictionary cpDict
   (
      IOobject
      (
           "cpDict",
          mesh.time().constant(),
          mesh,
          IOobject::MUST_READ,
          IOobject::NO_WRITE
      )
   );


autoPtr<DataEntry<scalar> > cpValue(DataEntry<scalar>::New("cpValue", cpDict));
    

    dimensionedScalar Cp  
    (
          cpDict.lookup("Cp")
    );

and in constant cpDict file

Cp        Cp    [0 0 0 0 1 0 0]    0;

cpValue     tableFile;       
cpValueCoeffs       
{       
    fileName     "$FOAM_CASE/myDataFile"
    outOfBounds  clamp;       
}

myDataFile has been put in a folder in case according to same format..
Solver is compiling but again case is not running and now error is

--> FOAM FATAL IO ERROR: 
error in IOstream "/home/ajay/OpenFOAM/ajay-2.4.0/run/tutorials/incompressible/porousSimpleFoam/cncrnozeroporositytime/myDataFile" for operation operator>>(Istream&, List<T>&) : reading first token

file: /home/ajay/OpenFOAM/ajay-2.4.0/run/tutorials/incompressible/porousSimpleFoam/cncrnozeroporositytime/myDataFile at line 1.

    From function IOstream::fatalCheck(const char*) const
    in file db/IOstreams/IOstreams/IOstream.C at line 114.

FOAM exiting

I am not understanding now. Is something wrong with myDataFile format. Please suggest..

Regards
Ajay

[wyldckat]

Hi Ajay,

That is very strange.... why did you try those lines of code that are not exactly as the examples I had given?

The following should work:

   IOdictionary cpDict
   (
      IOobject
      (
           "cpDict",
          mesh.time().constant(),
          mesh,
          IOobject::MUST_READ,
          IOobject::NO_WRITE
      )
   );


autoPtr<DataEntry<scalar> > cpValue(DataEntry<scalar>::New("cpValue", cpDict));
    
dimensionedScalar Cp("Cp", dimensionSet(0, 0, 0, 0, 1, 0, 0), 0.0);

And then when updating the value:

Cp = cpValue->value(mesh.time().timeOutputValue());

Best regards,
Bruno

[AJAY BHANDARI]

Hi bruno,

FIrst a very happy new year to you..

I have done the same thing many times. i Have used the same code as you described above and compiled but again the error is same

   Different dimensions for =
     dimensions : [0 0 0 0 1 0 0] = [0 0 0 0 0 0 0]


    From function dimensionSet::operator=(const dimensionSet&) const
    in file dimensionSet/dimensionSet.C at line 171.

FOAM aborting

#0  Foam::error::printStack(Foam::Ostream&) at ??:?
#1  Foam::error::abort() at ??:?
#2  Foam::dimensionSet::operator=(Foam::dimensionSet const&) const at ??:?
#3  ? at ??:?
#4  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#5  ? at ??:?
Aborted (core dumped)

I have checked my case many times for dimensions . I have created dictionary in createFields.h I have created cpdict in constant and created myDataFile in case according to same format.. about updating Cp values in calculation section i have done it before using Cp.

    Cp = cpValue->value(mesh.time().timeOutputValue());

                  solve
                  (
                         fvm::ddt(C) 
                       + (1/por)*fvm::div(phi, C) 
                       - fvm::laplacian(D, C) 
                       + fvm::Sp((ktrans/por), C) 
                       + fvm::Sp((lfc/por)*(p-lp), C) 
                      == 
                        (ktrans*Cp)

                 );

I am not clear about one thing why in error its not mentioning which dimensions are wrong or where is the error now...

Regards
Ajay

[AJAY BHANDARI]

Hi bruno,

Mission accomplished. There was minor error . Instead of this

Cp = cpValue->value(mesh.time().timeOutputValue());

It should be

Cp.value() = cpValue->value(mesh.time().timeOutputValue());

It ran.. Thanks for the help and happy new year....

[wyldckat]

Hi Ajay,

I'm glad you managed to figure it out! I only did a quick test yesterday and it seemed to have worked for me, but I didn't do much more testing with it.

And a Happy New Year!
Best regards,
Bruno