[Dicanic]

Hi all,



I am getting an error here and I believe the relevant output is here:





(START ERROR)

codeStream : dictionary:"/home/user/OpenFOAM/user-9/mysimulation/0/region1/T" master-only-reading:0


--> FOAM FATAL IO ERROR:
wrong token type - expected Scalar, found on line 2 the word 'ٌ@33333ٌ@�\�s�x�@33333ٌ@��:.�@33333ٌ@33333ٌ@�lh�@ 33333ٌ@33333ٌ@33333ٌ@33333ٌ@33333ٌ@33333ٌ@33333ٌ@3 3333ٌ@33333ٌ@33333ٌ@�'

file: IStringStream.sourceFile at line 2.

From function Foam::Istream& Foam::operator>>(Foam::Istream&, Foam::doubleScalar&)
in file lnInclude/Scalar.C at line 101.

FOAM exiting


(END ERROR)



I am just trying out codeStream for the first time and below is my code. I am concerned it might be the wrong writeEntry command, but if anyone knows for sure let me know please. Below is my codeStream.



Thanks!

dimensions      [ 0 0 0 1 0 0 0 ];

internalField  #codeStream
{
        codeInclude
        #{
            #include "fvCFD.H"
                #include <math.h>  
        #};
        
        codeOptions
        #{
            -I$(LIB_SRC)/finiteVolume/lnInclude \
            -I$(LIB_SRC)/meshTools/lnInclude
        #};
        
        codeLibs
        #{
            -lmeshTools \
            -lfiniteVolume
        #};
        
        code
        #{
            const IOdictionary& d = static_cast<const IOdictionary&>(dict);
            const fvMesh& mesh = refCast<const fvMesh>(d.db());
            scalarField T(mesh.nCells());
            
            const scalar maxt = 90;
            const scalar core_r = 0.762; 
            const scalar avg_t = 40;
            const scalar a = (maxt - avg_t)/pow(core_r, 2);
            double r;
            
            forAll(T, i)
            {
                // Get Cell positions
                const scalar x = mesh.C()[i][0]; 
                const scalar y = mesh.C()[i][1];
                //const scalar z = mesh.C()[i][2];
                r = sqrt(pow(x, 2) + pow(y,2));
                if (r < core_r)
                {
                    T[i] = maxt - a*pow(r, 2);
                } else {
                    T[i] = avg_t;
                }
            }
            writeEntry(os, "", T);  // Write to input dictionary
        #};
};

[Dicanic]

I found that I can only set T[i] with hardcode? I am so confused right now.
If I set T[i] = 75; for example, it works.

If I set T[i] = Th; where Th is ANY variable type and even the same value (75), it will break and give me a new error

--> FOAM FATAL IO ERROR:
wrong token type - expected Scalar, found on line 2 the word '��E����@�\��\��@
��З*�@�9L��@f��Gs��@�'

Really this makes codeStream useless to me, why would it be doing this?

[Dicanic]

I am thinking this may be a memory overflow error of some sort? I have around 2 million cells. If I even add a if statement it won't work, but if I set it to a stagnant value... it does.



This one is a real head scratcher.

[Dicanic]

I have tried every iteration of the #codeStream and read all the relevant source code and combed the internet. I absolutely cannot initialize a temperature field and neither have I seen it done successfully with #codeStream.

It should be as easy as implementing these:

https://www.cfd-china.com/assets/upl...1-solution.pdf

The above examples work, but the temperature will not work in any circumstances I try. This is a very small blockmesh with 1000 cells, so it is not a memory error.

internalField #codeStream
{	
	codeInclude
	#{
		#include "fvCFD.H"
	#};
		
	codeOptions
	#{
		-I$(LIB_SRC)/finiteVolume/lnInclude \
		-I$(LIB_SRC)/meshTools/lnInclude
	#};
		
	codeLibs
	#{
		-lmeshTools \
		-lfiniteVolume
	#};
		
	code
	#{
		const IOdictionary& d = static_cast<const IOdictionary&>(dict);
		const fvMesh& mesh = refCast<const fvMesh>(d.db());
		scalarField T(mesh.nCells(), 0.);
		
		double maxt = 90;
		double avg_t = 50;
		const scalar block = 0.05;
			
		forAll(T, i)
		{
			// Get Cell positions
			const scalar x = mesh.C()[i][0]; 
			const scalar y = mesh.C()[i][1];

			//const scalar z = mesh.C()[i][2];
			///const scalar r = pow(pow(x, 2.0) + pow(y, 2.0),0.5);
			if (x+y >= block)
			{
				T[i] = maxt;
			} else {
				T[i] = avg_t;
			}
		}
		writeEntry(os, "", T);  // Write to input dictionary
		//Pout << "Initialization of internalField"; 
	#};
};

This gives error:

on processor 0 have masterSize:826176 and localSize:826176

on processor 0 after waiting: have masterSize:826176 and localSize:826176
Opening cached dictionary:"/home/user/OpenFOAM/user-9/2DTestGround/dynamicCode/platforms/linux64GccDPInt32Opt/lib/libcodeStream_5bcb7371585e69419bfd74cf784f21d4784acc5e.so"
codeStream : dictionary:"/home/user/OpenFOAM/user-9/2DTestGround/0/T" master-only-reading:0


--> FOAM FATAL IO ERROR: 
error in IOstream "IStringStream.sourceFile" for operation operator>>(Istream&, List<T>&) : reading entry

file: IStringStream.sourceFile at line 2.

    From function void Foam::IOstream::fatalCheck(const char*) const
    in file db/IOstreams/IOstreams/IOstream.C at line 109.

FOAM exiting

[LuckyTran]

well... for starters... anything with the const type qualifier is read only

[Dicanic]

I can see how this is relevant when I add x and y together, but I get the same problem when using x alone in the boolean operator.


These snippets of code:

        const IOdictionary& d = static_cast<const IOdictionary&>(dict);
        const fvMesh& mesh = refCast<const fvMesh>(d.db());
        scalarField T(mesh.nCells(), 0.);

as well as

            const scalar x = mesh.C()[i][0]; 
            const scalar y = mesh.C()[i][1];

work in all the above tutorials but the code also only reads them so declaring them as const is appropriate as far as I can tell. The only thing I am writing to is scalarField T. For example, I could take my exact code and only change T to alpha, and it would run and I would see the results as intended. I must be referencing T incorrectly but I am not sure how.

[Dicanic]

With new code (using as few consts as possible)

internalField #codeStream
{	
	codeInclude
	#{
		#include "fvCFD.H"
	#};
		
	codeOptions
	#{
		-I$(LIB_SRC)/finiteVolume/lnInclude \
		-I$(LIB_SRC)/meshTools/lnInclude
	#};
		
	codeLibs
	#{
		-lmeshTools \
		-lfiniteVolume
	#};
		
	code
	#{
		const IOdictionary& d = static_cast<const IOdictionary&>(dict);
		const fvMesh& mesh = refCast<const fvMesh>(d.db());
		scalarField T(mesh.nCells(), 0.);
		
		scalar maxt = 90.0;
		scalar avg_t = 40.0;
		scalar block = 0.025;
			
		forAll(T, i)
		{
			// Get Cell positions
			scalar x = mesh.C()[i][0];
			scalar y = mesh.C()[i][1];

			if (x >= block)
			{
				T[i] = scalar(maxt);
			} else {
				T[i] = scalar(avg_t);
			}
		}
		T.writeEntry("", os);  // Write to input dictionary
	#};
};

--> FOAM FATAL IO ERROR: (openfoam-2106)
Bad token - could not get scalar value
file: input at line 2.
    From Foam::Istream& Foam::operator>>(Foam::Istream&, Foam::doubleScalar&)
    in file lnInclude/Scalar.C at line 141.
FOAM exiting
OpenFOAM-2106:~/OpenFOAM/user-2106/run/2DTestGround/

[LuckyTran]

you have a token error... Check all your { } ( ) pairs and ;'s

I would start with removing the semicolon at the end of your bracket for internalField

[Dicanic]

I couldn't figure it out even with trying every permutation of semicolon and brackets. I instead just used the setExprFields utility on the v2106 of OpenFOAM, and then ran it on OF 9 (as v2106 isn't very friendly with solid only chtMultiRegionFoam). If anyone figures out how to get codeStream to work with temperature, let me know. I am just flabbergasted at this error and it might be something simple that I did wrong.

Thanks for the help thus far!

[LuckyTran]

A token error is really simple indeed

[Dicanic]

I don't believe the error message is suggesting the token is actually in my dictionary and I have tried just in case. It compiles the dictionary code just fine and then makes a bad stream that gives a token error. The function it points to is not much help.

This also wouldn't necessarily make sense since this code snippet works verbatim with other scalar and vector fields as well. Thus, it might be that I am giving T the wrong datatype (I"ve tried everything here) or I am referencing T wrong.

[LuckyTran]

This

internalField
{

};

And this

internalField
{

}

Are not equivalent


It's also only one block of the dict so you may have made the same mistake elsewhere. The good news is that the parser tells you the token error is on this block (line 2).

[Dicanic]

Yes, but per my previous replies. It does not change the end result.

--> FOAM FATAL IO ERROR: 
wrong token type - expected Scalar, found on line 2 the word '�Sg��V@㛿�!V@w��c?V@lL1�Q�V@ŴJYV@���TV@��>�E'

file: IStringStream.sourceFile at line 2.

    From function Foam::Istream& Foam::operator>>(Foam::Istream&, Foam::doubleScalar&)
    in file lnInclude/Scalar.C at line 101.

FOAM exiting

Seeing I am pretty sure I didn't type �Sg��V@㛿�!V@w��c?V@lL1�Q�V@ŴJYV@���TV@��>�E on line 2, I assume it is a bad stream.

Here is my entire T dictionary

/*--------------------------------*- C++ -*----------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Version:  8
     \\/     M anipulation  |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      binary;
    class       volScalarField;
    location    "0";
    object      T;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [ 0 0 0 1 0 0 0 ];

internalField  #codeStream
{
        codeInclude
        #{
            #include "fvCFD.H"
            #include <math.h>  
        #};
        
        codeOptions
        #{
            -I$(LIB_SRC)/finiteVolume/lnInclude \
            -I$(LIB_SRC)/meshTools/lnInclude
        #};
        
        codeLibs
        #{
            -lmeshTools \
            -lfiniteVolume
        #};
        
        code
        #{
            const IOdictionary& d = static_cast<const IOdictionary&>(dict);
            const fvMesh& mesh = refCast<const fvMesh>(d.db());
            scalarField T(mesh.nCells());
            
            const scalar maxt = 90;
            const scalar core_r = 0.762; 
            const scalar avg_t = 40;
            const scalar a = (maxt - avg_t)/pow(core_r, 2);
            double r;
            
            forAll(T, i)
            {
                // Get Cell positions
                const scalar x = mesh.C()[i][0]; 
                const scalar y = mesh.C()[i][1];
                //const scalar z = mesh.C()[i][2];
                r = sqrt(pow(x, 2) + pow(y,2));
                if (r < core_r)
                {
                    T[i] = maxt - a*pow(r, 2);
                } else {
                    T[i] = avg_t;
                }
            }
            writeEntry(os, "", T);  // Write to input dictionary
        #};
}

boundaryField
{
    inlet
    {
        type            fixedValue;
        value		 uniform 40;
    }
    outlet
    {
        type            inletOutlet;
        inletValue	 uniform 40;
        value		 uniform 40;        
    }
    walls
    {
        type            zeroGradient;
    }	
}


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

Go ahead and try it, maybe something in my dependencies is incorrectly installed if it should work on a simple blockmesh case on your side. I am still hoping I have a glaring error due to my tunnel vision because I would very much love to actually use a codestream versus the setExprFields utility. Nonetheless, I have made codestream work with both U (as a vector) and alpha as a scalar and in the simple translation from alpha to T, it still produces this error.

[LuckyTran]

Your codeStream block works for me after I spent the time to manually retype it into a random case of mine in OF 2.4. You have a typo in your dict somewhere. It's that simple. Or maybe you have something extraordinary going on in your custom solver. Then I can't tell you where in the universe the token error might appear.

T.writeEntry("", os); is slightly safer to use if you continue to have trouble

I'm done

[Dicanic]

Could you post the manually retyped dict? I've looked at mine for hours and don't think I am going to find it.

T.writeEntry("", os) is for the ESI version which I have posted a dict also attempting to get it to work with that.

[mill]

Hi Dicanic
I meet the similar problem when i use codeStream to set alpha of water. It shows a fatal error:

--> FOAM FATAL IO ERROR
expected keyword 'uniform' or 'nonuniform' , found codeInclude

The version of OPenFoam is V9.

[Legacy]

I was having this issue and I changed the write format from binary to ascii and it fixed it.

[Wowbagger]

Hi Foamers,

same here.
I tried and tried and did not found my error.
I was not able to set a temperature field with codeStream.

I tried using http://www.wolfdynamics.com/wiki/pro...streamINIT.pdf
But without success.
I searched and foud differences in the writeEntry which 'only' gets my a different error, see note in the code:

Any idea to solve this?

        code
        #{
        const IOdictionary& d = static_cast<const IOdictionary&>(dict);
        const fvMesh& mesh = refCast<const fvMesh>(d.db());
        scalarField T(mesh.nCells(), 0);

            forAll(T, i)
                {
                    const scalar z = mesh.C()[i][2];
                    // T[i] = 459.634 + 139.937*z + 71.306*z^2 - 50.764*z^3 + 10.339*z^4 - 0.722*z^5;
                    
                        T[i] = 20. * z;
                                       
                }

        writeEntry(os, "", T);       // wrong token type - expected Scalar, found on line 2 the word '���'
        // T.writeEntry("", os);        // error: ‘Foam::scalarField’ {aka ‘class Foam::Field<double>’} has no member named ‘writeEntry’
        #};

Edit: This error was created by using Foundation Version 11


Best regards
Michael

[Wowbagger]

I was not able to set a temperature field with common operations.
However I helped myself with a script appyling a lot of setFields runs.

Preparing the table for the iterations is simple by using Excel, etc.
Maybe this workaround helps somebody else.

However - if one got a solution for the initial question please note it here.

#!/bin/bash
cd ${0%/*} || exit 1    # Run from this directory

# Source tutorial run functions
. $WM_PROJECT_DIR/bin/tools/RunFunctions



z=(-0.2 0.1 0.2 0.3 0.4 ... );
Temp=(459.634 474.29102268 490.08383936 506.74400344 524.02614912 ... );

for i in 0 1 2 3 4 5 ... ;
do

echo "${z[i]} & ${Temp[i]}";
            
runApplication -a foamDictionary system/porous/setFieldsDict.T  -entry regions -set "(boxToCell {box (-1 -1 ${z[i]})(1 1 60); fieldValues ( volScalarFieldValue T ${Temp[i]});});"
runApplication -a foamDictionary system/air/setFieldsDict.T     -entry regions -set "(boxToCell {box (-1 -1 ${z[i]})(1 1 60); fieldValues ( volScalarFieldValue T ${Temp[i]});});"

runApplication -a setFields -region porous -dict setFieldsDict.T
runApplication -a setFields -region air -dict setFieldsDict.T

done

Best regards
Michael

[wangsen992]

For anyone who's having similar issue, change "format" in FoamFile to "ascii" might be able to help.