[Nafiz375]

I'm using openFoam v2306 and trying to calculate the gradients of velocity fields during each iteration. I have used the code below in system/controlDict:

grad1
{
        type            grad; 
        libs            (fieldFunctionObjects); 
        field
        {
            U; 
        }
		enabled         true;
		log             true;
		timeStart       0;
		timeEnd         4000;
		executeControl  timeStep;
		executeInterval 1;
		writeControl    timeStep;
		writeInterval   100;    
}

But I couldn't find any results in the saving files (i.e., 100,200 ... iterations). How can I solve this issue, any suggestions?

[Yann]

Hello Nafiz,

There is a syntax error in your function definition. You should not even be able to run the solver.

Your field parameter should be defined like this:

field			U;

You can have a look at the documentation, and check the tutorials mentioned in it: https://doc.openfoam.com/2306/tools/...ts/field/grad/

Cheers,
Yann

[nnprashant]

grad1
{
// Mandatory entries
type grad;
libs (fieldFunctionObjects);
field U;

// Optional (inherited) entries
result gradU;
region region0;
enabled true;
log true;
timeStart 0.25;
timeEnd 1000;
executeControl timeStep;
executeInterval 5;
writeControl timeStep;
writeInterval 25;
}

This should resolve your isse

[Nafiz375]

Hello
I've modified the code and still I couldn't find any results. Where should I be able to check the results. The modified code:

application     simpleFoam;

startFrom       latestTime;
startTime       0;
stopAt          endTime;
endTime         100;
deltaT          1;
writeControl    timeStep;
writeInterval   100;
purgeWrite      0;
writeFormat     binary;
writePrecision  12;
writeCompression uncompressed;
timeFormat      general;
timePrecision   6;
runTimeModifiable yes;

grad1
{
// Mandatory entries
type grad;
libs (fieldFunctionObjects);
field U;

// Optional (inherited) entries
result gradU;
region region0;
enabled true;
log true;
timeStart 0;
timeEnd 100;
executeControl timeStep;
executeInterval 1;
writeControl timeStep;
writeInterval 100;
}

[Yann]

You should have a new gradU variable (file) in your timestep directories.
Did you re-run your simulation?

[Yann]

Originally Posted by Nafiz375

application     simpleFoam;

startFrom       latestTime;
startTime       0;
stopAt          endTime;
endTime         100;
deltaT          1;
writeControl    timeStep;
writeInterval   100;
purgeWrite      0;
writeFormat     binary;
writePrecision  12;
writeCompression uncompressed;
timeFormat      general;
timePrecision   6;
runTimeModifiable yes;

grad1
{
// Mandatory entries
type grad;
libs (fieldFunctionObjects);
field U;

// Optional (inherited) entries
result gradU;
region region0;
enabled true;
log true;
timeStart 0;
timeEnd 100;
executeControl timeStep;
executeInterval 1;
writeControl timeStep;
writeInterval 100;
}

This is not the proper syntax. Your function object should be enclosed in a functions {} block.

Please check the syntax here: https://doc.openfoam.com/2306/tools/...ects/#run-time

[Nafiz375]

Hello Yann,
Yes I rerun the simulation after modifying the code.
Still, I couldn't find any results in the timestep. Only epsilon, K, Nut, P,phi and U are available.
What to do ?
Best Nafiz

[Nafiz375]

Hello Yann,
This the modified code:

functions
{
	gradU
	{
		// Mandatory entries
		type grad;
		libs (fieldFunctionObjects);
		field U;

		// Optional (inherited) entries
		result gradU;
		region region0;
		enabled true;
		log true;
		timeStart 0;
		timeEnd 100;
		executeControl timeStep;
		executeInterval 1;
		writeControl timeStep;
		writeInterval 100;
	}
}

But now my simulation stops after iteration 1. This error appears:

Time = 1

smoothSolver:  Solving for Ux, Initial residual = 1, Final residual = 0.0240735220355, No Iterations 1
smoothSolver:  Solving for Uy, Initial residual = 1, Final residual = 0.02458226803, No Iterations 1
smoothSolver:  Solving for Uz, Initial residual = 0.999999999999, Final residual = 0.0136152165375, No Iterations 1
GAMG:  Solving for p, Initial residual = 1, Final residual = 0.0910537418564, No Iterations 11
time step continuity errors : sum local = 1.04300070627e-05, global = 3.76833088599e-06, cumulative = 3.76833088599e-06
smoothSolver:  Solving for epsilon, Initial residual = 1, Final residual = 0.0561016871376, No Iterations 4
smoothSolver:  Solving for k, Initial residual = 1, Final residual = 0.0604477590299, No Iterations 4
ExecutionTime = 3.45 s  ClockTime = 4 s



--> FOAM FATAL ERROR: (openfoam-2306)
Attempted non-const reference to const object: tmp<N4Foam14GeometricFieldINS_6TensorIdEENS_12fvPatchFieldENS_7volMeshEEE>

    From T& Foam::tmp<T>::ref() const [with T = Foam::GeometricField<Foam::Tensor<double>, Foam::fvPatchField, Foam::volMesh>]
    in file ./src/OpenFOAM/lnInclude/tmpI.H at line 255.

FOAM aborting

[stack trace]
=============
#1  Foam::error::simpleExit(int, bool)sh: 1: addr2line: not found
 addr2line failed
#2  ?sh: 1: addr2line: not found
 addr2line failed
#3  ?sh: 1: addr2line: not found
 addr2line failed
#4  Foam::functionObjects::grad::calc()sh: 1: addr2line: not found
 addr2line failed
#5  Foam::functionObjects::fieldExpression::execute()sh: 1: addr2line: not found
 addr2line failed
#6  Foam::functionObjects::timeControl::execute()sh: 1: addr2line: not found
 addr2line failed
#7  Foam::functionObjectList::execute()sh: 1: addr2line: not found
 addr2line failed
#8  Foam::Time::run() constsh: 1: addr2line: not found
 addr2line failed
#9  Foam::Time::loop()sh: 1: addr2line: not found
 addr2line failed
#10  ?sh: 1: addr2line: not found
 addr2line failed
#11  ?sh: 1: addr2line: not found
 addr2line failed
#12  __libc_start_mainsh: 1: addr2line: not found
 addr2line failed
#13  ?sh: 1: addr2line: not found
 addr2line failed
=============
Aborted (core dumped)

[Yann]

Not sure about your error.

I don't think this is related, but you can remove these lines:

timeStart 0;
timeEnd 100;

It doesn't make sense to stop the function at 100 iterations since you are asking to write the result every 100 iterations.

In order to sort things out, you can also try to remove these ones:

result gradU;
region region0;

[Nafiz375]

Hello Yann,
Still, the same issue exists. The updated code is:
system/controlDict:

application     simpleFoam;
startFrom       latestTime;
startTime       0;
stopAt          endTime;
endTime         100;
deltaT          1;
writeControl    timeStep;
writeInterval   50;
purgeWrite      0;
writeFormat     binary;
writePrecision  12;
writeCompression uncompressed;
timeFormat      general;
timePrecision   6;
runTimeModifiable yes;

functions
{
	gradU
	{
		// Mandatory entries
		type grad;
		libs (fieldFunctionObjects);
		field U;
		// Optional (inherited) entries
		enabled true;
		log true;
		executeControl timeStep;
		executeInterval 1;
		writeControl timeStep;
		writeInterval 50;
	}
}

[Yann]

Not sure what is going on, the function definition looks OK.

[Nafiz375]

Thanks, YANN, for the comments.

The above problem was solved. I just deleted some lines from system/fvSolution:

cache
{
    grad(U);
}