[clempel]

Hello,

I am on a project on which one I want build a variation of the boundary condition of the slope. For this, I use codedFixedValue and want to retrieve the time of the simulation and the endtime of the simulation as a scalar as it runs. But I can't find the good function or syntaxe to retrieve these both values. I work on OpenFOAM 9.
Here is the code to let you understand what I want to explain.
I hope that someone can help me.
Thank you very much in advance,

Clément

/*--------------------------------*- C++ -*----------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Version:  9
     \\/     M anipulation  |
\*-----------------------------------------------------------------------------*/
FoamFile
{
    format      ascii;
    class       volScalarField;
    location    "0";
    object      T;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [ 0 0 0 1 0 0 0 ];

internalField   uniform 296.15;

boundaryField
{
    ground
    {
        type            fixedValue;
        value           uniform 296.15;
    }   

    slope
    {
    type            codedFixedValue;
    value           uniform 0;  // initial value
    name            variationHeatFlux;
    code
    #{
        #include "createTime.H"
        #include "Time.H"


        const fvPatch& patch = this->patch();
        const vectorField& cf = patch.Cf();
        scalarField& field = *this;
        forAll(cf, i)
        {
            const scalar currentTime = runTime.time();  // current time of the simulation
            const scalar endTime = runTime.endtime();  // end of the simulation
            const scalar tStart = 0;         // initial time
            const scalar gradStart = 0;    // initial gradient
            const scalar gradMax = 758.99;     // maximal gradient
            const scalar tMax = endTime/2;         // maximal gradient time (half of the simulation)
            const scalar gradDecrease = gradMax/tMax;  // decrease step after reach maximum

            scalar grad;
            if (currentTime <= tMax)
            {
                grad = gradStart + (gradMax - gradStart) * (currentTime - tStart) / (tMax - tStart);
            }
            else
            {
                grad = gradMax - gradDecrease * (currentTime - tMax) / (endTime - tMax);
            }

            field[i] = grad;
        }
    #};
    }
    ceiling
    {
        type            fixedValue;
        value           uniform 296.15;
    }
    front
    {
        type            symmetryPlane;
    }
    back //maybe here we need to use frontandback with zerogradient
    {
        type            fixedValue;
        value           uniform 296.15;
    }
    right //maybe here we need to use sideWalls with zerogradient
    {
        type            cyclic;
    }
    left
    {
        type            cyclic;
    }
}

[CFDUser29]

I am new to openfoam, but if you set a good writing step in controlDict, shouldn't it be enough ?

I notice that you might forgot a "const" before "scalar grad".

[olesen]

You mostly have the right idea except for the fatal mistake of using 'include "createTime.H"' within your code. This is definitely not what you want!
It goes off and tries to create TIme by reading the system/controlDict (every time that you call the boundary condition). It also means that that particular Time you have created corresponds to the time state at the start of the simulation.

What you do want is to go from the *this (the boundary condition) back upwards, for example:

// Starting from the fvPatchField (*this)
const Time& runTIme = this->db().time();
...

https://www.openfoam.com/documentati...atchField.html


Oh, and it would be cleaner to grab the current/end times outside of the loop! If you rework the code you'll see that it reduces down to a single value, which you can then assign to the entire field in one step.