[Marshak]

Can someone tell me what is the difference between defining

volScalarField myTemperature = thermo.T()
volScalarField mypressure = thermo.p()

and

const volScalarField& myTemperature = mesh_.lookupObject<volScalarField>("T");
const volScalarField& mypressure= mesh_.lookupObject<volScalarField>("p");

[dkxls]

Typically, in a solver that solves an energy equation (e.g. rhoPimpleFoam), the temperature is defined in the thermo class (see basicThermo.H).
You can access the field like this

const volScalarField& T = thermo.T();

(see e.g. createFields.H in the reactingFoam)

So, if you didn't implement some extra volScalarField named "T" (not quite sure if it is even possible to define two fields with the same same in the object registry), you should also be able to get access to the same field by looking it up from the object registry like this

const volScalarField& T = mesh.lookupObject<volScalarField>("T");

Note that you only get a const access to "T" from "thermo.T()".

[deepbandivadekar]

Originally Posted by dkxls

Note that you only get a const access to "T" from "thermo.T()".

Errr, what do you exactly mean by this? Can you please elaborate a little?

[Mowgli]

const is a data-type qualifier, which gives only read access within the current scope.

So, here T calculated from thermo object (returned using thermo.T() and depending on the thermophysical model chosen for the simulation) is passed by reference(&). One thus cannot change the value of T after that and is used for further computation. (Just in case you are wondering, return value of thermo.T() can be / is updated usually at the next step of computation) .

You can look up 'passing reference by const', this technique is used to save space by not creating a new object and also, not allowing code to modify it in that scope.

[Gerhard]

Hi,


I am using rhoPorousSimpleFoam and in a specified cell zone I want to modify the temperature. Looping through the cells in the cell zone, I basically want to do this:

if (alignedFlow)
{
    T[i] = T_upstream[i];
}

where alignedFlow is a check if the flow is in a certain direction an T_upstream is a temperature field which I defined (it is upstream of this cell zone I am talking about).


This code, upon compilation, gives an error (as expected) that I am trying to modify a const variable.
How can I gain access to the temperature field? In other words, I want to be able to modify the temperature in this cell zone.


Any advice will be much appreciated.

[mAlletto]

you can get rid of the const by using const_cast<volScalarField&>. you can convert a constant type to a non-constant type which can be modified.


However by doing this you get rid of a type safety. This is not done by be developer to annoy you but has a purpose.



In case of the temperature it as a dependent variable, i.e. you do not solve explicitly for the temperature. In most solvers you solve the energy equation (either enthalpy h or internal energy e depending on the choice of the user) and the temperature is calculated a thermodynamic relation.



For details see https://caefn.com/openfoam/temperature-calculation.


So before modifying the temperature be sure you are not messing around too much.

[Gerhard]

Thank you for that advice, Michael.
Perhaps a better approach would be to modify the temperature by introducing an energy source term into the specified cell zone to achieve T[i] = T_upstream[i].
I will give it some thought.