[qingqingliu]

I am learning the programming in interCondensatingEvaporatingFoam solver. In the constant folder, the following is used to define T:
const volScalarField& T = mesh_.lookupObject<volScalarField>("T");
I am wondering what the "mesh_" mean?

In the other solver, interPhaseChangeFoam, they use the following to define p:
const volScalarField& p = alpha1_.db().lookupObject<volScalarField>("p")

One uses mesh_, while the other one uses alpha1_.db(), what are the differences between these two terms?

[Severus]

Hello,
We will make full use of the API guide (Doxygen) to understand.

objectRegistry and lookupObject
With both mesh_ and db you call the lookupObject member function. Note that lookupObject is a member function in the objectRegistry class: https://www.openfoam.com/documentati...ce.html#l00541. For the documentation regarding lookupObject member function, see line 482 - https://www.openfoam.com/documentati...8H_source.html

You can understand the objectRegistry better here: https://openfoamwiki.net/index.php/Contrib/IOReferencer

mesh_ and db
mesh_ is a reference to the fvMesh class defined in temperaturePhaseChangeTwoPhaseMixture class. See line 69: https://www.openfoam.com/documentati...ce.html#l00068
You are able to access mesh_ in the constant class because the constant class inherits temperaturePhaseChangeTwoPhaseMixture class (https://www.openfoam.com/documentati...1constant.html)

db is also a reference to the objectRegistry class, but is defined in IOobject.H class (https://www.openfoam.com/documentati...8H_source.html)

In other words, in both the cases you are calling the lookupObject member function of the objectRegistry class but with different instances that have been created from the derived classes. With both you are able to access all your field variables such as temperature and pressure in the mesh.

I am not an expert in C++, so feel free to correct me if I messed up somewhere.

Thanks

[qingqingliu]

Originally Posted by Severus

Hello,
We will make full use of the API guide (Doxygen) to understand.

objectRegistry and lookupObject
With both mesh_ and db you call the lookupObject member function. Note that lookupObject is a member function in the objectRegistry class: https://www.openfoam.com/documentati...ce.html#l00541. For the documentation regarding lookupObject member function, see line 482 - https://www.openfoam.com/documentati...8H_source.html

You can understand the objectRegistry better here: https://openfoamwiki.net/index.php/Contrib/IOReferencer

mesh_ and db
mesh_ is a reference to the fvMesh class defined in temperaturePhaseChangeTwoPhaseMixture class. See line 69: https://www.openfoam.com/documentati...ce.html#l00068
You are able to access mesh_ in the constant class because the constant class inherits temperaturePhaseChangeTwoPhaseMixture class (https://www.openfoam.com/documentati...1constant.html)

db is also a reference to the objectRegistry class, but is defined in IOobject.H class (https://www.openfoam.com/documentati...8H_source.html)

In other words, in both the cases you are calling the lookupObject member function of the objectRegistry class but with different instances that have been created from the derived classes. With both you are able to access all your field variables such as temperature and pressure in the mesh.

I am not an expert in C++, so feel free to correct me if I messed up somewhere.

Thanks

Thanks for the explanation. Do you think the following two definitions will get the same "p"? I am modifying a solver, but get the wrong results. I am not sure if the definition of "p" caused the problem.

const volScalarField& p = alpha1_.db().lookupObject<volScalarField>("p")
const volScalarField& p = mesh_.lookupObject<volScalarField>("p")

[Severus]

Hello,
I think it should be the same. But we can check it out.

const volScalarField& p1 = alpha1_.db().lookupObject<volScalarField>("p")
const volScalarField& p2 = mesh_.lookupObject<volScalarField>("p")

Then you can print these fields and open it and check, or even check in Paraview.

Let us say you want to write it out every output time, then use the following,

 if(runTime.outputTime())
 {
 p1.write();
 p2.write();
 }

You can even subtract these fields to see if they are zero (or machine precision value)

Thanks

[qingqingliu]

Originally Posted by Severus

Hello,
I think it should be the same. But we can check it out.

const volScalarField& p1 = alpha1_.db().lookupObject<volScalarField>("p")
const volScalarField& p2 = mesh_.lookupObject<volScalarField>("p")

Then you can print these fields and open it and check, or even check in Paraview.

Let us say you want to write it out every output time, then use the following,

 if(runTime.outputTime())
 {
 p1.write();
 p2.write();
 }

You can even subtract these fields to see if they are zero (or machine precision value)

Thanks

Thanks for your help. I will check.

[olesen]

The important part to note is that most volume fields will also be registered onto the corresponding volume mesh (ie, polyMesh, which is also an objectRegistry). Thus the db() referenced by the volume field will be identical to the mesh (or mesh.thisDb() to be even pickier).
The only current exception would be for volume internal fields for lagrangian sources. These are constructed on the mesh, but registered separately.

[olesen]

When in doubt, check things yourself. For example, print the address returned by db() and the memory location occupied by the mesh - if they have the same address, they are the same