[duan]

Hi,

I am trying to set different writeTimeInterval rather than a constant one during the runTime.

for example:
if (currentRunTime<t0)
writeTimeInterval=value0;
else
writeTimeInterval=value1;

Now I have problems on how to get current time within the controlDict.

Here is my code:

writeInterval   #codeStream
{
    
    code
    #{
        /*// the sample works    
          scalar start = readScalar(dict.lookup("startTime"));
          scalar end = readScalar(dict.lookup("endTime"));
          label nDumps = 5;
          os << ((end - start)/nDumps);*/
        //==================================================
        //how to get the current time within controlDic???
          
          //Tried but Not work
          //scalar t=this->db().time().value(); 
          //error: invalid use of ‘this’ in non-member function
         
          //scalar t = runTime().value() ; 
          //error: ‘runTime’ was not declared in this scope
          //scalar t = timeDirs.last().value(); 
          //error: ‘timeDirs’ was not declared in this scope
          //scalar t = time().value(); 
          //error: too few arguments to function ‘time_t time(time_t*)
          label t0 = 0.4;
          if (t <= t0) {
                os << 0.05;
          }
          else {
                os << 0.02;
          } 
    #};
};

I also have found some post related:
http://www.cfd-online.com/Forums/ope...ntroldict.html
http://www.openfoam.org/version2.0.0...me-control.php
http://www.cfd-online.com/Forums/ope...me-scalar.html


Thanks in advance.

[alexeym]

Hi,

you'd like just to update writeInterval, depending on current time, you can create controlDict_1 with writeInterval_1, controlDict_2 with writeInterval_2 and use timeActivatedFileUpdate like below:

functions
{
    fileUpdate1
    {
        type            timeActivatedFileUpdate;
        functionObjectLibs ("libutilityFunctionObjects.so");
        outputControl   timeStep;
        outputInterval  1;
        fileToUpdate    "$FOAM_CASE/system/controlDict";
        timeVsFile
        (
            (-1    "$FOAM_CASE/system/controlDict_1")
            (10    "$FOAM_CASE/system/controlDict_2")
        );
    }
}

I.e. take your controlDict, put code snippet there, copy it to coltrolDict_1 and controlDict_2, modify writeInterval settings in controlDict_* and that's it.

[duan]

Hi, @alexeym

Thanks for your quick reply.

It works.

[duan]

For alternative,

I also wrote a script, to run the case in 3 steps:
0=>t1 ,with write time interval WI1
t1=>t2 ,with write time interval WI2
t2=>t3 ,with write time interval WI3

It's not a very good solution, but works.
If someone is interested, see the attached file.

[canopus]

Does any one know how to get

scalar t = runTime().value

in controldict to modify the writeinterval using

writeInterval #codeStream

?

I am getting the same error as reported here

system/controlDict.#codeStream:40:13: error: ‘runTime’ was not declared in this scope

[Tobi]

It's more like:

scalar t = U.runTime().value();

You only can call runTime().value() with an object. Or maybe with the Namespace::

[CarlesCQL]

Hi Tobi,

I tried

 scalar t = U.runTime().value();

and I get:

 error: ‘U’ was not declared in this scope

I searched for this topic a lot in this forum but I didn't found any solutions.

Can you elaborate a little more about that and the namespace option?

Thanks!

[aerogt3]

Originally Posted by CarlesCQL

Hi Tobi,

I tried

 scalar t = U.runTime().value();

and I get:

 error: ‘U’ was not declared in this scope

I searched for this topic a lot in this forum but I didn't found any solutions.

Can you elaborate a little more about that and the namespace option?

Thanks!

Did you ever figure this out?

[Diro7]

Originally Posted by aerogt3

Did you ever figure this out?

I didn't try myself, but you should be able to access the mesh database, and then the simulation time with something like

db().time().value()

where db() is a call from a objectRegistry object.

In the codeStream documentation (https://cpp.openfoam.org/v6/classFoa...m.html#details) there should be an example on how to access the database from within a codeStream instance:

someEntry  #codeStream
{
    code
    #{
        const IOdictionary& d = static_cast<const IOdictionary&>(dict);
        const fvMesh& mesh = refCast<const fvMesh>(d.db());

        ...
    #};
};

I guess you don't need to explicitly use namespaces or to link other libraries, but still I didn't try. Just try to put together the pieces and see if it works

Andrea

[Tobi]

If you call db() you need an object. It is the same as with U.time().value(). U is an object of e.g., volVectorField.

It is not possible to just call db().time().value(). Probably this works:

this->db().time().value();

Depending if »this« is a pointer or a reference you have to choose the point ».« operator or the other one »->«.

[Diro7]

Originally Posted by Tobi

If you call db() you need an object. It is the same as with U.time().value(). U is an object of e.g., volVectorField.

It is not possible to just call db().time().value(). Probably this works:

this->db().time().value();

Depending if »this« is a pointer or a reference you have to choose the point ».« operator or the other one »->«.

You are definitely right, my answer was a little ambiguous.
If you already have some object U like a volScalarField, then it is much easier to just call U.db().

If not, this->db() may do the job in general but since I wasn't sure about what is returned by this in a codeStream context, my suggestion was to look at the documentation and see how to retrieve the simulation database from the current dictionary.

Andrea

[Tobi]

Does not fit 100 % but here is something similar.


https://www.youtube.com/watch?v=cvWaXBnEz1U&t=1095s

[sh.yu]

Hi,

I meet the same issue here.

Does anyone know how to get the current time in the controlDict via codeStream?

[bou]

mesh().time().value();

works for me with OpenFOAM v12.

[walidta]

Hello everyone,

I am currently working with OpenFOAM 11 and previously used the solver InterCondensatingEvaporatingFoam in an older version for simulating condensation and evaporation processes. I am wondering if anyone knows the equivalent solver or method to handle condensation processes in OpenFOAM 11, as InterCondensatingEvaporatingFoam appears to no longer be available or updated.

Could anyone guide me on how to replace InterCondensatingEvaporatingFoam or suggest an alternative solver in OpenFOAM 11 that can handle both condensation and evaporation effectively?

Thank you in advance for your help!

Best regards,