[Abhishek@123]

Hi,
I am relatively new in openFoam and currently I am using chtMultiRegionFoam Solver to solve a transient case. I want to run the solver for 20 times (i.e. for 20 iterations) in a single time step and also I want to give convergence criteria in each time step. Can anyone tell me how can I do this?

[saidc.]

Hi Abhishek,

If I understood you correctly, the PIMPLE algorithm does this. With residual control you can give convergence criteria. The algorithm is in fvSolution (i.e. tutorials/heatTransfer/buoyantPimpleFoam/hotRoom/system/fvSolution) dictionary.

Lets say, you have,

PIMPLE
{    

        nNonOrthogonalCorrectors 0;     
        nCorrectors          1;    
        nOuterCorrectors    50;       

        residualControl
        {
               U
               {
                      tolerance  1e-5;
                      relTol      0;
               }
               p
               {
                      tolerance  5e-4;
                      relTol      0;
               }
         } 
}

In a single time step pimple algorithm will iterates 50 (nOuterCorrectors) times if it does not converge (residualControl) before. After 50 iterations it will move to the next time step.

Usefull links:
https://openfoamwiki.net/index.php/O...hm_in_OpenFOAM
https://www.simscale.com/forum/t/cfd...lgorithm/81418

Kind regards,
Said.

[keitaro7_14]

Originally Posted by saidc.

Hi Abhishek,

If I understood you correctly, the PIMPLE algorithm does this. With residual control you can give convergence criteria. The algorithm is in fvSolution (i.e. tutorials/heatTransfer/buoyantPimpleFoam/hotRoom/system/fvSolution) dictionary.

Lets say, you have,

PIMPLE
{    

        nNonOrthogonalCorrectors 0;     
        nCorrectors          1;    
        nOuterCorrectors    50;       

        residualControl
        {
               U
               {
                      tolerance  1e-5;
                      relTol      0;
               }
               p
               {
                      tolerance  5e-4;
                      relTol      0;
               }
         } 
}

In a single time step pimple algorithm will iterates 50 (nOuterCorrectors) times if it does not converge (residualControl) before. After 50 iterations it will move to the next time step.

Usefull links:
https://openfoamwiki.net/index.php/O...hm_in_OpenFOAM
https://www.simscale.com/forum/t/cfd...lgorithm/81418

Kind regards,
Said.

Indeed, now it is a little bit different with OF-10. If you want to perform a real PIMPLE algorithm in chtMultiRegionFoam, you need to write the following in system/fvSolution

"(PIMPLE | PISO)"
{    
  
        nOuterCorrectors    500;       

}

Then, you need to introduce the outerCorrectorResidualControl in your PIMPLE block of fvSolution corresponding to every region with your desired tolerance. Notice that if you leave some region without residual control, all nOuterCorrectors will be iterated.

PIMPLE
{    

        outerCorrectorResidualControl
        {
               U
               {
                      tolerance  1e-5;
                      relTol      0;
               }
               e
               {
                      tolerance  5e-4;
                      relTol      0;
               }
         } 
}

What chtMultiRegionFoam does with the code I have written above is to iterate the same time step 500 times for all regions, unless all regions have a residual control criterion via the outerCorrectorResidualControl subdictionary.