[paolovescovo]

Good evening, i am new in this forum.

I am trying to implement and chtMultiRegionFOAM-solve a thermal contact problem between two solids in OpenFOAM 2.3.0 (due to some troubles between ParaView and the OpenGL that suit my PC graphic card, troubles i am working about too).

The undesired result is that it seems to me that the simulation just does not start and with no visibile log to me. Is there a way to make the solver output what is going on in detail?

Here attached You can find two archives: the only difference i expect You to find is that in version 01 distinct nodes coincide at the same points in the space on the boundary between the two solids while in version 02 every space point hosts one node.

[wyldckat]

Greetings Paolo and welcome to the forum!


I've only looked at the case "01" and there are two problems with it:

1. It is defined to use adjustable time steps, based on maxCo and maxDi, which is why it simply jumps a time step larger than your end time of 0.5, namely the output was:
   

   Region: corpo1 Diffusion Number mean: 3.0963523e-06 max: 3.0965588e-06
   Region: corpo2 Diffusion Number mean: 2.7777778e-07 max: 2.7777778e-07
   deltaT = 322.93913
   End

2. After changing the following settings:
   

   writeControl    runTime;
   adjustTimeStep  no;

   It then crashes on the very first time step, because it complains that it is missing the "phi" field.
3. The reason is because you are trying to use the boundary condition "inletOutlet" in the "p" field, but "inletOutlet" only works if there is fluid velocity, which does not exist in the solid regions. Therefore you should only use the type "fixedValue" instead of "inletOutlet".

As for the problems with OpenGL, I know that you are using blueCFD-Core 2.3-1 from emails we have exchanged in the past and due to the log files in the cases you attached.

Therefore, you can install a more recent blueCFD-Core version (2016-2 or 2017-2) that provides a more recent version of OpenFOAM (4.x and 5.x, respectively) that has this bug fixed. Then you can install another version of ParaView, namely version 4.4, by following the instructions provided here: http://bluecfd.github.io/Core/FAQ/ho...n-of-ParaView/

Best regards,
Bruno