[kjgrzywnowicz]

Hello everyone,

I would like to post my experience, because I have not seen it here on CFD-Online before. I hope it might help someone in the future.

I was trying to perform simulation of thermal solar water collector, with two different sources of radiation. First source was the direct solar radiation, derived onto upper part of the (cylindrical) pipe, forming the absorber, whereas the second source - concentrated solar radiation (approx. 5-6 times the direct radiation) derived onto the lower part of the pipe.

Absorber was filled with circulating fluid (water at high pressure).

In order to limit the thermal conduction between the parts, I have partially separated the upper and lower part of pipe with a thin thermal insulator as the third domain (solid type), which has been treated simply as an obstacle (excluded from thermal modeling).

As I was trying to run the simulation, during the very first iteration I got such error message:


ERROR #001100279 has occurred in subroutine ErrAction.
Message:
Stopped in routine WALK


This situation occured for Monte Carlo radiation model and Conservative Interface Flux boundary at the interface. Swithing to the Opaque model enabled running the model without such an error, but with limited convergence concerning the RMS T-Energy variable.

After detailed analysis of the physics model, I have found the reason for such error. During automatic generation of the solid-solid interface (between upper and lower parts of the absorber pipe), CFX has selected not only the faces directly contacting each other, but the faces contacting the thermal insulator as well. Since, the insulator has not been thermally modeled, physically it introduced just a narrow gap between the upper and lower parts of pipe. Nevertheless, the gap was too wide, to handle it as the interface - therefore, the CFX-Solver during analysis of the model, failed to initialize the solid-solid interface.

When I have manually corrected the interfaces, the model ran easily.
So, I guess, that any error within the WALK routine is somehow connected to the interface connection checking for radiation heat transfer - when you get it, carefully check the interfaces within your model or switch to opaque boundaries wherever it is possible without strong violation of physics you want to model.

[ghorrocks]

Are you sure you need the Monte Carlo radiation model? It is a very expensive model and will make your simulations MUCH slower. It is also difficult to achieve mesh independent results on. If the radiation is directional but there is no complex physics other than that you should use the Discrete Transfer model. It runs much quicker and is easier to obtain good results with. By no complex physics I mean something which requires ray tracing, such as absorption in the fluid, wavelength effects and so on.

You should also make sure you do not have a radiation model in your thermal insulation layer. Then the radiation model will use the solid/fluid interface as a wall boundary.