CFD Online Logo CFD Online URL
Home > Forums > Software User Forums > ANSYS > CFX

Error #001100279 in WALK routine - Solid/Fluid Radiation Modeling

Register Blogs Members List Search Today's Posts Mark Forums Read

LinkBack Thread Tools Search this Thread Display Modes
Old   March 16, 2020, 07:57
Default Error #001100279 in WALK routine - Solid/Fluid Radiation Modeling
New Member
Join Date: Oct 2019
Posts: 2
Rep Power: 0
kjgrzywnowicz is on a distinguished road
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.
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.

Last edited by kjgrzywnowicz; March 16, 2020 at 08:46. Reason: Requirement for correction
kjgrzywnowicz is offline   Reply With Quote

Old   March 16, 2020, 16:31
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,728
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
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.
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote


error, interface, walk routine

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On

Similar Threads
Thread Thread Starter Forum Replies Last Post
Fluent Radiation/porous media Schmitt pierre-Louis FLUENT 26 September 1, 2016 10:29
Radiation Modeling Chris89 CFX 20 August 14, 2014 07:51
Modeling both radiation and convection on surfaces - Ansys Transient Thermal R13 s.mishra ANSYS 0 March 31, 2012 04:12
user subroutine error CFDUSER CFX 2 December 9, 2006 06:31
user defined function cfduser CFX 0 April 29, 2006 10:58

All times are GMT -4. The time now is 21:38.