Error in s2s radiation model view factor calculation

  • Last Post 20 January 2020
  • Topic Is Solved
Johannes posted this 07 January 2020


When calculating the view factors in the s2s radiation model, i get the following error prompt:

Error at Node 3: delete_dual_edge_from_list : not in list

The view factors have been successfully calculated using the same geometry before. Anybody knows what the problem is?



Order By: Standard | Newest | Votes
rwoolhou posted this 07 January 2020

Have you changed anything? 

Johannes posted this 07 January 2020

The mesh changed slightly, as i remeshed the area, but I don't know what the error might be associated with... is it a geometry/mesh issue? Everything else works just as before.

rwoolhou posted this 07 January 2020

So, focus on the remeshed region. It's not one I've seen, but I tend to use DO for most applications. What's the cell quality like?

Johannes posted this 08 January 2020

The quality was improved compared to the mesh/case with successfull view factor calculation (reason for remesh). I have a poly-hexcore mesh with 10.2 million cells, worst quality (inverse orthogonal) is 0.8. 

I had problems with a corrupted case file before. I'll set up a new case and see if the problem persists.

rwoolhou posted this 08 January 2020

Read the Theory Guide (Help) on the S2S model: specifically limitations. 

Johannes posted this 08 January 2020

I'm aware of that but as it worked like a charm before I did not expect any troubles after some minor changes in the mesh which in principle stayed the same.

rwoolhou posted this 09 January 2020

And no hanging nodes?

Johannes posted this 10 January 2020


rwoolhou posted this 10 January 2020

What exactly changed in the mesh? 

Johannes posted this 10 January 2020

I just did some local refinements and changed the geometry recovery settings for a few elements. I'm just now setting up a new case from scratch and will let you know if the same error appears again.

rwoolhou posted this 10 January 2020

Thanks. Changing the geometry recovery may mean you've picked up a new feature that's then causing the problem. If that's the case look (very carefully) for folds and/or baffles. 

Johannes posted this 14 January 2020

Hi rwoolhou,

After setting up a new case I do not get the error prompt as described above any longer. However, I'm experiencing a different issue. When I start the simulation, the energy residual just explodes and goes straight up to 1e+35 after just 15 iterations. I'm also getting warnings from iteration 1, that temperature was limited to 5000 K in 12000 cells etc. even though I have external CFD of an urban setting with solar ray tracing. I should not get temperatures above 300 K, as my inlet temperature is 278 K. I set the solar parameters to 425 W/m2 direct, and 95 W/m2 diffuse (measured values). 

The thing is, I'm not sure how to set the boundary conditions for my domain boundaries correctly. I set the external radiation temperature (I assume this to be Tsky in my case) to 273 K and that the domain boundaries do not take part in the solar ray tracing (so that radiation would pass right through them without any interaction). Or  longwave radiation losses to the sky be modelled differently?



rwoolhou posted this 14 January 2020

If you plot temperatures after about 5 iterations what does it look like. Those settings don't look silly, so it could be mesh related. 

Johannes posted this 14 January 2020

The area of interest, meaning the buildings and center area of my domain show extremely high temperatures. This affects the ground and air temperature in the wake of this area, as it is also extremely high (but a little lower than in the center of the area of interest). I first assumed I entered a digit too many in the temperature boundary condition for the buildings and ground surfaces, but I checked and everything looks fine. 

If it is a mesh related problem, what do you suggest? Refining?


Johannes posted this 15 January 2020

I just used a tetrahedral mesh, using the exact same settings for sizing and boundary conditions etc. and everything works just fine. I think the nature of the mesh is therefore responsible for the divergence. Would be nice to know why, though.

rwoolhou posted this 15 January 2020

Were there any jumps in cell size and/or hanging nodes in the problem area?

Johannes posted this 16 January 2020

No, no hanging nodes/jumps. Growth rate was set to 1.2 globally. Here's the situation after 15 iterations.

Residuals after 15 iterations

Situation after 15 iterations

rwoolhou posted this 16 January 2020

That almost looks like a parallel node has done something odd. The solution hasn't even tried to converge so there's something very broken with the model somewhere. 

Johannes posted this 20 January 2020

FYI, problem solved. As you suspected, it was a couple of bad cells that were not easy to find using the standard quality identification options in Fluent. It was a problem in the inflation layer. After the correction of the area, the simulation runs smoothly!

Thank you for your help!