Error in s2s radiation model view factor calculation

JohannesJohannes NorwayMember

Hi,

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?

 

-Johannes

Comments

  • RobRob UKForum Coordinator
    edited January 7

    Have you changed anything? 

  • JohannesJohannes NorwayMember
    edited January 7

    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.

  • RobRob UKForum Coordinator
    edited January 7

    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?

  • JohannesJohannes NorwayMember
    edited January 8

    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.

  • RobRob UKForum Coordinator
    edited January 8

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

  • JohannesJohannes NorwayMember
    edited January 8

    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.

  • RobRob UKForum Coordinator
    edited January 9

    And no hanging nodes?

  • JohannesJohannes NorwayMember
    edited January 10
  • RobRob UKForum Coordinator
    edited January 10

    What exactly changed in the mesh? 

  • JohannesJohannes NorwayMember
    edited January 10

    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.

  • RobRob UKForum Coordinator
    edited January 10

    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. 

  • JohannesJohannes NorwayMember
    edited January 14

    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?

    -Johannes

     

  • RobRob UKForum Coordinator
    edited January 14

    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. 

  • JohannesJohannes NorwayMember
    edited January 14

    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

  • JohannesJohannes NorwayMember
    edited January 15

    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.

  • RobRob UKForum Coordinator
    edited January 15

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

  • JohannesJohannes NorwayMember
    edited January 16

    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

  • RobRob UKForum Coordinator
    edited January 16

    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. 

  • JohannesJohannes NorwayMember
    edited January 20

    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!

    Johannes

Sign In or Register to comment.