Fluids

Fluids

A mesh skewness problem

    • m.shafiee1374
      Subscriber

      Hi,

      I ran a steady 3d simulation of a grid shown in the first picture using realizable k-e turbulence model, and my mesh skewness across all my domain is below 0.65 (which is acceptable according to fluent guidelines). However, I find some irregularities in the velocity contour at locations with highest skewness (second picture). Now I'm worried about another geometry with a bit higher max skewness(<0.75), and whether that will give me acceptable results or not.

      Can this issue be solved by changing any of the simulation parameters? Or changing the mesh (which I'd rather not) is the only way to fix it?

      Thanks :)


      p.s. I'm using Ansys Workbench 17.0 for this project.

    • Keyur Kanade
      Ansys Employee
      Please check orthogonality. The min orthogonal quality should be above 0.1 to proceed to solver. If it is less than 0.1 then please improve the mesh.
      First check the locations of the bad elements. Please see following video for the same.

      " target="blank">


      Once you have locations, please check if you can improve mesh using different mesh sizing. Please see following video.

      " target="blank">

      Please go through help manual for more details
      Regards Keyur
      How to access Ansys Online Help Document
      Guidelines on the Student Community

  • Rob
    Ansys Employee
  • m.shafiee1374
    Subscriber
    Hello I checked my mesh quality and my min ortho quality is 0.387 and max ortho skew is 0.613, so i assume there are no "bad quality elements" .
    --------------
    And regarding this thread which was also mine:
    I managed to solve the divergence issue by reducing the under-relaxation factors of pressure, momentum and turbulence properties by 0.2 as was suggested by the Fluent guide.
    Also there are no blocking here, because I'm using Gambit not ICEM. I've decomposed the domain into lots of smaller volumes to be able to generate a structured hex mesh.
    However, I'm going to refine my mesh in this area to reduce the "jump" in aspect ratio and cell size. Hopefully this might work...
    Thanks for your answers.
  • Rob
    Ansys Employee
    Ortho quality and skew are only part of the problem. You also need to avoid large jumps in cell size and add sufficient mesh to resolve the gradients: in your case you have jumps in cell size in the same region as the relatively steep gradients.
    Fixing this isn't as straightforward. GAMBIT is about 10-15 years from it's last update, and whilst it has several powerful features has been largely superceeded by the current geometry tools and Fluent Meshing. Using a poly or poly-hexcore mesh on the entire fluid region will reduce the jumps in cell size, and allow you to then use either adaption or controlled growth rates to get a better mesh around the pins/stubs.
  • m.shafiee1374
    Subscriber

    Hello Rob So I went ahead and generated a tetrahedral mesh using icem cfd, then imported it to fluent and converted the mesh to polyhedral as you suggested.
    I've also smoothed the mesh to make sure its quality is within the acceptable range.

    But now the velocity contour in the x-z plane looks like this:
    Since I'm completely new to icem/poly mesh, I expect there must be a way to smooth these results?? Or should i use even a finer grid?


  • Rob
    Ansys Employee
    Where is that plane relative to the obstructions?
  • m.shafiee1374
    Subscriber
    Those obstructions are 10 meters tall and this plane is 1 meter above them.
  • Rob
    Ansys Employee
    Zoom in and replot with node values off.
  • m.shafiee1374
    Subscriber

  • Rob
    Ansys Employee
    That's weird. How's the convergence? I've only seen that effect where there was only 1-2 cells between the plotted surface and a wall.
  • m.shafiee1374
    Subscriber
    Convergence is pretty good actually, better than the hex mesh, solution converged after around 400 iterations with residuals less than 0.001 and no fluctuations in them .
    There's also much more than 2 cells between the contour plane and the wall boundaries.
    I also didn't see this problem in the contours plotted on the x-y or y-z planes, which is super weird.

  • Rob
    Ansys Employee
    But you do have very disturbed contour boundaries in the vertical plane: look at the bounds of the green and yellow contours.
  • m.shafiee1374
    Subscriber

    I figured what the problem was. Since im using a custom velocity profile at the inlet, my velocity gradient in the vertical direction around the location at which this contour is plotted, was higher than that my mesh could resolve. Which means I have to refine my grid near the bottom of the domain in the vertical direction, but I'm struggling to do so because fluent runs out of memory during tetra to poly conversion.
    I'm open to suggestions, and once again thanks for your answers.
  • Rob
    Ansys Employee
    Read the geometry into Fluent Meshing and create the poly mesh directly. Memory overheads are significantly reduced and you don't then need to go anywhere near GAMBIT.
  • Viewing 14 reply threads
    • You must be logged in to reply to this topic.