[Mathewl1]

https://ibb.co/KXTMRCv
https://ibb.co/zP5q5H4
https://ibb.co/NjRjwSm
(These are the 3 imagines of the geometry and the residuals)
Hi everyone, I’m currently trying to run a simulation on the above image. It’s a 2D simplified model of a pipe (78mm) with a bluff body inserted inside of it. The model is currently not converging.

A 2D planar space was set.

Water is used as the fluid. As this is the case, a pressure based solver was used.

With Reynolds number being quite high in this, both transient flow was used alongside the turbulence model Realisable k-e with standard wall function with all default setting was used.

The following boundary conditions were used: -inlet: mass-flow inlet of 5kg/s -outlet: pressure outlet with result settings (0 gauge pressure)

• ⁠wall: both the pipe walls and the obstruction were set as walls with no slip condition applied.

For pressure-velocity coupling, the method used was simple (I’ve also tried piso)

For spacial discretisation the following was used: -gradient - Least squares cell based -pressure- second order

• ⁠momentum - second order upwind
• ⁠turbulent kinetic energy - second order upwind
• ⁠turbulent dissipation rate - second order upwind

Relaxation factors were set as default

Residuals were set to 1e-6

Initialisation: used standard and hybrid but neither helped.

Really any advice on this. Things to look at and general tips would be really really appreciated. This is for my honours degree thesis and I’ve been trying to get it to work for some time now to no avail. I’m beginning to panic and is why I’ve come to this server as I’ve seen some great advice on it already and think it would be really useful getting help from more advance people in cfd.

Thanks in advance for those that help and anything else I can provide just let me know!!

[CFDKareem]

Can you post a picture of what your mesh looks like?

The flow channels around the body are really narrow. I want to make sure these regions are refined sufficiently. Also, try using Enhanced Wall Treatment for your near wall condition instead of Standard. To use EWT you should make sure that your Y+ value is ~1.

Once I confirm the mesh quality we can discuss some next steps, assuming this is not the issue.

P.S. Try using the internal image hosting on this forum. Many users are wary of clicking on external links.

[Mathewl1]

Hi CFD Kareem,

Thank you for responding. I will fix my mesh and ensure y+ ~ 1 and let you know if this works - this may take a few days. Could you give some advice on the meshing to ensure I’m coving all bases when doing it, like things to research. I’ve also had some trouble meshing it as warnings come up with face meshing. I’m using aspect ration and skewness of the elements to ensure quality so far. I’ve also split the mesh up to get a structured mesh but had some errors with face meshing. Anything else you could guide me with this would be appreciated, maybe things like types of meshing techniques that would be suitable for such a narrow gap.

Also I gave your video a watch. Great content and you’ve earned a new subscriber!

[CFDKareem]

Originally Posted by Mathewl1

Hi CFD Kareem,

Thank you for responding. I will fix my mesh and ensure y+ ~ 1 and let you know if this works - this may take a few days. Could you give some advice on the meshing to ensure I’m coving all bases when doing it, like things to research. I’ve also had some trouble meshing it as warnings come up with face meshing. I’m using aspect ration and skewness of the elements to ensure quality so far. I’ve also split the mesh up to get a structured mesh but had some errors with face meshing. Anything else you could guide me with this would be appreciated, maybe things like types of meshing techniques that would be suitable for such a narrow gap.

Also I gave your video a watch. Great content and you’ve earned a new subscriber!

I wouldn't worry about keeping the mesh structured. The tradeoff of an unstructured mesh is usually simulation time. For 2D geometry the difference in compute time is usually minimal. There should be no tradeoff in accuracy as long as the mesh is high quality.

As far a research goes, a good place to start is understanding wall functions and how they relate to Y+ value. The Ansys theory manual has a bit of info, but there are many great resources online explaining the theory of wall functions and Y+.

For specifics on meshing your model. I would focus first on setting your inflation layers to achieve the proper Y+. The first layer height will change from the inlet region through the narrow channel. There's no need to over refine the inlet and outlet region. You can use multiple inflation layers and wall sizing to vary the boundary layer throughout the domain. When checking the mesh statistics do not be discouraged by aspect ratios greater than 1, fi they occur in the inflation layer. It is okay for the boundary layer elements to be elongated in the direction of flow. Also, check the "Capture Proximity" option under mesh and play with the number of cells across the gap. This can help automatically refine the mesh in those narrow channels. It's hard to give hard recommendations as mesh generation is as much of an art as it is a science, but hopefully these few tips help.

Finally, don't get too wrapped up in mesh generation. Convergence issues can be caused by the mesh, but are much more likely to be other solver settings in Fluent. Once you have the solver settings nailed down and a mesh converging well, you can go back and do a proper mesh refinement study to further reduce the error and make sure your achieving mesh independence.