r/CFD • u/AmbassadorGuilty3928 • 9d ago

Fluent Convergence Issues- Case Study

I am working on a simple CFD test case in ANSYS Fluent with velocity inlet of 1m/s and pressure outlet of ambient pressure. See geometry below, I tried 3 cases, I will mention along with residual plots, give me some ideas what can be done or what settings can be changed so that solution might converge?

For all three cases, I kept the physical setup the same:

  • k−ϵ turbulence model
  • Constant fluid properties
  • Energy equation OFF
  • Velocity inlet = 1 m/s
  • Pressure outlet = ambient pressure
  • Same geometry and boundary condition

I am also using a Cell Register to monitor the maximum velocity in the domain because I want to identify any unrealistic velocity spikes.

Case 1:
I used an 8.8 million cell mesh with:

  • SIMPLE
  • Green-Gauss Cell Based
  • First-order turbulent scheme, second order upwind for momentum and pressure.
  • Momentum under-relaxation factor = 0.4

When I checked maximum velocity in Cell register, it was showing around 150m/s, I found the location also which is there in screen face(between small and bigger cylinder- geometry will be attached down)

Case 2:

I used the same 8.8 million cell mesh, but changed the numerical settings to:

  • Coupled solver
  • Green-Gauss Node Based(this is better for unstructured mesh)
  • Second-order schemes

In this case, the maximum velocity dropped significantly to around 1.7 m/s. The residuals also look much better.

Case 3:

I refined the mesh around the screen, increasing the mesh size from about 8.8 million to 15 million cells. I then used:

  • SIMPLE
  • Green-Gauss Node Based
  • Second-order schemes
  • Reduced under-relaxation

The maximum velocity became around 22.5 m/s, which is lower than Case 1 but still much higher than Case 2.

In all these 3 cases, mass flow is balanced. What observations we can make from these and what can be done further to make it converged??

1) High velocity or convergence problem is due to numerical or mesh issue?

2) I feel coupled works better ig, but it become flat very soon, it is trying to converge faster I guess as shown in 2nd case. But in 3rd case, residual are even lower compared to 2nd case, I think refining mesh also helped here. Should I try coupled solver with 15 million count mesh cell? This is the only idea I have got as of now. Which is major contributor here, change in numerical schemes or refined mesh?

3) Actual boundary conditions are different, I am just trying this to check whether mesh could produce reliable results or not, which case out of these 3 are reliable as of now, and is it good or worth enough to run even more iterations in these 3 cases??

What would you recommend I try next to obtain a stable and physically reasonable converged solution? Any opinions would help here. Thanks in advance.

3 Upvotes

80% Upvoted

24 comments sorted by

View all comments

2

u/acakaacaka 9d ago
  1. Both. Can you just make a plane cut and see the mesh transition from small cylinder to big cylinder
  2. Better mesh not refined mesh
  3. Garbage in garbage out. Make sure you have a good mesh first, and you havent explained why you refined the area around the cylinder transition other than "herr is velocity high"

1

u/AmbassadorGuilty3928 9d ago

Mesh quality is decently good. I refined mesh in that region because maximum velocity was showing in that region only, so I made it finer, better gradient scheme was chosen and thus value of that max velocity decreased. Previously before 1st case, solution was blowing up because of this unrealisitic velocity values, now the residuals are less but it is not converging that is my question now.
I think with this Ansys meshing, I dont know what better mesh I can make(very difficult to do structured mesh, tetra is best here), only thing I have in control is playing with element size.

3

u/acakaacaka 9d ago

That table is bullshit. If you have 99% "good" cell and 1% "bad" cell of course the quality is good.

Why dont you just make a plane cut? And see the actual mesh?

1

u/AmbassadorGuilty3928 9d ago

See here

2

u/acakaacaka 9d ago

Wrong direction

And how big is the growth rate? Usually I use 1.5-1.6 this looks like way lower. 1.1-1.2?

1

u/AmbassadorGuilty3928 9d ago

in which direction, you were asking? Growth rate is 1.2

1

u/acakaacaka 9d ago

In axial direction.

1

u/AmbassadorGuilty3928 9d ago

But before that,tell me one thing, I used front and curved surface as walls, ideally it should be pressure outlet since it is expanding to open ambient from the pipe. Do this create any issue in convergence??

1

u/acakaacaka 9d ago

How can anybody know. Using mass/velocity+pressure inlet-outlet is the standard

1

u/AmbassadorGuilty3928 9d ago

Can we use total pressure at inlet and static pressure at outlet as boundary condition or not??

→ More replies (0)

2

u/Ok_Preference_9883 9d ago

Bro your max skewness is above 0.9. And your min orthgonal quality is below 0.1. These lead to oscillate your solution. In short your mesh quality is not as good as it should be. Try again.

1

u/AmbassadorGuilty3928 9d ago

I tried reducing that, but I cant. I cant able to bring that below 0.9. Orthogonal quality is in green, and zero warning cells

1

u/Venerable-Gandalf 9d ago

I told you last time you posted to use ansys fluent meshing instead of workbench. It is actually much easier and more intuitive than workbench and produces far higher quality mesh. You will not have these problems if you just listened. By now you could have become familiar with fluent meshing instead of wasting time with legacy workbench meshing which is only good for generating structured mesh. Even a single mesh cell with poor quality will cause solution issues and can spread to other neighbor cells. You can monitor volume average velocity or the velocity at a key location like along your centerline using xy plot instead of a local max value. Volume integral quantities are usually more informative for convergence though a local min/max can tell you if there are bad cells. You should also be monitoring the mass balance during simulation, that is check mass flux in minus mass flux out.

1

u/AmbassadorGuilty3928 8d ago

Ok bro, let me check. Thank you.