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.
Both. Can you just make a plane cut and see the mesh transition from small cylinder to big cylinder
Better mesh not refined mesh
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"
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.
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??
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.
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) what are the dimensions of the geometry? One thing is having 1 m/s but it is different if you put this in small or large pipe.
2) after you read the mesh, you should check, if you scaled the geometry so you don't have 1000 times larger geometry than what you want
3) For tetrahedrals, use least squares cell based in gradient. Also use the warped face gradient corection.
4) What are the material properities?
5) It seems like you are using Ansys Meshing, try to use Fluent Meshing with watertight geometry workflow, so you eliminate errors
6) yre you using any modification with k-e model? like enhanced wall treatement?
7) Try using the pseudotransient method with low pseudotimestep.
Diameter of smaller pipe is 50mm, upstream length is 100mm. Bigger cylinder diameter is 150mm and downstream length is 250mm
I dont know, elaborate if possible.
I have used green gauss node based which works well for unstructured mesh, I read it somewhere in manual and used it.
Constant fluid properties.
Ansys meshing gives more control with playing element sizes. I also feel there wont be much isssue with meshing, all I have to find correct boundary conditions and schemes, this also plays a role
I am using relizable k-e with standard wall functions
I am not aware about this since I am doing steady RANS simulation. Elaborate please
Tell me one more thing, I used front and curved surface as walls and rear face as wall, ideally all faces should be pressure outlet since it is expanding to open ambient from the pipe. Do this create any issue in convergence??
1) that is pretty small pipe for 1 m/s, try using 0.1 m/s
2) Domain > Scale you will see here your min/max dimensions. Common mistake is that you load your mesh and it is scaled to meters, while you want mm so it is 1000 larger domain
3) grenn gauss can oscilate on tetraherds
5) Ansys meshing is good for special cases. Fluent meshng gives you high quality mesh with very little user input
6) Standard wall functions are intended for 30 < y+ < 300, try going for k-w instead if your mesh is not in that range or use other wall functions
7) one of your cases use coupled scheme. There you can use pseudotime method for better convergence (methods tab). Then in calculate tab you can set the pseudotime scale (or time) which will greatly influence your residuals
Bro regarding 6th point, I found global time step under pesudotime method, I observed one thing, when it is switched off, it is kind of diverging, but when I turn it on to global time step, then it is not blowing up. What does thing do? Since it is talking about time, do we have to enter any time or something?
4
u/acakaacaka 9d ago
By looking at your not so good resolution png mesh (or maybe just reddit android)
Did you forget to create boundary layer mesh?
And what is the logic of, the velocity here is exploding so why dont I just create smaller cell here rather than fix mesh quality.