|
[Sponsors] |
k-w-SST-Model does not converge. Mesh too fine? |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
January 23, 2017, 00:55 |
k-w-SST-Model does not converge. Mesh too fine?
|
#1 |
Member
Join Date: Nov 2016
Posts: 73
Rep Power: 9 |
Hello everybody,
I am simulating an induction coil flowed through by water. With Ansys APDL, I model the w/m³ in the coil and import the values by UDF into the Fluent model. With Fluent, I try to simulate the flow and how the cooling works. I started first with a rough mesh and increased its accuracy. So I started with a very rough mesh and the model converges. Now, I am using a very fine mesh and my k and my Omega do not fall below the demanded 1e-4. I tried very many iterations. Does someone have an idea how I may make this model converge? Best regards h0rst |
|
January 25, 2017, 00:49 |
|
#2 |
Member
Join Date: Dec 2013
Posts: 47
Rep Power: 12 |
Can you post the converge history of k, w and density?
Sent from my EVA-AL10 using CFD Online Forum mobile app |
|
January 25, 2017, 00:51 |
|
#3 |
Member
Join Date: Dec 2013
Posts: 47
Rep Power: 12 |
And can you further describe the flow condition in detail?
Sent from my EVA-AL10 using CFD Online Forum mobile app |
|
January 25, 2017, 14:14 |
|
#4 |
Member
Join Date: Nov 2016
Posts: 73
Rep Power: 9 |
Hello,
attached you'll find a picture of the residual history. I also tried to run for 100.000 itereations but it still does not converge. When I change Momentum to 1st order, the model converges, but the results look very strange, whereas the results with the non-converging model are not that bad. The picture of the mesh shows a part of my model. Blue is water inlet and red is water outlet. The rest of the model looks basically the same as the part to be seen on the picture: The coil continues where the picture is stopped and later on, both leads go together at the end in a half circle similar to the leads in the beginning. I tried different meshes. When I increase the number of elements, the convergence gets harder and harder until it does not reach the demanded default residual. I have choosen velocity inlet and outflow. On the whole, I always took the standard parameters from fluent. Best regards h0rst |
|
January 26, 2017, 01:22 |
|
#5 |
Senior Member
Lucky
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 5,676
Rep Power: 66 |
Compare the mesh quality. It's likely your fine mesh has worse quality, higher aspect ratios, lower orthogonality, higher skewness, etc.
|
|
January 28, 2017, 16:16 |
|
#6 |
Member
Join Date: Dec 2013
Posts: 47
Rep Power: 12 |
Hi h0rst,
It seems that in the inlet and outlet region, the transition of your grid is toooo fast in the streamwise and you may need to refine that. Physically, you may need more streamwise points in inlet and outlet in this case to let the fluid "flow" into and out of the long pipe Sent from my EVA-AL10 using CFD Online Forum mobile app |
|
February 5, 2017, 04:06 |
|
#7 |
Member
Join Date: Nov 2016
Posts: 73
Rep Power: 9 |
I extended the mesh size of the length of the inlet conductors (see attachment).
Still it does not converge If I change momentum to first order or reduce relaxation sweep of momentum, then it converges, but the results seems to be very wrong. Any other ideas how I can improve my mesh? |
|
February 5, 2017, 08:11 |
|
#8 |
Member
Join Date: Dec 2013
Posts: 47
Rep Power: 12 |
In the unconverged case, you may extract streamlines in each part of the pipe(inlet outlet and anyother region)to see whether something is wrong(for example, if you find streamlines in inlet or outlet are wrong or in other smooth region, a strange vortex comes up which triggers separation, you may know what is impacting your computation)
Sent from my EVA-AL10 using CFD Online Forum mobile app |
|
February 5, 2017, 08:20 |
|
#9 |
Member
Join Date: Dec 2013
Posts: 47
Rep Power: 12 |
And I also suggest you should check the velocity vector distribution in streamwise plane from inlet to outlet, to observe whether the BC layer is correct or whether the grid is fine enough to capture the BC layer near solid walls. Maybe some other paramters distribution, such as density, pressure, turbulent quantity k and omega, should also be carefully taken care of.
Sent from my EVA-AL10 using CFD Online Forum mobile app |
|
February 5, 2017, 08:29 |
|
#10 |
Member
Join Date: Nov 2016
Posts: 73
Rep Power: 9 |
Can you explain me how I can draw the streamlines?
I didn't find it under Results/Plots/contours/velocity |
|
February 5, 2017, 08:32 |
|
#11 |
Member
Join Date: Dec 2013
Posts: 47
Rep Power: 12 |
Sorry about that, it has been two years since the last time I use commercial softwares. I think u can get your answer from google
Sent from my EVA-AL10 using CFD Online Forum mobile app |
|
February 5, 2017, 11:38 |
|
#12 |
Senior Member
|
Make sure your mesh transition is very low. I suggest to keep the change rate as low as possible not greater than 20%. What you are doing is quite time consuming and when you expect to get a better convergence just by reducing the mesh you endup with the opposite result. Sometimes you must use a transient approach even more when the problem has a lot of recirculation. I would also suggest to interpolate the solution from the coarse mesh onto the finer. That may work if and only if your mesh quality is good.
|
|
February 5, 2017, 14:01 |
|
#13 |
Member
Join Date: Nov 2016
Posts: 73
Rep Power: 9 |
Thank you for the answers.
I switched now to transient simulation and made very small time steps: - timestep: 0,001 s - 10.000 timesteps - max. 1.000.000 iteration per time step so, when it's done it is 10 s real time which is much longer than the actual test took time to go into steady state. I left the residuals as default (10e-4 for all except energy which is 10e-6). So far, all the timesteps are converging quite well (always after about 5 iterations). Can I expect that the results from this solution are reliable? I am wondering why the transient does converge but not the steady-state... |
|
February 5, 2017, 16:04 |
|
#14 |
Senior Member
|
Well I would not be worry about the computational Time vs the actual experimental time. They don't have to be the same. I will e quite surprise if so. For example; currently, I'm running hypersonic flow over a flat plate: the experimental test lasted 3ms and my computational time is close to 160 seconds. Now; you might start looking st the average solution. The steady state solution will be dominated by the boundary conditions and the flow will "forget the initial conditions". Also, remember that you have at the beginning of the computation false transient information. Nonetheless, this is my humble opinion. I am looking forward to read professor Denaro opinion about the computational and experimental time.
All the best !! |
|
February 5, 2017, 16:19 |
|
#15 | |
Senior Member
|
Quote:
Once again, this humble opinion and I'm not a professor in CFD. Professor Denaro's opinion will be very insightful and way better than mine. Looking forward to his contribution about these two comments. |
||
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
decomposePar problem: Cell 0contains face labels out of range | vaina74 | OpenFOAM Pre-Processing | 37 | July 20, 2020 05:38 |
General question about SST turbulence model | Richard Renaud | CFD Freelancers | 1 | December 19, 2015 04:13 |
[GAMBIT] How to mesh a cylinder with fine to coarse cells | Bharatt | ANSYS Meshing & Geometry | 3 | August 12, 2013 00:45 |
Wall treatment mesh refinement in k-omega SST model | Jorg | FLUENT | 0 | February 27, 2013 11:32 |
[Gmsh] 2D Mesh Generation Tutorial for GMSH | aeroslacker | OpenFOAM Meshing & Mesh Conversion | 12 | January 19, 2012 03:52 |