CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > FLUENT

k-w-SST-Model does not converge. Mesh too fine?

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   January 23, 2017, 01:55
Default k-w-SST-Model does not converge. Mesh too fine?
  #1
New Member
 
Join Date: Nov 2016
Posts: 26
Rep Power: 2
h0rst is on a distinguished road
Hello everybody,

I am simulating an induction coil flowed through by water. With Ansys APDL, I model the w/m 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
h0rst is offline   Reply With Quote

Old   January 25, 2017, 01:49
Default
  #2
swm
Member
 
swm's Avatar
 
Song Weimin
Join Date: Dec 2013
Posts: 41
Rep Power: 5
swm is on a distinguished road
Can you post the converge history of k, w and density?

Sent from my EVA-AL10 using CFD Online Forum mobile app
swm is offline   Reply With Quote

Old   January 25, 2017, 01:51
Default
  #3
swm
Member
 
swm's Avatar
 
Song Weimin
Join Date: Dec 2013
Posts: 41
Rep Power: 5
swm is on a distinguished road
And can you further describe the flow condition in detail?

Sent from my EVA-AL10 using CFD Online Forum mobile app
swm is offline   Reply With Quote

Old   January 25, 2017, 15:14
Default
  #4
New Member
 
Join Date: Nov 2016
Posts: 26
Rep Power: 2
h0rst is on a distinguished road
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
Attached Images
File Type: jpg coil part.jpg (142.5 KB, 31 views)
File Type: jpg residuals.jpg (58.9 KB, 28 views)
h0rst is offline   Reply With Quote

Old   January 26, 2017, 02:22
Default
  #5
Senior Member
 
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 1,568
Rep Power: 22
LuckyTran will become famous soon enough
Compare the mesh quality. It's likely your fine mesh has worse quality, higher aspect ratios, lower orthogonality, higher skewness, etc.
LuckyTran is offline   Reply With Quote

Old   January 28, 2017, 17:16
Default
  #6
swm
Member
 
swm's Avatar
 
Song Weimin
Join Date: Dec 2013
Posts: 41
Rep Power: 5
swm is on a distinguished road
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
swm is offline   Reply With Quote

Old   February 5, 2017, 05:06
Default
  #7
New Member
 
Join Date: Nov 2016
Posts: 26
Rep Power: 2
h0rst is on a distinguished road
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?
Attached Images
File Type: png mesh.png (110.6 KB, 6 views)
h0rst is offline   Reply With Quote

Old   February 5, 2017, 09:11
Default
  #8
swm
Member
 
swm's Avatar
 
Song Weimin
Join Date: Dec 2013
Posts: 41
Rep Power: 5
swm is on a distinguished road
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
swm is offline   Reply With Quote

Old   February 5, 2017, 09:20
Default
  #9
swm
Member
 
swm's Avatar
 
Song Weimin
Join Date: Dec 2013
Posts: 41
Rep Power: 5
swm is on a distinguished road
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
swm is offline   Reply With Quote

Old   February 5, 2017, 09:29
Default
  #10
New Member
 
Join Date: Nov 2016
Posts: 26
Rep Power: 2
h0rst is on a distinguished road
Can you explain me how I can draw the streamlines?


I didn't find it under Results/Plots/contours/velocity
h0rst is offline   Reply With Quote

Old   February 5, 2017, 09:32
Default
  #11
swm
Member
 
swm's Avatar
 
Song Weimin
Join Date: Dec 2013
Posts: 41
Rep Power: 5
swm is on a distinguished road
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
swm is offline   Reply With Quote

Old   February 5, 2017, 12:38
Default
  #12
Senior Member
 
Julio Mendez
Join Date: Apr 2009
Location: Greensboro, U.S.A
Posts: 218
Rep Power: 10
juliom is on a distinguished road
Send a message via Skype™ to juliom
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.
juliom is offline   Reply With Quote

Old   February 5, 2017, 15:01
Default
  #13
New Member
 
Join Date: Nov 2016
Posts: 26
Rep Power: 2
h0rst is on a distinguished road
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...
h0rst is offline   Reply With Quote

Old   February 5, 2017, 17:04
Default
  #14
Senior Member
 
Julio Mendez
Join Date: Apr 2009
Location: Greensboro, U.S.A
Posts: 218
Rep Power: 10
juliom is on a distinguished road
Send a message via Skype™ to juliom
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 !!
juliom is offline   Reply With Quote

Old   February 5, 2017, 17:19
Default
  #15
Senior Member
 
Julio Mendez
Join Date: Apr 2009
Location: Greensboro, U.S.A
Posts: 218
Rep Power: 10
juliom is on a distinguished road
Send a message via Skype™ to juliom
Quote:
Originally Posted by h0rst View Post
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...
I forgot to elaborate more about the issue with steady state and transient approach. I had the same questions years ago. The problem is more related to how the system reacts to the initial guess in the steady state approach. If your initial condition is not close enough your problem instead of converge will diverge. Once, I was told that transient simulation are less stiff. That statement make a lot of sense if you remember the CFL criteria for explicit schemes where you see the combination of dx and dt in the definition. Also, a professor told me that there are some problems that are not possible to solve with a steady state solver. Imagine the vortex street karman problem. That is due to the transient nature of the problem (related to turbulence) and that transient phenomenon is not dominated by transient boundary conditions. I can cite one paragraph from one textbook I have that described this issue better but I have my textbook at home.
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.
juliom is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
General question about SST turbulence model Richard Renaud CFD Freelancers 1 December 19, 2015 05:13
decomposePar problem: Cell 0contains face labels out of range vaina74 OpenFOAM Pre-Processing 27 November 2, 2015 18:04
[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 12:32
2D Mesh Generation Tutorial for GMSH aeroslacker Open Source Meshers: Gmsh, Netgen, CGNS, ... 12 January 19, 2012 04:52


All times are GMT -4. The time now is 08:26.