CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > SU2

Problem with convergence

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

Like Tree2Likes
  • 2 Post By fpalacios

Reply
 
LinkBack Thread Tools Display Modes
Old   January 17, 2013, 07:35
Default Problem with convergence
  #1
Member
 
Roberto Pieri
Join Date: Feb 2012
Location: Milan
Posts: 57
Rep Power: 5
robyTKD is on a distinguished road
Hello, I'm trying to simulate the flow around NACA0012 airfoil. It is a simple incompressible viscous case without separations, to be more clear the configuration file is attached below.

I also attach the convergence history; regarding the plot I have two questions:
  • why the residual rises around iteration 2000?
  • why the last iterations the solution is diverging?

Please note that in these two points the CFL(=2) isn't changing.

Thank you very much in advance.

Roberto
Attached Images
File Type: jpg NACA0012.jpg (81.2 KB, 44 views)
Attached Files
File Type: zip NS_NACA0012.zip (6.1 KB, 12 views)
robyTKD is offline   Reply With Quote

Old   January 19, 2013, 18:09
Default
  #2
Super Moderator
 
Francisco Palacios
Join Date: Jan 2013
Location: Stanford, CA
Posts: 301
Rep Power: 5
fpalacios is on a distinguished road
Quote:
Originally Posted by robyTKD View Post
Hello, I'm trying to simulate the flow around NACA0012 airfoil. It is a simple incompressible viscous case without separations, to be more clear the configuration file is attached below.

I also attach the convergence history; regarding the plot I have two questions:
  • why the residual rises around iteration 2000?
  • why the last iterations the solution is diverging?

Please note that in these two points the CFL(=2) isn't changing.

Thank you very much in advance.

Roberto
Hi Roberto,
As far I see in the config file, you are running the compressible solver.

With respect to the parameters this is my recommendation.
MACH_NUMBER= 0.15
AoA= 10.0
FREESTREAM_TEMPERATURE= 273.15
REYNOLDS_NUMBER= 6.0E6
REYNOLDS_LENGTH= 1.0
Remember that FREESTREAM_PRESSURE is computed by the code for viscous flows!

With the values below the non-dimensional temperature, density and pressure will be 1.0:
REF_AREA= 1.0
REF_PRESSURE= 244948.0
REF_TEMPERATURE= 273.15
REF_DENSITY= 3.11513

It is better to use an upwind scheme to deal with viscous flows
CONV_NUM_METHOD_FLOW= ROE-2ND_ORDER
SLOPE_LIMITER_FLOW= VENKATAKRISHNAN
LIMITER_COEFF= 0.01
If your convergence stall then, reduce the value of the LIMITER_COEFF

Remember that the NASA validation has been done with a 230529 points grid, this is 5x finer than the grid that you are using.

To start with, it is always a good idea to switch off the MG
MGLEVEL= 0

We have done an extensive V&V of the compressible solver (described in http://su2.stanford.edu/documents/SU2_AIAA_ASM2013.pdf ) but the incompressible solver is in a V&V stage, you are very welcome to contribute (first Euler, then Laminar NS, and finally RANS).

Best,
Francisco
momo_sjx and mrenergy like this.

Last edited by fpalacios; January 19, 2013 at 23:00.
fpalacios is offline   Reply With Quote

Old   January 23, 2013, 17:19
Default
  #3
Member
 
Roberto Pieri
Join Date: Feb 2012
Location: Milan
Posts: 57
Rep Power: 5
robyTKD is on a distinguished road
Thank you for your reply.

In these days I tested different settings.

Quote:
Originally Posted by fpalacios View Post
With the values below the non-dimensional temperature, density and pressure will be 1.0:
REF_AREA= 1.0
REF_PRESSURE= 244948.0
REF_TEMPERATURE= 273.15
REF_DENSITY= 3.11513
I found out that, with these settings, reference values are not unitary, therefore I changed them; nevertheless results are the same in the two cases.

Quote:
Originally Posted by fpalacios View Post
It is better to use an upwind scheme to deal with viscous flows
CONV_NUM_METHOD_FLOW= ROE-2ND_ORDER
SLOPE_LIMITER_FLOW= VENKATAKRISHNAN
LIMITER_COEFF= 0.01
I obtained better results with JST scheme, they are very close to reference ones.

Quote:
Originally Posted by fpalacios View Post
To start with, it is always a good idea to switch off the MG
MGLEVEL= 0
With MG disabled, the solution converges more smoothly; I also tried to set MG on, but only with one level (W cycle or V cycle is the same) of MG the solution doesn't show the problems presented before.
Do you have some advice to find a better configuration of MG technique? For my tests I considered config files of tutorials as a reference, but the solution becomes not stable.

Now I have a fair solution, but the same config file, on the same mesh, gives different results if run in parallel or serial. Have you ever experienced the same problem before?

Thank you very much,
Roberto
robyTKD is offline   Reply With Quote

Old   January 29, 2013, 16:04
Default
  #4
Super Moderator
 
Thomas D. Economon
Join Date: Jan 2013
Location: Stanford, CA
Posts: 260
Rep Power: 5
economon is on a distinguished road
Just a couple of notes on finding a good set of parameters for multigrid (it can be a bit of an art):

A 'W' cycle will be more expensive per multigrid iteration, but in general should provide the best overall convergence acceleration. If you are having trouble keeping stability, try a 'V' cycle too.

The number of levels that one should use is largely dependent on the individual mesh, as the agglomeration should produce successive coarser mesh levels that have 'good' agglomeration rates. Depending on the element type, the agglomeration rates should in general be in the 1/3-1/8 range for better quality. If an agglomerated rate for a coarse level approaches 1/1, it will not be as effective. Creating appropriately sized levels is important for the multigrid algorithm (the idea is to damp high and low frequency oscillations in the solution by using the residuals computed on the various fine and coarse meshes to form a better update). The agglomeration rates are printed to the screen during the preprocessing during a run of SU2_CFD. For instance, the following is printed for the inviscid NACA 0012 test case:

CVs of the MG level: 1533. Agglom. rate 1/3.41357. MG level: 1.
CVs of the MG level: 457. Agglom. rate 1/3.35449. MG level: 2.
CVs of the MG level: 166. Agglom. rate 1/2.75301. MG level: 3.

There are two parameters in the config file that give the user some control over the agglomeration process:

%
% Maximum number of children in the agglomeration stage
MAX_CHILDREN= 50
%
% Maximum length of an agglomerated element (relative to the domain)
MAX_DIMENSION= 0.1

By modifying these inputs, the agglomeration rates can be influenced, which can help create higher quality coarse mesh levels.

Hope this helps!
economon is offline   Reply With Quote

Old   February 4, 2013, 11:14
Default
  #5
Member
 
Roberto Pieri
Join Date: Feb 2012
Location: Milan
Posts: 57
Rep Power: 5
robyTKD is on a distinguished road
I thank you very much for the exhaustive clarification to my question and I would like to apologize for my late reply, I was testing different settings to activate multigrid strategy.
Unfortunately, I was not able to reach a converged solution because it appears to become unstable using 3 MG levels (an example is attached below) either with W cycle or V cycle. Now I'm trying to decrease the number of MG levels in order to reach the solution.
However, is it possible that I can obtain a more stable behaviour by setting appropriately pre/post-smoothing level? Are there some hints to find the best setting?

Roberto
Attached Images
File Type: jpg Residual.jpg (37.4 KB, 22 views)
robyTKD is offline   Reply With Quote

Reply

Tags
convergence, naca0012

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
convergence problem when use pisoFoam, LES for wind tunnel case Forrest_Lei OpenFOAM 3 July 19, 2011 06:00
convergence problem commonyue Main CFD Forum 1 December 1, 2009 04:54
Convergence of CFX field in FSI analysis nasdak CFX 2 June 29, 2009 01:17
3D Fluid Flow Convergence problem Emily FLUENT 2 March 21, 2007 23:18
Non Convergence of 3D Heat transfer cfd problem Balraj Main CFD Forum 3 December 9, 2004 01:24


All times are GMT -4. The time now is 16:23.