CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

Problems with the RSM in simpleFoam

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

Like Tree1Likes
  • 1 Post By hjasak

Reply
 
LinkBack Thread Tools Display Modes
Old   September 1, 2006, 14:59
Default I've tried to run some 3D simu
  #1
New Member
 
Steve Berg
Join Date: Mar 2009
Posts: 9
Rep Power: 8
sberg is on a distinguished road
I've tried to run some 3D simulations with a Reynolds stress model lately, but they will not converge. I've played around with the settings and variables but the simulations remains unstable. However, with the k-epsilon model the simulations converges nicely. Have anyone else had succees with the RSM, or am I doing something utterly wrong?
sberg is offline   Reply With Quote

Old   September 1, 2006, 15:19
Default It should work without problem
  #2
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,758
Rep Power: 21
hjasak will become famous soon enough
It should work without problems. If you are running something relatively small and simple I wouldn't mind having a look, just to make sure RSTM is still fine.

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   September 2, 2006, 05:21
Default It's a small case where two sq
  #3
New Member
 
Steve Berg
Join Date: Mar 2009
Posts: 9
Rep Power: 8
sberg is on a distinguished road
It's a small case where two square ducts, each of them with dimensions 0.1*0.1*1 (m), are joined together in a 90 degree bend. Air is flowing through at a Reynolds number of 100,000. The turbulence intensity, and the turbulent length scales compared to the outer dimensions, are both assumed to be 10 %.

The kEpsilon and RNGkEpsilon works well on this geometry, but I cannot obtain a solution with the LRR or LaunderGibsonRSTM models.


sberg is offline   Reply With Quote

Old   September 2, 2006, 05:40
Default
  #4
New Member
 
Steve Berg
Join Date: Mar 2009
Posts: 9
Rep Power: 8
sberg is on a distinguished road

sberg is offline   Reply With Quote

Old   September 2, 2006, 05:48
Default Steve, I don't think you ma
  #5
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,758
Rep Power: 21
hjasak will become famous soon enough
Steve,

I don't think you managed to attach the file.

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   September 2, 2006, 05:49
Default Hi, Im a beginner att openF
  #6
newbee
Guest
 
Posts: n/a
Hi,

Im a beginner att openFOAM but I have tried the turbmodels you mension and I have had a similar problem which i got thru by having a epsilon value 3 times as big as when I used the kepsilon models.

/erik
  Reply With Quote

Old   September 2, 2006, 08:15
Default I'll try again:-) Here is a
  #7
New Member
 
Steve Berg
Join Date: Mar 2009
Posts: 9
Rep Power: 8
sberg is on a distinguished road
I'll try again:-)

Here is a link to the case: http://home.chello.no/~sberg/bend.tar.gz


Steve
sberg is offline   Reply With Quote

Old   September 2, 2006, 15:02
Default I don't see a problem: it conv
  #8
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,758
Rep Power: 21
hjasak will become famous soon enough
I don't see a problem: it converges monotonically. This is what I did:
- run 100 iterations with k-epsilon
- calculated Reynolds stress using R
- restarted with Launder-Reece-Rodi RSTM.

Converges smoothly with no trouble. I can either give in normal stress only at the inlet of the full equilibrium R from the k-epsilon model.

A few comments:
- your numerics is rubbish: you should try using second order
- if you try to start up LRR from the beginning it blows up because of epsilon. You should really start k-epsilon and restart; otherwise you will have fun trying to set up under-relaxation coefficients
- at the end of the residual graph you start hitting solver convergence tolerances: hence the plateau
- I can make this even better using my fixedMeanValue outlet b.c.: makes it prettier close to the outlet



Hrv
ingcorra likes this.
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   September 3, 2006, 12:00
Default Hi Hrvoje I didn't now abou
  #9
New Member
 
Steve Berg
Join Date: Mar 2009
Posts: 9
Rep Power: 8
sberg is on a distinguished road
Hi Hrvoje

I didn't now about the "R" function.

When I followed you steps the solution converged without problem.

Thank you

Steve
sberg is offline   Reply With Quote

Old   August 15, 2010, 07:14
Default
  #10
Senior Member
 
Daniele
Join Date: Feb 2010
Posts: 134
Rep Power: 7
Daniele111 is on a distinguished road
Hi
I try to use LRR for my simulation. I'm simulating an atmospheric boundary layer, but my result with it are completely different from the same case with k-eps model. Post my case.
Thanks
Attached Files
File Type: gz blayer3.tar.gz (4.1 KB, 61 views)
Daniele111 is offline   Reply With Quote

Old   February 25, 2014, 20:39
Default
  #11
Member
 
CHARLES
Join Date: May 2013
Posts: 46
Rep Power: 4
CHARLES is on a distinguished road
Quote:
Originally Posted by hjasak View Post
A few comments:
- your numerics is rubbish: you should try using second order
Hrv
Hrvoje,
Could you please provide an fvSchemes and fvSolution that aren't "rubbish"?
I'm not very well-versed in numerical methods (yet!) and would like to get a better idea of what 'good' settings for LRR are.

Thanks!
CHARLES 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
SimpleFoam convergence problems brahim OpenFOAM Running, Solving & CFD 20 June 9, 2015 09:09
What is phi in simpleFoam ehsan_vaghefi OpenFOAM Running, Solving & CFD 7 September 29, 2013 11:00
SimpleFoam problems with converging maybe skewness hoochie OpenFOAM Running, Solving & CFD 4 May 14, 2007 07:23
SimpleFoam woes msrinath80 OpenFOAM Bugs 2 April 13, 2007 10:15
SimpleFoam convergence problems schnitzlein OpenFOAM Running, Solving & CFD 6 June 24, 2005 09:51


All times are GMT -4. The time now is 09:27.