CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > FLUENT > Fluent Multiphase

DDPM with RSM convergence problem

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   April 30, 2020, 08:36
Default DDPM with RSM convergence problem
  #1
New Member
 
mohamad ali mirzaei
Join Date: Feb 2017
Posts: 24
Rep Power: 6
mohamadalimirzaei1994 is on a distinguished road
I am trying to simulate a cyclone using DDPM and RSM with structured hexahedral mesh. although the mesh quality seems to be fine (Minimum Orthogonal Quality = 0.53), the solution diverges immediately after the start with the following warning:

turbulent viscosity limited to viscosity ratio of 1.000000e+05 in many cells
and then:
reverse flow at the outlet

the turbulent boundary condition is assigned at inlet using intensity and hydraulic diameter.
is there any solution method that might help?
at the moment I am using phase coupled SIMPLE, green-gauss node based, presto!, second-order upwind for momentum, quick for volume fraction and first-order upwind for the rest.

I ran the same simulation using sst-cc and it was fine. I tired converged solution of sst-cc as initial for RSM simulation bit it did not help. can you help find the problem?
mohamadalimirzaei1994 is offline   Reply With Quote

Old   April 30, 2020, 09:13
Default Rsm
  #2
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,948
Blog Entries: 1
Rep Power: 32
vinerm will become famous soon enough
k-\omega is not a good starting point for RSM; k-\varepsilon is. But even with k-\omega to begin with, you should be able to converge. Firstly, when the model is changed, URFs should be very very low, of the order of 0.01, so that the matrix could be developed. Use only first-order numerics and disable volume fraction for a few iterations. If the mesh is hex and structured, node based gradient does not add anything, so, prefer using LSQ.
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Old   April 30, 2020, 10:19
Default
  #3
New Member
 
mohamad ali mirzaei
Join Date: Feb 2017
Posts: 24
Rep Power: 6
mohamadalimirzaei1994 is on a distinguished road
Quote:
Originally Posted by vinerm View Post
k-\omega is not a good starting point for RSM; k-\varepsilon is. But even with k-\omega to begin with, you should be able to converge. Firstly, when the model is changed, URFs should be very very low, of the order of 0.01, so that the matrix could be developed. Use only first-order numerics and disable volume fraction for a few iterations. If the mesh is hex and structured, node based gradient does not add anything, so, prefer using LSQ.
thank you so much. so far, it seems that using very low URFs for the transition from one turbulence model to the other is solving the problem. just one question. with these very low UTFs (0.01) residuals are dropped in order of 10e-3 after a very low number of iteration at each time step (meaning that the convergence at each time step is achieved fast enough). so do you think it is ok to continue with these very low UFRs or these values must increase? if they must increase should it be gradually increased?
mohamadalimirzaei1994 is offline   Reply With Quote

Old   April 30, 2020, 10:23
Default URFs
  #4
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,948
Blog Entries: 1
Rep Power: 32
vinerm will become famous soon enough
You should increase the URFs otherwise there could be conservation issues. You can increase in two to three steps, say, every 10 time-steps.
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Old   April 30, 2020, 10:26
Default
  #5
New Member
 
mohamad ali mirzaei
Join Date: Feb 2017
Posts: 24
Rep Power: 6
mohamadalimirzaei1994 is on a distinguished road
Quote:
Originally Posted by vinerm View Post
You should increase the URFs otherwise there could be conservation issues. You can increase in two to three steps, say, every 10 time-steps.
and eventually, work with default values?
I mean, how can we ensure that our URFs are big enough??
mohamadalimirzaei1994 is offline   Reply With Quote

Old   April 30, 2020, 10:32
Default URFs
  #6
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,948
Blog Entries: 1
Rep Power: 32
vinerm will become famous soon enough
Yes, usually default values are good. However, if convergence is good within each time-step for given values of URF and URFs are not very small, say below 0.1, then its alright. With very small URFs, the changes in the coefficient matrix are so small and numerical solver considers everything converged. What happens in reality is that high frequency errors are reduced but low frequency errors remain. So, using high URFs are required but 0.5 and 0.9 won't make a difference as long as solution is well converged.
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Old   May 1, 2020, 05:33
Default
  #7
New Member
 
mohamad ali mirzaei
Join Date: Feb 2017
Posts: 24
Rep Power: 6
mohamadalimirzaei1994 is on a distinguished road
Quote:
Originally Posted by vinerm View Post
Yes, usually default values are good. However, if convergence is good within each time-step for given values of URF and URFs are not very small, say below 0.1, then its alright. With very small URFs, the changes in the coefficient matrix are so small and numerical solver considers everything converged. What happens in reality is that high frequency errors are reduced but low frequency errors remain. So, using high URFs are required but 0.5 and 0.9 won't make a difference as long as solution is well converged.
I started from 0.01 for all URFs and increased them all gradually up to 0.2 and up to there it was ok (residuals were drop enough after 2 or 3 iterations in each time steps), but when I increase them to 0.3, it immediately diverges (warning: very high turbulent viscosity ratio). is it normal?
in general is it ok to continue the simulation with 0.2 for URFs? how can we ensure that the final converged result is not affected by this value?
mohamadalimirzaei1994 is offline   Reply With Quote

Old   May 1, 2020, 15:02
Default URFs
  #8
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,948
Blog Entries: 1
Rep Power: 32
vinerm will become famous soon enough
If it is diverging with 0.3, then you can continue with 0.2 or 0.25. Once converged, which will take longer due to small URF, solution will be more or less independent of the URF used. Most importantly, you should set up some monitors. If those monitors become constant, then you can consider it converged.
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Reply

Tags
convergence, ddpm, rsm

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
SU2-7.0.1 on ubuntu 18.04 hyunko SU2 Installation 7 March 16, 2020 04:37
a problem with convergence in buoyantSimpleFoam skuznet OpenFOAM Running, Solving & CFD 6 November 15, 2017 12:12
convergence in rsm sharath21 ANSYS 0 June 22, 2014 15:12
Force can not converge colopolo CFX 13 October 4, 2011 22:03
Submerged fin, Convergence problem supermouniette FLUENT 10 July 6, 2009 10:47


All times are GMT -4. The time now is 04:10.