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

Residual rise

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

Like Tree1Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   July 29, 2010, 04:02
Default
  #21
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 3,145
Rep Power: 32
-mAx- will become famous soon enough
Quote:
Originally Posted by Mohsin View Post
After almost 9500 iterations for 1 million mesh. I got the following residulas with under relaxation for Pressure=0.35, momentum=0.6 and K and E equal to 0.5 each. Its confusing. (why increasing the mesh size from 0.21 million to 1 million caused even the continuity and velocity residuals to diverge keeping all other factors same).
Ok here it diverges
Well without the model I can't do more (and I don't have Fluent)

Try to switch with unsteady solver
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   July 29, 2010, 04:10
Default
  #22
Senior Member
 
Mohsin Mukhtar
Join Date: Mar 2010
Location: South Korea
Posts: 249
Rep Power: 9
Mohsin is on a distinguished road
Brrrrrrrrr

Well. I think i have to invite you here to South Korea to solve this one

Lets nap first and then think about some solutionThanks anyway....
Mohsin
Mohsin is offline   Reply With Quote

Old   October 13, 2011, 05:07
Default
  #23
New Member
 
m
Join Date: May 2011
Posts: 6
Rep Power: 7
riccia is on a distinguished road
hi mohsin,
it has been a year since your message. but i have a similar problem amd i would be glad if you could tell me how did you manage to solve this problem?
riccia is offline   Reply With Quote

Old   October 13, 2011, 10:25
Default
  #24
Senior Member
 
Mohsin Mukhtar
Join Date: Mar 2010
Location: South Korea
Posts: 249
Rep Power: 9
Mohsin is on a distinguished road
Please explain your problem....
Are u seeing residual rise in your solution?
Mohsin is offline   Reply With Quote

Old   October 13, 2011, 10:49
Default
  #25
New Member
 
m
Join Date: May 2011
Posts: 6
Rep Power: 7
riccia is on a distinguished road
yes. residuals decrease until 0.1 or 0.01 for 500~ iterations and then continuity strarts increasing and it diverges (e20 or so) at 1500~ iterations.
now i decreased URFs a lot and got a converged solution. i will try increasing URFs step by step.
so you have any other suggestions?
i am only solving turbulent flow and using k-epsilon model (realizable).
thanks already
riccia is offline   Reply With Quote

Old   October 13, 2011, 20:13
Default
  #26
Senior Member
 
Mohsin Mukhtar
Join Date: Mar 2010
Location: South Korea
Posts: 249
Rep Power: 9
Mohsin is on a distinguished road
Hello Riccia

Suggestions for you:

1. If the residuals rise (for example, first converge and then start to diverge) then wait for some iterations to see whether they converge again or not. If the resiudals don't converge and keep on diverging then there is a problem. The problem (MOSTLY) comes from poor mesh quality. Go back and try to improve your mesh quality. Use hexahedral meshes and avoid tetrahedral meshing scheme unless u have a very complex geometry. Mesh quality should be as follows for 3D.

a. Skewness for Hexahdral mesh elements should not exceed 0.8.
b. Skewness for tetrahderal elements should not exceed 0.85.

2. if the residuals keep on diverging, You SHOULD NOT change the URF to a very low value. If you change it to a very low value then apparently the solution would converge but it wont be accurate. For example you may not reduce the URF for momentum to 0.1 0r 0.01. If you use this value for momentum then the solution will drastically jump to convergence criteria specified by u. However, the solution would be wrong and inaccurate. So, at first, try to use the same URFs as provided by FLUENT (Default). If you get fluctuations then it means you have to change some urf to get steady lines. The following URF values mostly work for me.

a. Presure: 0.4
b. Momenutm: 0.6
c. Turbulent kinetic energy=0.6
d. Turbluent dissipation=0.6
e. Rest=Default

3. Discretization scheme: Use of discretization scheme may also affect. Choose the best discritization scheme for ur problem which do not give you divergence. for example: If swirl is there in ur flow then i would recommend PRESTO scheme.

4. Turbulence scheme: You may also try to find appropriate scheme for turbulence in order to get steady converged solution.

5. last but not least, Residulas are not the only convergence criteria. For instance, if your residulas are not going below 10-3 then let it be there and check the mass flux (in and out) if the valuesof total mass flux in and out are (for example) lesser than 10-4 then your solution might be converged.You can also monitor the surface intgrals on some point of importance in ur domain and call ur solution converged when the value is not changing.

Keeping in view the aforementioned points, try to solve your problem. I hope you will get a solution.

Good luck

Last edited by Mohsin; October 24, 2011 at 20:07.
Mohsin is offline   Reply With Quote

Old   July 23, 2013, 13:32
Default
  #27
New Member
 
Honey
Join Date: Mar 2011
Location: Finland
Posts: 18
Rep Power: 7
Honey is on a distinguished road
Quote:
Originally Posted by Mohsin View Post
Convergence Criteria
Contours
flux reports

In the previous case of 1200 iterations all were satisfied. Would you still recommend to iterate more? (if i iterate more the residuals for K and E will cross the convergence limit and never converge)
I have the same problem, somehow. The residuals are decreasing for the first 700 iterations to about 1e-4 but then suddenly it increases to about 1e+2. After following your problem here, I have ended up with your last post which is still a problem without any solution.

I am wondering whether you have solved the problem?? if yes, could you kindly post here what steps you took??

Or, is there anyone here who can help??

Thank you in advance
Honey is offline   Reply With Quote

Old   July 23, 2013, 14:00
Default
  #28
New Member
 
Honey
Join Date: Mar 2011
Location: Finland
Posts: 18
Rep Power: 7
Honey is on a distinguished road
Quote:
Originally Posted by Mohsin View Post
Hello Riccia

Suggestions for you:

1. If the residuals rise (for example, first converge and then start to diverge) then wait for some iterations to see whether they converge again or not. If the resiudals don't converge and keep on diverging then there is a problem. The problem (MOSTLY) comes from poor mesh quality. Go back and try to improve your mesh quality. Use hexahedral meshes and avoid tetrahedral meshing scheme unless u have a very complex geometry. Mesh quality should be as follows for 3D.

a. Skewness for Hexahdral mesh elements should not exceed 0.8.
b. Skewness for tetrahderal elements should not exceed 0.85.

2. if the residuals keep on diverging, You SHOULD NOT change the URF to a very low value. If you change it to a very low value then apparently the solution would converge but it wont be accurate. For example you may not reduce the URF for momentum to 0.1 0r 0.01. If you use this value for momentum then the solution will drastically jump to convergence criteria specified by u. However, the solution would be wrong and inaccurate. So, at first, try to use the same URFs as provided by FLUENT (Default). If you get fluctuations then it means you have to change some urf to get steady lines. The following URF values mostly work for me.

a. Presure: 0.4
b. Momenutm: 0.6
c. Turbulent kinetic energy=0.6
d. Turbluent dissipation=0.6
e. Rest=Default

3. Discretization scheme: Use of discretization scheme may also affect. Choose the best discritization scheme for ur problem which do not give you divergence. for example: If swirl is there in ur flow then i would recommend PRESTO scheme.

4. Turbulence scheme: You may also try to find appropriate scheme for turbulence in order to get steady converged solution.

5. last but not least, Residulas are not the only convergence criteria. For instance, if your residulas are not going below 10-3 then let it be there and check the mass flux (in and out) if the valuesof total mass flux in and out are (for example) lesser than 10-4 then your solution might be converged.You can also monitor the surface intgrals on some point of importance in ur domain and call ur solution converged when the value is not changing.

Keeping in view the aforementioned points, try to solve your problem. I hope you will get a solution.

Good luck
Sorry for the previous message, in fact I got access to the rest of the conversation (on the other page) right after posting the message.

Anyway, I got your suggestions. I have implemented most of them but did not lead me to a converge solution yet. Now, I will try to refine the mesh size even though the mesh quality for the current case is relatively good. Hopefully I will manage to get a good converged solution if not then I would most probably need your help!
Honey is offline   Reply With Quote

Old   July 24, 2013, 02:06
Default
  #29
Senior Member
 
Saeed
Join Date: Jan 2013
Posts: 177
Rep Power: 5
flow_CH is on a distinguished road
Hi.
I am modeling a open channel flow.
What the problem of this residuals?
Can you tell this is going to diverge or not?
please see image
thanks
Attached Images
File Type: jpg 52.jpg (69.5 KB, 31 views)

Last edited by flow_CH; July 31, 2013 at 04:26.
flow_CH 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
How to write k and epsilon before the abnormal end xiuying OpenFOAM Running, Solving & CFD 8 August 27, 2013 15:33
Floating point exception error Alan OpenFOAM Running, Solving & CFD 10 April 6, 2012 14:02
Low Mach number Compressible jet flow using LES ankgupta8um OpenFOAM Running, Solving & CFD 7 January 15, 2011 14:38
Computational time sunnysun OpenFOAM Running, Solving & CFD 5 March 16, 2009 04:32
Differences between serial and parallel runs carsten OpenFOAM Bugs 11 September 12, 2008 11:16


All times are GMT -4. The time now is 08:28.