# Residual rise

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

July 29, 2010, 05:02
#21
Super Moderator

Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 3,291
Rep Power: 36
Quote:
 Originally Posted by Mohsin 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

 July 29, 2010, 05:10 #22 Senior Member   Mohsin Mukhtar Join Date: Mar 2010 Location: South Korea Posts: 249 Rep Power: 12 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

 October 13, 2011, 06:07 #23 New Member   m Join Date: May 2011 Posts: 6 Rep Power: 10 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?

 October 13, 2011, 11:25 #24 Senior Member   Mohsin Mukhtar Join Date: Mar 2010 Location: South Korea Posts: 249 Rep Power: 12 Please explain your problem.... Are u seeing residual rise in your solution?

 October 13, 2011, 11:49 #25 New Member   m Join Date: May 2011 Posts: 6 Rep Power: 10 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

 October 13, 2011, 21:13 #26 Senior Member   Mohsin Mukhtar Join Date: Mar 2010 Location: South Korea Posts: 249 Rep Power: 12 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 21:07.

July 23, 2013, 14:32
#27
New Member

Honey
Join Date: Mar 2011
Location: Dmg
Posts: 23
Rep Power: 10
Quote:
 Originally Posted by Mohsin 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??

July 23, 2013, 15:00
#28
New Member

Honey
Join Date: Mar 2011
Location: Dmg
Posts: 23
Rep Power: 10
Quote:
 Originally Posted by Mohsin 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!

July 24, 2013, 03:06
#29
Senior Member

Saeed
Join Date: Jan 2013
Posts: 193
Rep Power: 8
Hi.
I am modeling a open channel flow.
What the problem of this residuals?
Can you tell this is going to diverge or not?
thanks
Attached Images
 52.jpg (69.5 KB, 69 views)

Last edited by flow_CH; July 31, 2013 at 05:26.

 November 21, 2018, 14:37 #30 New Member   mehran mohammadi Join Date: Aug 2016 Posts: 12 Rep Power: 5 hi Mohsin I'm master student and work on swirl flow . i have problem like your's would you pleas help me if you solve your problem. thank you

 October 14, 2019, 08:05 #31 Member   Arthur Join Date: Aug 2014 Location: Italy Posts: 38 Rep Power: 7 Many have already answered to this question. You should monitor the interested quantities to understand if the solution converged or didn't. Anyway having continuity residual of 10e-2 order is too high from my experience. In this cases check the BC, it can be generated by recirculations on outlet.