How to avoid the sudden divergence

Haoran

unread,

May 16, 2019, 4:08:26 AM5/16/19

to Nek5000

Hi Neks,

Recently I meet a tough problem. During the calculation process , the Courant number will increase sharply in a several steps. I have try to decrease the fixed time step, reduce Re to solve the problem but I failed.

Do you have any suggestions about it? Part of the log file is appended below. Thank you for your support in advance.

Haoran

1. part of log

Step 865, t= 9.9465381E+01, DT= 1.0000000E-03, C= 0.676 1.1732E+04 3.7107E+01

Solving for fluid

865 Project PRES 6.5182E-02 1.2862E+02 1.9732E+03 8 8

865 PRES gmres 510 1.3665E-04 1.8470E-03 1.0000E-04 2.2139E+01 3.8261E+01 F

865 Hmholtz VELX 42 7.3102E-08 5.2118E+00 1.0000E-07

865 Hmholtz VELY 40 8.4808E-08 4.2469E+00 1.0000E-07

865 Hmholtz VELZ 60 8.2604E-08 1.8329E+03 1.0000E-07

865 volflow Z 1.8361E+03 3.1092E+01 4.3972E-02 3.1136E+01

L1/L2 DIV(V) 2.4790E-02 1.0814E+00

L1/L2 QTL 0.0000E+00 0.0000E+00

L1/L2 DIV(V)-QTL 2.4790E-02 1.0814E+00

WARNING: DIV(V)-QTL too large!

865 Fluid done 9.9465E+01 4.0846E+01

Step 866, t= 9.9466381E+01, DT= 1.0000000E-03, C= 0.676 1.1773E+04 4.1043E+01

Solving for fluid

866 Project PRES 5.8296E-02 1.2862E+02 2.2063E+03 8 8

866 PRES gmres 510 1.8368E-04 1.6519E-03 1.0000E-04 2.2711E+01 3.8805E+01 F

866 Hmholtz VELX 42 7.3101E-08 5.2125E+00 1.0000E-07

866 Hmholtz VELY 40 8.4875E-08 4.2672E+00 1.0000E-07

866 Hmholtz VELZ 60 8.2604E-08 1.8329E+03 1.0000E-07

866 volflow Z 1.8361E+03 3.1092E+01 4.3972E-02 3.1136E+01

L1/L2 DIV(V) 2.4790E-02 1.0820E+00

L1/L2 QTL 0.0000E+00 0.0000E+00

L1/L2 DIV(V)-QTL 2.4790E-02 1.0820E+00

WARNING: DIV(V)-QTL too large!

866 Fluid done 9.9466E+01 4.1382E+01

Step 867, t= 9.9467381E+01, DT= 1.0000000E-03, C= 0.677 1.1814E+04 4.1591E+01

Solving for fluid

867 Project PRES 7.6838E-02 1.2862E+02 1.6739E+03 8 8

867 PRES gmres 510 2.2527E-04 2.1773E-03 1.0000E-04 2.2423E+01 3.8507E+01 F

867 Hmholtz VELX 42 7.3104E-08 5.2139E+00 1.0000E-07

867 Hmholtz VELY 40 8.4996E-08 4.3027E+00 1.0000E-07

867 Hmholtz VELZ 60 8.2604E-08 1.8329E+03 1.0000E-07

867 volflow Z 1.8361E+03 3.1092E+01 4.3976E-02 3.1136E+01

L1/L2 DIV(V) 2.4790E-02 1.0829E+00

L1/L2 QTL 0.0000E+00 0.0000E+00

L1/L2 DIV(V)-QTL 2.4790E-02 1.0829E+00

WARNING: DIV(V)-QTL too large!

867 Fluid done 9.9467E+01 4.1102E+01

Step 868, t= 9.9468381E+01, DT= 1.0000000E-03, C= 0.807 1.1856E+04 4.1353E+01

Solving for fluid

868 Project PRES 1.4022E-01 1.2863E+02 9.1734E+02 8 8

868 PRES gmres 510 3.7823E-04 3.9732E-03 1.0000E-04 2.3275E+01 3.9419E+01 F

868 Hmholtz VELX 42 7.3110E-08 5.2168E+00 1.0000E-07

868 Hmholtz VELY 40 8.5203E-08 4.3706E+00 1.0000E-07

868 Hmholtz VELZ 60 8.2604E-08 1.8329E+03 1.0000E-07

868 volflow Z 1.8361E+03 3.1092E+01 4.3978E-02 3.1136E+01

L1/L2 DIV(V) 2.4790E-02 1.0843E+00

L1/L2 QTL 0.0000E+00 0.0000E+00

L1/L2 DIV(V)-QTL 2.4790E-02 1.0843E+00

WARNING: DIV(V)-QTL too large!

868 Fluid done 9.9468E+01 4.2031E+01

Step 869, t= 9.9469381E+01, DT= 1.0000000E-03, C= 0.956 1.1898E+04 4.2248E+01

Solving for fluid

869 Project PRES 1.8068E-01 1.2864E+02 7.1200E+02 8 8

869 PRES gmres 510 4.0328E-04 5.1196E-03 1.0000E-04 2.2137E+01 3.8222E+01 F

869 Hmholtz VELX 42 7.3124E-08 5.2233E+00 1.0000E-07

869 Hmholtz VELY 40 8.5564E-08 4.5171E+00 1.0000E-07

869 Hmholtz VELZ 60 8.2604E-08 1.8329E+03 1.0000E-07

869 volflow Z 1.8361E+03 3.1092E+01 4.3972E-02 3.1136E+01

L1/L2 DIV(V) 2.4790E-02 1.0869E+00

L1/L2 QTL 0.0000E+00 0.0000E+00

L1/L2 DIV(V)-QTL 2.4790E-02 1.0869E+00

WARNING: DIV(V)-QTL too large!

869 Fluid done 9.9469E+01 4.0833E+01

Step 870, t= 9.9470381E+01, DT= 1.0000000E-03, C= 1.110 1.1939E+04 4.1170E+01

Solving for fluid

870 Project PRES 4.0948E-01 1.2869E+02 3.1428E+02 8 8

870 PRES gmres 510 9.2960E-04 1.1603E-02 1.0000E-04 2.2244E+01 3.8336E+01 F

870 Hmholtz VELX 42 7.3183E-08 5.2411E+00 1.0000E-07

870 Hmholtz VELY 40 8.6194E-08 4.8911E+00 1.0000E-07

870 Hmholtz VELZ 60 8.2604E-08 1.8329E+03 1.0000E-07

870 volflow Z 1.8361E+03 3.1092E+01 4.3966E-02 3.1136E+01

L1/L2 DIV(V) 2.4790E-02 1.0924E+00

L1/L2 QTL 0.0000E+00 0.0000E+00

L1/L2 DIV(V)-QTL 2.4790E-02 1.0924E+00

WARNING: DIV(V)-QTL too large!

870 Fluid done 9.9470E+01 4.0950E+01

Step 871, t= 9.9471381E+01, DT= 1.0000000E-03, C= 1.720 1.1980E+04 4.1196E+01

Solving for fluid

871 Project PRES 8.0954E-01 1.2895E+02 1.5929E+02 8 8

871 PRES gmres 510 1.8954E-03 2.2939E-02 1.0000E-04 2.2305E+01 3.8383E+01 F

871 Hmholtz VELX 42 7.3411E-08 5.3072E+00 1.0000E-07

871 Hmholtz VELY 40 8.7196E-08 6.0546E+00 1.0000E-07

871 Hmholtz VELZ 60 8.2604E-08 1.8329E+03 1.0000E-07

871 volflow Z 1.8361E+03 3.1092E+01 4.3962E-02 3.1136E+01

L1/L2 DIV(V) 2.4790E-02 1.1075E+00

L1/L2 QTL 0.0000E+00 0.0000E+00

L1/L2 DIV(V)-QTL 2.4790E-02 1.1075E+00

WARNING: DIV(V)-QTL too large!

871 Fluid done 9.9471E+01 4.0959E+01

Step 872, t= 9.9472381E+01, DT= 1.0000000E-03, C= 3.841 1.2021E+04 4.1161E+01

Solving for fluid

872 Project PRES 3.9845E+00 1.3113E+02 3.2910E+01 8 8

872 PRES gmres 510 8.9476E-03 1.1290E-01 1.0000E-04 2.2963E+01 3.9068E+01 F

872 Hmholtz VELX 42 7.4327E-08 5.6950E+00 1.0000E-07

872 Hmholtz VELY 40 8.8701E-08 1.0373E+01 1.0000E-07

872 Hmholtz VELZ 60 8.2604E-08 1.8329E+03 1.0000E-07

872 volflow Z 1.8361E+03 3.1092E+01 4.4019E-02 3.1136E+01

L1/L2 DIV(V) 2.4789E-02 1.1739E+00

L1/L2 QTL 0.0000E+00 0.0000E+00

L1/L2 DIV(V)-QTL 2.4789E-02 1.1739E+00

WARNING: DIV(V)-QTL too large!

872 Fluid done 9.9472E+01 4.1656E+01

CFL, Ctarg! 13.308803137801068 0.50000000000000000

873 9.9472E+01 Write checkpoint

FILE:/home/Nek5000/run/re10000/turb0.f00005

2 Emergency exit: 873 time = 99.472381418594168

Latest solution and data are dumped for post-processing.

*** STOP ***

2. part of .par file

#

# nek parameter file

#

[GENERAL]

#startFrom = turb0.f00001

stopAt = endTime

endTime = 2000.0

dt = 1.0e-03

#dt = 0

timeStepper = bdf3

extrapolation = OIFS

variableDt = yes

targetCFL = 1.5

writeControl = runTime

writeInterval = 0.2

filtering = hpfrt

filterWeight = 10

filterCutoffRatio = 0.9

[PROBLEMTYPE]

variableProperties = no

equation = incompNS

[PRESSURE]

preconditioner = semg_amg

residualTol = 1e-04

residualProj = yes

[VELOCITY]

residualTol = 1e-07

density = 1

residualProj = no

viscosity = -7500

Divyansh Khattak

unread,

May 16, 2019, 4:12:04 AM5/16/19

to Haoran, Nek5000

You may try using variable time-stepping which will try to keep your Courant number near the value specified in your targetCFL in par file or parameter(26) in your rea file.

--
You received this message because you are subscribed to the Google Groups "Nek5000" group.
To unsubscribe from this group and stop receiving emails from it, send an email to nek5000+u...@googlegroups.com.
To post to this group, send email to nek...@googlegroups.com.
Visit this group at https://groups.google.com/group/nek5000.
To view this discussion on the web visit https://groups.google.com/d/msgid/nek5000/49c055ff-cbc5-4b68-9528-0509a12a9de7%40googlegroups.com.
For more options, visit https://groups.google.com/d/optout.

--

Divyansh Khattak

Graduate Student, Mechanical Science and Engineering,

University of Illinois, Urbana Champaign

Gmail, Illinois WebMail

Phone: +12179045789

Haoran

unread,

May 16, 2019, 5:28:15 AM5/16/19

to Nek5000

Thank you for your rapid reply. Khattak. And could you please give other suggestions to get a steady state of fully developed turbulent flow from a initial flow field in complex geometry? Thank you for your kindness.

Haoran

在 2019年5月16日星期四 UTC+8下午4:12:04，Divyansh Khattak写道：

To unsubscribe from this group and stop receiving emails from it, send an email to nek5000+unsubscribe@googlegroups.com.

To post to this group, send email to nek...@googlegroups.com.
Visit this group at https://groups.google.com/group/nek5000.
To view this discussion on the web visit https://groups.google.com/d/msgid/nek5000/49c055ff-cbc5-4b68-9528-0509a12a9de7%40googlegroups.com.
For more options, visit https://groups.google.com/d/optout.

Fischer, Paul

unread,

May 16, 2019, 8:18:07 AM5/16/19

to Haoran, Nek5000

Dear Haoran,

What is your geometry?

Have you looked (with visit) at the solution at times well before and just before

blow-up to see where it is blowing up?

It's possible that you have inflow coming into the outflow boundary, which

would not be resolved by reducing dt. If this is the case, you should use

turb_outflow or one of the other options. (grep turb_outflow Nek5000/core/navier5.f).

It's troubling that your pressure iteration counts are 510 per timestep---they should

be ~20 or so.

Paul

From: nek...@googlegroups.com <nek...@googlegroups.com> on behalf of Haoran <juhao...@gmail.com>
Sent: Thursday, May 16, 2019 4:28:15 AM
To: Nek5000
Subject: Re: [nek5000] How to avoid the sudden divergence

To unsubscribe from this group and stop receiving emails from it, send an email to nek5000+u...@googlegroups.com.

To post to this group, send email to nek...@googlegroups.com.
Visit this group at https://groups.google.com/group/nek5000.

To view this discussion on the web visit https://groups.google.com/d/msgid/nek5000/2a36e187-bc17-494f-8211-c3668d47fb13%40googlegroups.com.

Haoran

unread,

May 16, 2019, 10:12:22 PM5/16/19

to Nek5000

Dear Prof. fischer,

Thank you for your reply, Actually I am working with a 3by3 rod bundle with one pair of periodic boundaries through the flow direction. The way to add driving force in my case studies from turbChannel case. Now I am on the way from initial flow field to steady field with Re =10000 where iterations in PRES steps vary in each step at range from 30-130. The velocity contour near the divergence is attached below. Could you please give some comments about my case? Thank you very much for your time and support !

Haoran

在 2019年5月16日星期四 UTC+8下午8:18:07，fischerp写道：

123.png

Pau Fradera

unread,

Mar 26, 2025, 10:21:35 PM3/26/25

to Nek5000

Dear Paul Fischer,

I was reviewing some old discussions and I wanted to ask you if you or someone could clarify how do you know that the pressure iteration counts on that case were supposed to be ~20? I would really like to understand how you were able to know this. Is that something that is always like that? or you guessed this based on something that was shown on that logfile?

Thanks in advance to you or to anyone that can help me with this question.

Sincerely,

Pau

El dia dijous, 16 de maig del 2019 a les 5:18:07 UTC-7, fischerp va escriure:

To unsubscribe from this group and stop receiving emails from it, send an email to nek5000+u...@googlegroups.com.
To post to this group, send email to nek...@googlegroups.com.
Visit this group at https://groups.google.com/group/nek5000.
To view this discussion on the web visit https://groups.google.com/d/msgid/nek5000/49c055ff-cbc5-4b68-9528-0509a12a9de7%40googlegroups.com.
For more options, visit https://groups.google.com/d/optout.

--

Divyansh Khattak

Graduate Student, Mechanical Science and Engineering,

University of Illinois, Urbana Champaign

Gmail, Illinois WebMail

Phone: +12179045789

--
You received this message because you are subscribed to the Google Groups "Nek5000" group.

Philipp Schlatter

unread,

Mar 27, 2025, 2:49:10 AM3/27/25

to nek...@googlegroups.com

pressure iterations, once the flow has stabilised, should be somehwere between 10 and 30, so ~20.

To view this discussion visit https://groups.google.com/d/msgid/nek5000/eb10d0d9-59a2-4ad3-92a5-5dce621c98a6n%40googlegroups.com.

Fischer, Paul

unread,

Mar 27, 2025, 8:37:00 AM3/27/25

to Pau Fradera, Nek5000

Dear Pau,

Philipp is correct re. expected behavior.

We have developed scalable solvers for Nek5000/RS using multilevel preconditioners. Generally, these are based on local p multigrid within each element coupled with a scalable coarse-grid solver for the unstructured mesh comprising the initial 8 vertices of each element.

Occasionally if the mesh has extremely high aspect ratio cells we see something going up to 100 or so iterations, but 500 is an indicator that something is broken.

Often, the solution has blown up by that point and the initial residual is very large (e.g., 1e10), which makes it difficult to get down to 1e-4 or 1e-6, which are standard target values when the equations are nondimensionalized using a convective time scale.

hth.

Paul Fischer

From: nek...@googlegroups.com <nek...@googlegroups.com> on behalf of Pau Fradera <pau.fr...@gmail.com>
Sent: Wednesday, March 26, 2025 9:21 PM
To: Nek5000 <nek...@googlegroups.com>

Pau Fradera

unread,

Jun 12, 2025, 3:11:41 PM6/12/25

to Nek5000

Dear Paul and Philipp,

Thank you very much for your replies and for the very interesting information. I really appreciate it.

Thank you.

Sincerely,

Pau

El dia dijous, 27 de març del 2025 a les 5:37:00 UTC-7, fischerp va escriure:

Reply all

Reply to author

Forward