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

OpenFoam.1.7.x floatingObject tutorial case & MULES:alpha1 greater than 1

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

Reply
 
LinkBack Thread Tools Display Modes
Old   July 3, 2010, 13:04
Default OpenFoam.1.7.x floatingObject tutorial case & MULES:alpha1 greater than 1
  #1
Member
 
angel
Join Date: May 2009
Location: Spain
Posts: 46
Rep Power: 8
anmartin is on a distinguished road
Hello,
I have installed the OF.1.7.0 and the new OF1.7.x but I still continues trying to run the floating tutorial case without any success. I always obtain the following error.

Anybody know what it is possible that alpha start to increase and produce simulation crash?

Interface Courant Number mean: 0.00868469717822 max: 3.07048076829
Courant Number mean: 0.0214761703961 max: 3.07048076829
deltaT = 0.000368438312644
Time = 1.2731

Centre of mass: (0.373595449653 0.351882909424 0.482406400186)
Linear velocity: (-0.357961120598 -0.419740647472 -0.322074163028)
Angular velocity: (1.07106504184 -0.903173170713 -0.0110838047329)
GAMG: Solving for cellDisplacementx, Initial residual = 0.0056044966347, Final residual = 5.8395571122e-06, No Iterations 5
GAMG: Solving for cellDisplacementy, Initial residual = 0.00549399203972, Final residual = 5.71456061284e-06, No Iterations 5
GAMG: Solving for cellDisplacementz, Initial residual = 0.00997063228984, Final residual = 3.85256246304e-06, No Iterations 6
Execution time for mesh.update() = 1.15 s
time step continuity errors : sum local = 3.84344042594e-10, global = 2.49126712936e-11, cumulative = -0.000105905828067
GAMGPCG: Solving for pcorr, Initial residual = 1, Final residual = 2.81917055336e-06, No Iterations 7
time step continuity errors : sum local = 1.08353248665e-15, global = 2.55464254723e-16, cumulative = -0.000105905828067
MULES: Solving for alpha1
Liquid phase volume fraction = 0.533377598497 Min(alpha1) = -3.16898215629e+294 Max(alpha1) = 2.40723995432
#0 Foam::error:rintStack(Foam::Ostream&) in "/home/aml/OpenFOAM/OpenFOAM-1.7.x/lib/linux64GccDPOpt/libOpenFOAM.so"
#1 Foam::sigFpe::sigFpeHandler(int) in "/home/aml/OpenFOAM/OpenFOAM-1.7.x/lib/linux64GccDPOpt/libOpenFOAM.so"
#2 in "/lib/libc.so.6"
#3 Foam::fv::gaussGrad<double>::grad(Foam::GeometricF ield<double, Foam::fvsPatchField, Foam::surfaceMesh> const&) in "/home/aml/OpenFOAM/OpenFOAM-1.7.x/applications/bin/linux64GccDPOpt/interDyMFoam"
#4 Foam::fv::gaussGrad<double>::grad(Foam::GeometricF ield<double, Foam::fvPatchField, Foam::volMesh> const&) const in "/home/aml/OpenFOAM/OpenFOAM-1.7.x/lib/linux64GccDPOpt/libfiniteVolume.so"
#5 Foam::tmp<Foam::GeometricField<Foam:uterProduct< Foam::Vector<double>, double>::type, Foam::fvPatchField, Foam::volMesh> > Foam::fvc::grad<double>(Foam::GeometricField<doubl e, Foam::fvPatchField, Foam::volMesh> const&, Foam::word const&) in "/home/aml/OpenFOAM/OpenFOAM-1.7.x/lib/linux64GccDPOpt/libinterfaceProperties.so"
#6 Foam::tmp<Foam::GeometricField<Foam:uterProduct< Foam::Vector<double>, double>::type, Foam::fvPatchField, Foam::volMesh> > Foam::fvc::grad<double>(Foam::GeometricField<doubl e, Foam::fvPatchField, Foam::volMesh> const&) in "/home/aml/OpenFOAM/OpenFOAM-1.7.x/lib/linux64GccDPOpt/libinterfaceProperties.so"
#7 Foam::LimitedScheme<double, Foam::vanLeerLimiter<Foam::NVDTVD>, Foam::limitFuncs::magSqr>::limiter(Foam::Geometric Field<double, Foam::fvPatchField, Foam::volMesh> const&) const in "/home/aml/OpenFOAM/OpenFOAM-1.7.x/lib/linux64GccDPOpt/libfiniteVolume.so"
#8 Foam::limitedSurfaceInterpolationScheme<double>::w eights(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) const in "/home/aml/OpenFOAM/OpenFOAM-1.7.x/lib/linux64GccDPOpt/libinterfaceProperties.so"
#9 Foam::surfaceInterpolationScheme<double>::interpol ate(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) const in "/home/aml/OpenFOAM/OpenFOAM-1.7.x/lib/linux64GccDPOpt/libinterfaceProperties.so"
#10 Foam::fv::gaussConvectionScheme<double>::interpola te(Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) const in "/home/aml/OpenFOAM/OpenFOAM-1.7.x/lib/linux64GccDPOpt/libfiniteVolume.so"
#11 Foam::fv::gaussConvectionScheme<double>::flux(Foam ::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) const in "/home/aml/OpenFOAM/OpenFOAM-1.7.x/lib/linux64GccDPOpt/libfiniteVolume.so"
#12
in "/home/aml/OpenFOAM/OpenFOAM-1.7.x/applications/bin/linux64GccDPOpt/interDyMFoam"
#13
in "/home/aml/OpenFOAM/OpenFOAM-1.7.x/applications/bin/linux64GccDPOpt/interDyMFoam"
#14
in "/home/aml/OpenFOAM/OpenFOAM-1.7.x/applications/bin/linux64GccDPOpt/interDyMFoam"
#15 __libc_start_main in "/lib/libc.so.6"
#16
in "/home/aml/OpenFOAM/OpenFOAM-1.7.x/applications/bin/linux64GccDPOpt/interDyMFoam"
Floating point exception

I will be very grateful if somebody help me with this error
anmartin is offline   Reply With Quote

Old   July 3, 2010, 13:34
Default
  #2
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,894
Rep Power: 26
alberto will become famous soon enoughalberto will become famous soon enough
My guess:

Interface Courant Number mean: 0.00868469717822 max: 3.07048076829
Courant Number mean: 0.0214761703961 max: 3.07048076829
__________________
Alberto Passalacqua

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as live DVD/USB, hard drive image and virtual image.
OpenQBMM - An open-source implementation of quadrature-based moment methods
alberto is offline   Reply With Quote

Old   July 4, 2010, 12:28
Default
  #3
Member
 
angel
Join Date: May 2009
Location: Spain
Posts: 46
Rep Power: 8
anmartin is on a distinguished road
Hello,

Yes I know it but I have tried to limit the maxCo to 0.25 but it still continuous with the problem, at certain time (1.27), Co start to increase beyond 0.25 and stop the simulation.

I have tried to increase timePrecision but the problem persist, and I don't know what can I do.

Best regards,
anmartin is offline   Reply With Quote

Old   July 6, 2010, 06:14
Default
  #4
Senior Member
 
Join Date: Mar 2009
Posts: 854
Rep Power: 13
henry is on a distinguished road
This is an issue with the initialization (or lack of it) of the pressure (p_rgh) which imparts an unphysical impulse on the object which then moves further than the mesh-motion can cope with. We are reworking this tutorial to initialize the pressure correctly and will push the new version into 1.7.x when it is ready.

H
henry is offline   Reply With Quote

Old   July 6, 2010, 08:02
Default
  #5
Member
 
angel
Join Date: May 2009
Location: Spain
Posts: 46
Rep Power: 8
anmartin is on a distinguished road
ok thank you very much,

I look forward to the update

Thank you very much for your wonderful work

Angel
anmartin is offline   Reply With Quote

Old   July 7, 2010, 17:38
Default
  #6
Senior Member
 
Join Date: Mar 2009
Posts: 854
Rep Power: 13
henry is on a distinguished road
I found the problem and fixed it. Please pull the latest OpenFOAM-1.7.x and try it out.

H
henry is offline   Reply With Quote

Old   July 8, 2010, 03:10
Default
  #7
New Member
 
Khalid Abdulla
Join Date: Mar 2010
Posts: 2
Rep Power: 0
KhalidAbdulla is on a distinguished road
Hi,

I have just recently downloaded and installed OpenFOAM-1.7.x and pulled the latest update, but I am still getting an error very similar to the one described above and at about the same time-step (1.28s). Does the latest floatingObject case need to be downloaded from somewhere particular or is it just included in OF-1.7.x updates?

Also, out of interest, what was the problem that was resolved with this case? When I look at the solution I get up to 1.2s, following some water getting trapped above the floatingObject (as it resurfaces) there appears to be a shockwave in alpha (starting from this 'trapped' bit of water) through the entire solution volume (attached are 3 screenshots). Is it this shockwave reaching the mesh edge that causes the instability or is it a coincedence that's when my solution fails to converge?

Woops! henry - I just realised your post was dated last night so it's likely that my OF-1.7.x is out of date - I read the 'march' bit of your join date and thought it was an old post. Will get the update and let you know how I get on.
Attached Images
File Type: jpg alphaShockWave1.jpg (55.4 KB, 155 views)
File Type: jpg alphaShockWave2.jpg (55.3 KB, 124 views)
File Type: jpg alphaShockWave3.jpg (55.5 KB, 117 views)
KhalidAbdulla is offline   Reply With Quote

Old   July 8, 2010, 03:30
Default
  #8
Senior Member
 
Join Date: Mar 2009
Posts: 854
Rep Power: 13
henry is on a distinguished road
Did you recompile after downloading?

H
henry is offline   Reply With Quote

Old   July 8, 2010, 16:54
Default
  #9
New Member
 
Khalid Abdulla
Join Date: Mar 2010
Posts: 2
Rep Power: 0
KhalidAbdulla is on a distinguished road
Have now pulled the latest version and recompiled and run the case without any problems. Many thanks for all the work you must've put into this. Out of interest what was 'wrong' with the old case that was causing the instability?
- Khalid.
KhalidAbdulla is offline   Reply With Quote

Old   July 12, 2010, 05:25
Default
  #10
Member
 
angel
Join Date: May 2009
Location: Spain
Posts: 46
Rep Power: 8
anmartin is on a distinguished road
Many thanks,

Now i can run the tutorial example without any problem.

Best regards
anmartin is offline   Reply With Quote

Old   October 28, 2010, 10:44
Default
  #11
Senior Member
 
Ralph Moolenaar
Join Date: Aug 2010
Location: 's-Hertogenbosch, the Netherlands
Posts: 120
Rep Power: 7
Ralph M is on a distinguished road
Quote:
Originally Posted by KhalidAbdulla View Post
Have now pulled the latest version and recompiled and run the case without any problems. Many thanks for all the work you must've put into this. Out of interest what was 'wrong' with the old case that was causing the instability?
- Khalid.
Dear all,

I'm also interested in the problem with the pressure and also how to make it work.

I had no problems with running the mentioned tutorial (I have OF 1.7.1) but when using another floating object I see a sudden rise of Min(alpha1) from somewhere 1E-5 to 1E+295 in one iteration.

The Courant number is normal and slightly higher than the maximum given value in the ControlDict. Making this limit larger doesn't result in a converged result.

Another remarkable thing is that the angular velocity along the y-axis is becoming bigger. Tweaking the CoG result in a smaller velocity but the code explodes at the same timestep with the same sudden rise of Min(alpha1) as above.

Anyone any suggestions how to solve this problem? FYI: I'm trying to model the sinkage and trim of a boat.

Cheers,

Ralph
Ralph M is offline   Reply With Quote

Old   November 22, 2010, 11:24
Default
  #12
New Member
 
Join Date: Oct 2010
Posts: 23
Rep Power: 6
afo3 is on a distinguished road
has anyone figured out what was the problem and how was solutioned?? I have almost the same... after a certain number of timesteps, alpha1 becomes much greater than 1, so courant number increase and simulation stops...
afo3 is offline   Reply With Quote

Old   January 28, 2011, 16:51
Default
  #13
Member
 
Dave
Join Date: Jul 2010
Posts: 97
Rep Power: 7
daveatstyacht is on a distinguished road
To Ralph/All,
I noticed the same behavior on a hull set only to heave (the constraint moment goes through the roof) and alpha goes well above 1, time steps start shrinking while the courant number goes up and the simulation goes from perfectly normal to floating point error in two time steps of increasingly small size. It always occurs at the same time despite numerous attempts to make the solvers more robust. I am also using 1.7.1 and the simulation works fine without mesh motion.

Regards,
Dave
daveatstyacht is offline   Reply With Quote

Old   August 25, 2013, 12:13
Default
  #14
Member
 
Hrushi
Join Date: Jan 2013
Posts: 58
Rep Power: 4
hrushi.397 is on a distinguished road
I know I am couple of years late, but did anyone find solution to this problem?
hrushi.397 is offline   Reply With Quote

Old   August 25, 2013, 14:30
Default
  #15
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,511
Blog Entries: 34
Rep Power: 86
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Greetings Hrushi,

The latest talk I know of this topic is at this thread: The floating object tutorial
You can jump to the post #9 on that thread, if you want a very quick summary.

Best regards,
Bruno
wyldckat is offline   Reply With Quote

Old   August 28, 2013, 09:00
Default
  #16
New Member
 
Galchenko Olga
Join Date: Nov 2012
Posts: 16
Rep Power: 4
Galchenko is on a distinguished road
Hello, Hrushi!

Did you manage to solve the problem? I have read all the threads about this, but all my attempts to get a good converged solution failed. So I still wonder if someone was cleverer than me and found smth special)


Regards, Olga
Galchenko is offline   Reply With Quote

Old   August 28, 2013, 12:34
Default
  #17
Member
 
Hrushi
Join Date: Jan 2013
Posts: 58
Rep Power: 4
hrushi.397 is on a distinguished road
Hi Olga,

I am still trying. I tried doing it manually. I tried using

alpha1=alpha1>1?(1alpha1<0?0:alpha1));

But I am running into some logical model error now, unable to verify if this actually works. You can try and let me know.

Thanks

Hrushi
hrushi.397 is offline   Reply With Quote

Old   September 4, 2013, 07:52
Default
  #18
New Member
 
Galchenko Olga
Join Date: Nov 2012
Posts: 16
Rep Power: 4
Galchenko is on a distinguished road
Hi Hrushi!

This seems to be a kind of ignoring problems inside solving alpha1 equation or somewhere around.(anyway, I tried to use this, but got no results)
As I understand, alpha1 equation is solved by MULES, but can't find how. And are there any other shemes that can be used here?

Regards,
Olga
Galchenko is offline   Reply With Quote

Old   September 8, 2013, 01:30
Default
  #19
Member
 
Hrushi
Join Date: Jan 2013
Posts: 58
Rep Power: 4
hrushi.397 is on a distinguished road
Hi Olga,

I tried using shorter time step and it worked for me. I converted MULES equation into solve equation but I found the same result. Then I reduced the timestep, now I get max alpha1 as 1. I think you can try it in your problem too.

Regards,

Hrushi
hrushi.397 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
Request for pipe bifurcation fluent tutorial case Giorgos Momferratos FLUENT 0 October 20, 2008 15:10
case and dat file of FLUENT tutorial Sajad Ranjbaran FLUENT 0 November 8, 2006 07:55
Free surface boudary conditions with SOLA-VOF Fan Main CFD Forum 10 September 9, 2006 12:24
Compare stressedFoam and stressFemFoam in tutorial case plateHole weijing OpenFOAM Running, Solving & CFD 0 April 13, 2006 22:51
Case in Fluent Tutorial 1 Lam FLUENT 0 August 24, 2004 11:25


All times are GMT -4. The time now is 14:04.