CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

wingMotion tutorial

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

Reply
 
LinkBack Thread Tools Display Modes
Old   October 15, 2014, 22:29
Default wingMotion tutorial
  #1
Senior Member
 
Join Date: Jan 2013
Posts: 118
Rep Power: 5
kkpal is on a distinguished road
Is it just me or does someone else also meet this problem that the wingMotion tutorial with the pimpleDyMFoam solver does not run smoothly? It blows off after a few seconds.
kkpal is offline   Reply With Quote

Old   October 18, 2014, 17:15
Default
  #2
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 9,736
Blog Entries: 39
Rep Power: 103
wyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of light
Quick questions:
  1. Which version of OpenFOAM are you using?
  2. How exactly have you installed it and in which Linux Distribution?
  3. What commands did you use to execute that tutorial?
wyldckat is offline   Reply With Quote

Old   October 21, 2014, 02:32
Default
  #3
Senior Member
 
Join Date: Jan 2013
Posts: 118
Rep Power: 5
kkpal is on a distinguished road
Quote:
Originally Posted by wyldckat View Post
Quick questions:
  1. Which version of OpenFOAM are you using?
  2. How exactly have you installed it and in which Linux Distribution?
  3. What commands did you use to execute that tutorial?
Dear Bruno
1. I'm using OF-2.2.2.
2. I installed it on Ubuntu 12.04 following the steps on the website, there was no error in the installation.
3. I went inside the tutorial folder and run ./Allrun, after some time the simulation blew off.
kkpal is offline   Reply With Quote

Old   October 26, 2014, 14:08
Default
  #4
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 9,736
Blog Entries: 39
Rep Power: 103
wyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of light
Hi Kai,

Sorry, I forgot to ask the other day:
  1. What does this command give you?
    Code:
    uname -m
  2. How much memory is available in your system where you have OpenFOAM installed? You can check by running:
    Code:
    free -m
    The values shown are in Megabyte. For example, I get in a virtual machine I have:
    Code:
                 total       used       free     shared    buffers     cached
    Mem:          2970       1566       1403          0        103        982
    -/+ buffers/cache:        481       2489
    Swap:         2149          0       2149
    Which means I have roughly 3GB of RAM in this VM.
  3. Where exactly are you running this tutorial case? In other words, what exact steps have you taken for running this tutorial?
  4. edit: What is the error message contained in the log file for the application that crashed? For example, in the file "log.pimpleDyMFoam".
I ask all of this, because I'm not getting any problems when running this tutorial within a 64-bit VM with Ubuntu 12.04 installed, using the Deb package for OpenFOAM 2.2.2.

Best regards,
Bruno
__________________

Last edited by wyldckat; October 26, 2014 at 14:11. Reason: see "edit:"
wyldckat is offline   Reply With Quote

Old   October 26, 2014, 23:19
Default
  #5
Senior Member
 
Join Date: Jan 2013
Posts: 118
Rep Power: 5
kkpal is on a distinguished road
Dear Bruno
Thank you so much for your help.

1. x86_64 is the message I got when I run "uname -m";

2. The outcome of the second command is as follows
Code:
             total       used       free     shared    buffers     cached
Mem:          3849       3725        124          0         29        621
-/+ buffers/cache:       3074        775
Swap:         3990        406       3584
3. I ran the wingMotion case by typing ./Allrun in the terminal, I thought it would run smoothly since it is the direct copy from the tutorial cases.

4. The final message before blowing off is as follows:
Code:
Courant Number mean: 0.0004682635789 max: 0.2862657354
deltaT = 3.052758308e-68
--> FOAM Warning : 
    From function Time::operator++()
    in file db/Time/Time.C at line 1039
    Increased the timePrecision from 100385 to 100386 to distinguish between timeNames at time 0.1214197262
Time = 0.12141972624829507065857825409693759866058826446533203125

forces forces:

Restraint verticalSpring:  attachmentPt - anchor (5.800915304e-13 0.4647287209 0) spring length 0.4647287209 force (3.836546021e+46 3.073572069e+58 0) moment (0 0 0)
Restraint axialSpring:  angle -0.4669738203 force (0 0 0) moment (0 0 1.251171106e+59)
sixDoFRigidBodyMotion constraints converged in 1 iterations
Constraint force: (7.680846272e+124 0 0)
Constraint moment: (0 0 -1.018350594e+124)
Centre of mass: (0.4602888171 0.3391455969 0.125)
Linear velocity: (-3.333562493e+58 -6.831970333e+58 1.803187061e+40)
Angular velocity: (-1.595451218e+43 1.373302302e+43 -2.514046212e+59)
GAMG:  Solving for cellDisplacementx, Initial residual = 1.449473414e-05, Final residual = 4.055903807e-07, No Iterations 1
GAMG:  Solving for cellDisplacementy, Initial residual = 1.567565678e-05, Final residual = 4.429352025e-07, No Iterations 1
GAMG:  Solving for pcorr, Initial residual = 1, Final residual = 0.01395209455, No Iterations 3
time step continuity errors : sum local = 2.097306466e-12, global = -2.419682597e-13, cumulative = -0.001640880809
PIMPLE: iteration 1
DILUPBiCG:  Solving for Ux, Initial residual = 0.007411702271, Final residual = 4.453006086e-07, No Iterations 1
DILUPBiCG:  Solving for Uy, Initial residual = 0.001423361926, Final residual = 4.040040461e-08, No Iterations 1
GAMG:  Solving for p, Initial residual = 0.5250081574, Final residual = 0.003301159186, No Iterations 6
time step continuity errors : sum local = 7.137773976e-10, global = 1.448669154e-12, cumulative = -0.001640880807
PIMPLE: iteration 2
DILUPBiCG:  Solving for Ux, Initial residual = 0.001269659141, Final residual = 1.680689543e-07, No Iterations 1
DILUPBiCG:  Solving for Uy, Initial residual = 0.0002382044039, Final residual = 2.017258382e-08, No Iterations 1
GAMG:  Solving for p, Initial residual = 0.3536207741, Final residual = 8.84514014e-08, No Iterations 27
time step continuity errors : sum local = 2.058861651e-14, global = 2.679274617e-15, cumulative = -0.001640880807
DILUPBiCG:  Solving for omega, Initial residual = 9.345672593e-05, Final residual = 2.178608942e-07, No Iterations 1
[1] #0  Foam::error::printStack(Foam::Ostream&) in "/opt/openfoam222/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[1] #1  Foam::sigFpe::sigHandler(int) in "/opt/openfoam222/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[1] #2   in "/lib/x86_64-linux-gnu/libc.so.6"
[1] #3  double Foam::sumProd<double>(Foam::UList<double> const&, Foam::UList<double> const&) in "/opt/openfoam222/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[1] #4  Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/opt/openfoam222/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[1] #5  Foam::fvMatrix<double>::solveSegregated(Foam::dictionary const&) in "/opt/openfoam222/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
[1] #6  Foam::fvMatrix<double>::solve(Foam::dictionary const&) in "/opt/openfoam222/platforms/linux64GccDPOpt/lib/libincompressibleRASModels.so"
[1] #7  Foam::fvMatrix<double>::solve() in "/opt/openfoam222/platforms/linux64GccDPOpt/lib/libincompressibleRASModels.so"
[1] #8  Foam::incompressible::RASModels::kOmegaSST::correct() in "/opt/openfoam222/platforms/linux64GccDPOpt/lib/libincompressibleRASModels.so"
[1] #9  
[1]  in "/opt/openfoam222/platforms/linux64GccDPOpt/bin/pimpleDyMFoam"
[1] #10  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
[1] #11  
[1]  in "/opt/openfoam222/platforms/linux64GccDPOpt/bin/pimpleDyMFoam"
[zk:12297] *** Process received signal ***
[zk:12297] Signal: Floating point exception (8)
[zk:12297] Signal code:  (-6)
[zk:12297] Failing at address: 0x3e800003009
[zk:12297] [ 0] /lib/x86_64-linux-gnu/libc.so.6(+0x364a0) [0x7f29d620c4a0]
[zk:12297] [ 1] /lib/x86_64-linux-gnu/libc.so.6(gsignal+0x35) [0x7f29d620c425]
[zk:12297] [ 2] /lib/x86_64-linux-gnu/libc.so.6(+0x364a0) [0x7f29d620c4a0]
[zk:12297] [ 3] /opt/openfoam222/platforms/linux64GccDPOpt/lib/libOpenFOAM.so(_ZN4Foam7sumProdIdEEdRKNS_5UListIT_EES5_+0x39) [0x7f29d744c549]
[zk:12297] [ 4] /opt/openfoam222/platforms/linux64GccDPOpt/lib/libOpenFOAM.so(_ZNK4Foam5PBiCG5solveERNS_5FieldIdEERKS2_h+0x758) [0x7f29d72ec6a8]
[zk:12297] [ 5] /opt/openfoam222/platforms/linux64GccDPOpt/lib/libfiniteVolume.so(_ZN4Foam8fvMatrixIdE15solveSegregatedERKNS_10dictionaryE+0x137) [0x7f29d89562d7]
[zk:12297] [ 6] /opt/openfoam222/platforms/linux64GccDPOpt/lib/libincompressibleRASModels.so(_ZN4Foam8fvMatrixIdE5solveERKNS_10dictionaryE+0x152) [0x7f29d99b0f82]
[zk:12297] [ 7] /opt/openfoam222/platforms/linux64GccDPOpt/lib/libincompressibleRASModels.so(_ZN4Foam8fvMatrixIdE5solveEv+0xcc) [0x7f29d99b125c]
[zk:12297] [ 8] /opt/openfoam222/platforms/linux64GccDPOpt/lib/libincompressibleRASModels.so(_ZN4Foam14incompressible9RASModels9kOmegaSST7correctEv+0xe8c) [0x7f29d99f795c]
[zk:12297] [ 9] pimpleDyMFoam() [0x41b2bd]
[zk:12297] [10] /lib/x86_64-linux-gnu/libc.so.6(__libc_start_main+0xed) [0x7f29d61f776d]
[zk:12297] [11] pimpleDyMFoam() [0x41ed1d]
[zk:12297] *** End of error message ***
--------------------------------------------------------------------------
mpirun noticed that process rank 1 with PID 12297 on node zk exited on signal 8 (Floating point exception).
--------------------------------------------------------------------------
It seems that the timestep had become so small which led to the failure.

Thanks again for your patience!

Last edited by wyldckat; October 27, 2014 at 16:20. Reason: Changed [QUOTE][/QUOTE] to [CODE][/CODE]
kkpal is offline   Reply With Quote

Old   October 27, 2014, 17:03
Default
  #6
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 9,736
Blog Entries: 39
Rep Power: 103
wyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of light
Hi Kai,

Quote:
Originally Posted by kkpal View Post
Code:
Courant Number mean: 0.0004682635789 max: 0.2862657354
deltaT = 3.052758308e-68
--> FOAM Warning : 
    From function Time::operator++()
    in file db/Time/Time.C at line 1039
    Increased the timePrecision from 100385 to 100386 to distinguish between timeNames at time 0.1214197262
Time = 0.12141972624829507065857825409693759866058826446533203125
I've taken another look at the run I had tested... I had stopped it much earlier before any crash was able to occur, but the same symptom is still present: on my run, I had stopped when the "deltaT" was still in the scale of "1e-16" and I didn't notice it, since I was waiting for a crash to occur. If you had presented this output and version information in the very first post, I could have already tried a few versions of OpenFOAM, to see if this occurs with all of them or not .

I'll try to run this tutorial with OpenFOAM 2.2.x, 2.3.0 and 2.3.x. I'll report back as soon as I have some results.


edit: OK, it works fine with 2.2.x, 2.3.0 and 2.3.x. From what I can figure out, the commit that was introduced in 2.2.x that solves this issue is this one: https://github.com/OpenFOAM/OpenFOAM...fa30afd7c694c0

Best regards,
Bruno

Last edited by wyldckat; October 27, 2014 at 18:30. Reason: see "edit:"
wyldckat is offline   Reply With Quote

Old   November 13, 2016, 11:22
Default Boundary conditions!
  #7
New Member
 
Vickky
Join Date: Aug 2016
Posts: 5
Rep Power: 2
Vignesh2508 is on a distinguished road
I am somewhat new to openfoam. And I am trying to simulate the flow around an airfoil for my assignment. I was using the wingmotion2D test case as a base for my problem. But I found some difficulties with giving my boundary conditions and giving the reference area value for the airfoil.

1. I am using a NACA4413 with a chord length of 1m. The computational domain i chose has a thickness of 0.2m. Now my confusion is what should be the reference area for the problem in controldict, is it chord length x thickness i.e 1x0.2=0.2sq.m?

2. The turbulence model of the test case is k-omega SST. Here how should one choose the characteristic length? I chose a characteristic length of 0.1m. Is it right? If not how should one choose it?

If you were able to solve it, I want to know how you gave your boundary conditions and the reference area in controldict. Please help me out.

Thank you

Viki
Vignesh2508 is offline   Reply With Quote

Old   November 14, 2016, 02:44
Default
  #8
Member
 
benoit paillard
Join Date: Mar 2010
Posts: 56
Rep Power: 8
bennn is on a distinguished road
Hi Viki,

First of all you might want to read the guide to posting, which states Do not post replies to old threads asking your own question. Start your own new thread instead. Hi-jacking other peoples threads is against the Forum Rules and irritates everyone.

Regarding your questions :

1. I am using a NACA4413 with a chord length of 1m. The computational domain i chose has a thickness of 0.2m. Now my confusion is what should be the reference area for the problem in controldict, is it chord length x thickness i.e 1x0.2=0.2sq.m?

OpenFOAM does take the domain width into account, unlike other codes. However my advice is to not use force coefficients in controlDict, but simply compute the force and work out the coefficients yourself.

2. The turbulence model of the test case is k-omega SST. Here how should one choose the characteristic length? I chose a characteristic length of 0.1m. Is it right? If not how should one choose it?

This is a debatable topic, strongly related to the condition you're after. Wind tunnel or real world ? What kind of tunnel ? etc... 0.1m does not sound silly to me generally speaking.
bennn 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
wingMotion Tutorial dancfd OpenFOAM Native Meshers: snappyHexMesh and Others 3 November 13, 2016 11:12
Tutorial for subcooled nucleate boiling Asghari FLUENT 37 October 17, 2016 10:56
Problem on Fluent Tutorial: Horizontal Film Boilig Feng FLUENT 2 April 13, 2013 05:34
[Virtualization] OpenFOAM oriented tutorial on using VMware Player - support thread wyldckat OpenFOAM Installation 2 July 11, 2012 16:01
k-omega in wingmotion tutorial jlinterm OpenFOAM 1 December 29, 2010 16:34


All times are GMT -4. The time now is 12:59.