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

Segmentation Fault moving wing

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

Reply
 
LinkBack Thread Tools Display Modes
Old   May 3, 2006, 10:31
Default Hello, A set up a case conc
  #1
Senior Member
 
Frank Bos
Join Date: Mar 2009
Location: The Netherlands
Posts: 338
Rep Power: 9
lr103476 is on a distinguished road
Hello,

A set up a case concerning an o-type mesh to solve the flow around a moving wing. The following two links show this mesh:

http://www.aero.lr.tudelft.nl/~frank...wing_omesh.jpg
http://www.aero.lr.tudelft.nl/~frank...omesh_zoom.jpg

(Using firefox I cant put my pictures in the post.)

The BC of the left half of the outer boundary is 'inlet' and the right half is put to 'outlet'.

I already simulated a moving cylinder using the movingFlapFvMesh routine, which was adapted to contain harmonic motion. The o-type set-up is chosen since I also used this mesh for Fluent simulations, so I like to compare the results.

The solver I used for the moving cylinder worked perfectly, although the timesteps needed to be very very small. But in this case of the o-type mesh containing a moving wing I get a 'segmentation fault'. I already figured out that the problem occurs in the mesh.move() routine. As far as I know all other solver settings are correct, since I put them equal to my working moving cylinder case.

What are typical reasons for a segmentation error?
Are the tetrahedral cells near the outer boundary causing any troubles?

Thanks and regards,
Frank
__________________
Frank Bos
lr103476 is offline   Reply With Quote

Old   May 3, 2006, 13:40
Default Hi Frank. At first: I don't
  #2
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,915
Rep Power: 40
gschaider will become famous soon enoughgschaider will become famous soon enough
Hi Frank.

At first: I don't really know much about moving meshes, so I can't help you with your concrete problem.

@segmentation fault: this usually occurs when a program trys to access memory outside its bounds (see http://en.wikipedia.org/wiki/Segmentation_Fault). In OpenFOAM this usually occurs when a List<> or similar is accessed with an index outside of the allocated domain. To find out where this occurs make a separate copy of the OF-sources, recompile them with the swich WM_COMPILE_OPTION set to Debug (just uncomment the right lines in the bashrc/cshrc files). This makes OF run slower, but accesses to List<> etc are checked for ranges and the program aborts if you access outside of a range (plus you get a stack trace). This won't solve your problem, but it will help you find out where it occurs.

For recompiling OpenFOAM look at Martin's How-To at http://openfoamwiki.net/index.php/Howto_compile_O penFOAM

If you want stack traces with line-numbers and source-files try to apply the patch described in http://www.cfd-online.com/OpenFOAM_D...tml?1145526782
__________________
Note: I don't use "Friend"-feature on this forum out of principle. Ah. And by the way: I'm not on Facebook either. So don't be offended if I don't accept your invitation/friend request
gschaider is offline   Reply With Quote

Old   May 4, 2006, 02:19
Default All right, I did that. It took
  #3
Senior Member
 
Frank Bos
Join Date: Mar 2009
Location: The Netherlands
Posts: 338
Rep Power: 9
lr103476 is on a distinguished road
All right, I did that. It took a long time to compile OpenFOAM but it works again. Then I compiled my solver again.

Using that solver, which has moving meshes according to the movingFlapFvMesh class, the following output is generated. Before debugging the last statement was replaced with the segmentation fault.

=========================================+++
=========================================+++
Create time

Create mesh

Selecting movingFvMesh movingFlapFvMesh
Selection motion solver: laplace
Selection motion diffusion: quadratic
Performing a moving mesh calculation:
x-amplitude: 1.337 x-frequency: 0.25
y-amplitude: 0 y-frequency: 0.25
theta-amplitude: 0.5 theta-frequency: 0.25
Reading transportProperties

Reading field p

Reading field U

Reading/calculating face flux field phi

Mean and max Courant Numbers = 0 0.000152572

Starting time loop

Mean and max Courant Numbers = 0 0.305144
deltaT = 0.1
Time = 0.1



--> FOAM FATAL ERROR : index -1 out of range 0 ... 3

From function UList<t>::checkIndex(const label)
in file /home/frankl/OpenFOAM/OpenFOAM-1.2/src/OpenFOAM/lnInclude/UListI.H at line 107.

FOAM aborting

Aborted

=========================================+++
=========================================+++

So the problem has something to do with UListl.H, but what I could do with this information is not yet clear to me.

Thanks anyways, Frank
__________________
Frank Bos
lr103476 is offline   Reply With Quote

Old   May 4, 2006, 02:26
Default This looks very dubious and is
  #4
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,758
Rep Power: 21
hjasak will become famous soon enough
This looks very dubious and is probably somewhere in the moving flap class (where did you pick it up?).

Unfortunately, what is required is a trace-back of the error. For the moment, try running it in gdb and do where + post it here if you'd like comments. Ideally, I would like the debug version of trace-back (it porvides line numbers etc) but if you haven't got this ready, let's try the optimized trace-back first.

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   May 4, 2006, 06:35
Default Problem solved. I made a very
  #5
Senior Member
 
Frank Bos
Join Date: Mar 2009
Location: The Netherlands
Posts: 338
Rep Power: 9
lr103476 is on a distinguished road
Problem solved. I made a very stupid mistake. For my cylinder simulation I manipulated the kinematics in movingFvFlapMesh.C and changed the movingPatchID to the name of the cylinder wall.

movingPatchID = boundaryMesh().findPatchID("cyl_wall");

A few days ago I wanted to use the same solver for a moving wing, which name was "wing_wall".....All right, I changed the patch name and everything works OK, for now....

Btw, I found that OpenFOAM is approximately twice as fast compared to Fluent during an iteration. But OpenFOAM needs about more than twice the number of timesteps, due to the Courant restriction. Are there any plans to develop a second order fully implicit time scheme?

Frank
__________________
Frank Bos
lr103476 is offline   Reply With Quote

Old   May 4, 2006, 06:51
Default This is a second-order fully i
  #6
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,758
Rep Power: 21
hjasak will become famous soon enough
This is a second-order fully implicit scheme. If you wish to recover the time-step behaviour of Fluent, all you need to do is to set up the same discretisation (especially convection).

Additionally, Fluent uses transient SIMPLE for its transient runs by default, which is more time-step tolerant (whereas icoFoam/turbFoam uses PISO). If you wish to try it out, there's a few implementations about (Dr. Hakan Nilsson of Chalmers Uni and I played around with it a while back). However, you will also get some of the increased cost because of the different algorithm.

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak 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
Segmentation fault in map msg30 OpenFOAM Meshing Format & General Technical 6 March 27, 2008 11:49
Segmentation fault billy OpenFOAM Installation 20 April 23, 2007 22:57
segmentation fault Sheila CD-adapco 8 October 9, 2005 05:40
segmentation fault natesan CD-adapco 4 January 12, 2004 09:51
Segmentation Fault Prateep Chatterjee FLUENT 1 May 29, 2000 10:47


All times are GMT -4. The time now is 20:28.