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

Free Surface Ship Flow

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

Like Tree18Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   October 6, 2010, 11:54
Default results at the same Fr numbers
  #81
Senior Member
 
Emanuele
Join Date: Mar 2009
Posts: 110
Rep Power: 9
nuovodna is on a distinguished road
Ok... i made some test with same Fr.

C drag for computed hull was calculate imposing S= L*D = 1* 0.0675 = 0.0675 because forces are defined on an half hull
C drag fro exp hull : S=L*D*2=3*0.1875*2= 1.125

C drag values (pressure + viscous)

Fr = 0.1 ---------------------
OF : 10.3 * 10{-3} (force intensity on half hull : 0.0316 N [0.004 viscous + 0.0312 pressure])

Fr = 0.2 ---------------------
Experimental : 5.16479 * 10^{-3} (force intensity on entire hull : 3.42 N)
OF : 9.35 * 10{-3} (force intensity on half hull : 0.114 N [0.014 viscous + 0.1 pressure])

Fr = 0.3 ---------------------
Experimental : 6.69175 * 10^{-3} (force intensity on entire hull : 9.97 N)
OF : 8.77 * 10{-3} (force intensity on half hull : 0.242 N [0.064 viscous + 0.178 pressure])

Fr = 0.316 ---------------------
OF : 9.08 * 10{-3} (force intensity on half hull : 0.278 N [0.081 viscous + 0.197 pressure])


This is my Fr = 0.3 case

http://db.tt/uMEn7OB

Png attached shows the total force values in function of time
Attached Images
File Type: png totalForce_4_Fr.png (6.0 KB, 99 views)

Last edited by nuovodna; October 6, 2010 at 12:30.
nuovodna is offline   Reply With Quote

Old   October 8, 2010, 03:40
Default
  #82
Senior Member
 
Join Date: Aug 2010
Location: Groningen, The Netherlands
Posts: 216
Rep Power: 10
colinB is on a distinguished road
Hey there,

after some weeks (o0) of experimenting I finally got a system running like the wigley case with my own test cases.
Basically not the solving part took so long, but the preparation of the hull and getting to know sHM.
Currently I have two running hull forms and on these I'm performing further tests.
One of them you might know as the kishinev hull form provided on the salome-platform.

My active question I'm struggling with is now how to visualize the pressure and velocity distribution on the hull patch.
I'm not sure if this is possible with the present setting of the p_rgh and U file
(patch for the hull-form U = fixedValue uniform (0 0 0) p_rgh = buoyantPressure uniform 0 )

Can somebody give me a hint how I can visualize this and/or what kind of changes I have to do in the relevant files.

thanks for your trouble
kind regards
Colin

PS: Is somebody of you attending the NuTTS in Duisburg starting on Sunday ?
I know that it is not limited to OF but would probably be nice to have some discussion
about OF in the break.

Edit:

forget about what I posted here, I figured out that there are still too many failures in the case
andthat there got some files lost when when compressing the case folder.

Last edited by colinB; November 5, 2010 at 06:04.
colinB is offline   Reply With Quote

Old   January 23, 2011, 03:26
Default
  #83
New Member
 
Ippokratis
Join Date: Nov 2010
Location: Athens, Greece
Posts: 13
Rep Power: 7
chripp is on a distinguished road
Hi everyone, i'm new to OF and i have finished some runs using Colin's case. From what i can see in paraview everything seems nice except the waves reflection i have in my domain. Is there any way i can fix this? I would also like to know how exactly do we calculate the drag force.
Thanks
chripp is offline   Reply With Quote

Old   February 11, 2011, 08:55
Default
  #84
New Member
 
edoardo
Join Date: Nov 2010
Posts: 8
Rep Power: 7
albertofast is on a distinguished road
Hello,
after reading extensively this post I decided to have my chance with the free surface evaluation for the wigley hull case.
I have studied 2 different models (using for both OF 1.7.1) at Fr=0.35:
a) Wigley hull model from Eric Paterson (mesh is exactly the same, while something, like variables names, changed to port it under OF 1.7.1);
b) Wigley hull model 'hand-made' importing point-coordinates in CAD and the featuring the hull surface, this model has the same parameters as Eric Paterson's wigley but it's scaled to a LWL of 10 meters (instead of 1 meter); the mesh has been made with snappyHexMesh, and resulted in about 1.5 millions of volume-elements. In this case the domain dimensions are: Length*Width*Height = 4LWL*1.5LWL*1LWL . The hull bow is placed at 1LWL downstream the inlet.

Being interested in a comparison between the results of these two models (at same Froude number but different Reynolds number
because of the different LWL) I let them run for 30 seconds of simulation (with the adjustable time-step option activated).

At the end of the simulation (after a long time!) I noticed that after about 10 to 15 seconds of simulation in each case I can find the generation
of a pattern of waves in front of the hull, whose transverse extension interests the whole domain. The nodes of the wave pattern seem to be always
in the same position whereas their amplitude varies with time. The transverse wave pattern has some differences in the examined cases:
In CASE B the amplitude of waves is smaller compared with CASE A, they also seem to appear after a longer time in respect to CASE A.
CASE B has a bigger length dimension of the domain (CASE B: 2*LWL downstream the hull stern, CASE A: 1*LWL downstream the hull stern).

What do you think about the origin of the transverse wave pattern upstream the bow? Is it something physically reasonable, like a wave reflection, or it is numerical instability so the more I let the simulation run , the more the amplitude of these waves grows?

Did you experienced something like this in your cases?

Note that after 5-10 seconds of simulation, my solution is very close to that from literature (at Fr=0.348) and that, after all,
my goal is to compute the wave resistance.

I've attached some pictures of the two cases.

One more question:
I would like to evaluate the wave drag component: do you use the Michell's integral or what else?

Thank you very much, Edoardo

Download my images from this link:
http://dl.dropbox.com/u/14793999/wigley_hull_images.zip
albertofast is offline   Reply With Quote

Old   March 11, 2011, 08:43
Default
  #85
New Member
 
Join Date: Feb 2011
Posts: 8
Rep Power: 7
kolloff is on a distinguished road
Dear albertofast,

I am running through the same kind of wigley case. I am just in the beginning of learning OF.

Could you please give me a hint on how to view the wave elevation. (Similar to the pictures you have posted.) So fare I can only view velocity and pressure.

Thank you very much in anticipation.
kolloff is offline   Reply With Quote

Old   March 24, 2011, 19:41
Default Wigley with Turbulence
  #86
New Member
 
Join Date: Jan 2010
Posts: 11
Rep Power: 8
cutty4sark is on a distinguished road
Hello,

As with many of the previous posts in this thread, I am new to OF. I have been running Patterson's version of the Wigley hull. Everything has been working well until I try and simulate turbulence and use rasInterFoam. Does anybody have any hints to get turbulence running with this simulation. I have been predominately using OF 1.5 but also have 1.6 loaded.

Also, does anybody know of any University on the west coast of the U.S., particularly CA that is using OF?

Thank you all for your time and consideration.
cutty4sark is offline   Reply With Quote

Old   March 25, 2011, 04:00
Default
  #87
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 kolloff View Post
Dear albertofast,

I am running through the same kind of wigley case. I am just in the beginning of learning OF.

Could you please give me a hint on how to view the wave elevation. (Similar to the pictures you have posted.) So fare I can only view velocity and pressure.

Thank you very much in anticipation.
I'm not running Linux now but under filters you can find the button "contour". Select from your data alpha (which indicates of cells contain water (1) or air (0), select your internal domain and choose the contour-filter. From the dropdown menu in contour choose alpha. then you have to delete the provided level for the contour and add a new level of 0.5 (intersection between water and air).

Let me know if there's a problem.

Cheers,

Ralph
__________________
CFD for marine applications? Go to http://www.marinecfd.com/ and join the OF Ship Hydromechanics Group: http://www.cfd-online.com/Forums/gro...mechanics.html
Ralph M is offline   Reply With Quote

Old   April 5, 2011, 12:32
Default
  #88
New Member
 
Jianxi Yao
Join Date: Apr 2011
Posts: 15
Rep Power: 7
jianxiyao is on a distinguished road
Quote:
Originally Posted by albertofast View Post
Hello,
after reading extensively this post I decided to have my chance with the free surface evaluation for the wigley hull case.
I have studied 2 different models (using for both OF 1.7.1) at Fr=0.35:
a) Wigley hull model from Eric Paterson (mesh is exactly the same, while something, like variables names, changed to port it under OF 1.7.1);
b) Wigley hull model 'hand-made' importing point-coordinates in CAD and the featuring the hull surface, this model has the same parameters as Eric Paterson's wigley but it's scaled to a LWL of 10 meters (instead of 1 meter); the mesh has been made with snappyHexMesh, and resulted in about 1.5 millions of volume-elements. In this case the domain dimensions are: Length*Width*Height = 4LWL*1.5LWL*1LWL . The hull bow is placed at 1LWL downstream the inlet.

Being interested in a comparison between the results of these two models (at same Froude number but different Reynolds number
because of the different LWL) I let them run for 30 seconds of simulation (with the adjustable time-step option activated).

At the end of the simulation (after a long time!) I noticed that after about 10 to 15 seconds of simulation in each case I can find the generation
of a pattern of waves in front of the hull, whose transverse extension interests the whole domain. The nodes of the wave pattern seem to be always
in the same position whereas their amplitude varies with time. The transverse wave pattern has some differences in the examined cases:
In CASE B the amplitude of waves is smaller compared with CASE A, they also seem to appear after a longer time in respect to CASE A.
CASE B has a bigger length dimension of the domain (CASE B: 2*LWL downstream the hull stern, CASE A: 1*LWL downstream the hull stern).

What do you think about the origin of the transverse wave pattern upstream the bow? Is it something physically reasonable, like a wave reflection, or it is numerical instability so the more I let the simulation run , the more the amplitude of these waves grows?

Did you experienced something like this in your cases?

Note that after 5-10 seconds of simulation, my solution is very close to that from literature (at Fr=0.348) and that, after all,
my goal is to compute the wave resistance.

I've attached some pictures of the two cases.

One more question:
I would like to evaluate the wave drag component: do you use the Michell's integral or what else?

Thank you very much, Edoardo

Download my images from this link:
http://dl.dropbox.com/u/14793999/wigley_hull_images.zip
Hi,albertofast
i have got the results data. but i do not know how to display the contor of the wave in paraview. can you tell me? thank you!
jianxiyao is offline   Reply With Quote

Old   April 6, 2011, 02:08
Default
  #89
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
Hello Jianxi Yao,

Maybe you can have a look at post #87? I checked it yesterday and it should work.

Cheers,

Ralph
__________________
CFD for marine applications? Go to http://www.marinecfd.com/ and join the OF Ship Hydromechanics Group: http://www.cfd-online.com/Forums/gro...mechanics.html
Ralph M is offline   Reply With Quote

Old   April 6, 2011, 09:58
Default
  #90
New Member
 
Jianxi Yao
Join Date: Apr 2011
Posts: 15
Rep Power: 7
jianxiyao is on a distinguished road
Quote:
Originally Posted by jianxiyao View Post
Hi,albertofast
i have got the results data. but i do not know how to display the contor of the wave in paraview. can you tell me? thank you!
Hi Ralph,
can you give me more details about how to get the same pictures at post #84? following the post #87 i just get a isosurfaces.
jianxiyao is offline   Reply With Quote

Old   April 6, 2011, 15:58
Default
  #91
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
Well, after you've followed the points as described in #84 (thus creating an isosurface for alpha1=0.5) you go again to the filter-menu and choose "calculator". You can give the output a name or leave it as sugested (I think its called Results). On the left botoom corner there's a drop down menu where you can select scalars/z-coords. This allowes you to create colours in your plot and to get the same pictures as Alberto had.

Good luck!
__________________
CFD for marine applications? Go to http://www.marinecfd.com/ and join the OF Ship Hydromechanics Group: http://www.cfd-online.com/Forums/gro...mechanics.html
Ralph M is offline   Reply With Quote

Old   April 7, 2011, 11:07
Default
  #92
New Member
 
Ippokratis
Join Date: Nov 2010
Location: Athens, Greece
Posts: 13
Rep Power: 7
chripp is on a distinguished road
Hi everyone.
I'm trying to use the wigley case with some other ship. I've managed to make a new blockMeshDict, snappyHexMeshDict and setFields file to import the new geometry and everything seems fine when i start the interFoam, i even get some right force results. I'm having troubles though: first of all the timestep is really small, after 2 days of running in an 8 core pc, i'm stil at 0.15secs. the resuls started to mess up some time and i got this error:
ippex_foam@Fine04:~/FoamJob/case001$ [2] [0] #0 [7] #0 Foam::error:rintStack(Foam::Ostream&)Foam::error :rintStack(Foam::Ostream&)[5] #0 Foam::error:rintStack(Foam::Ostream&)#0[6] # [4] 0 #0 Foam::error:rintStack(Foam::Ostream&)Foam::error :rintStack(Foam::Ostream&)[3] #0 Foam::error:rintStack(Foam::Ostream&)[1] #0 Foam::error:rintStack(Foam::Ostream&)Foam::error :rintStack(Foam::Ostream&) in "/opt/openfoam171/lib/linux64GccDPOpt/libOpenFOAM.so"
[3] #1 Foam::sigFpe::sigFpeHandler(int) in "/opt/openfoam171/lib/linux64GccDPOpt/libOpenFOAM.so"
[1] #1 Foam::sigFpe::sigFpeHandler(int) in "/opt/openfoam171/lib/linux64GccDPOpt/libOpenFOAM.so"
[7] #1 Foam::sigFpe::sigFpeHandler(int) in "/opt/openfoam171/lib/linux64GccDPOpt/libOpenFOAM.so"
[4] #1 Foam::sigFpe::sigFpeHandler(int) in "/opt/openfoam171/lib/linux64GccDPOpt/libOpenFOAM.so"
[2] #1 Foam::sigFpe::sigFpeHandler(int) in "/opt/openfoam171/lib/linux64GccDPOpt/libOpenFOAM.so"
[5] #1 Foam::sigFpe::sigFpeHandler(int) in "/opt/openfoam171/lib/linux64GccDPOpt/libOpenFOAM.so"
[6] #1 Foam::sigFpe::sigFpeHandler(int) in "/opt/openfoam171/lib/linux64GccDPOpt/libOpenFOAM.so"
[0] #1 Foam::sigFpe::sigFpeHandler(int) in "/opt/openfoam171/lib/linux64GccDPOpt/libOpenFOAM.so"
[2] #2 in "/opt/openfoam171/lib/linux64GccDPOpt/libOpenFOAM.so"
[5] #2 in "/opt/openfoam171/lib/linux64GccDPOpt/libOpenFOAM.so"
[7] #2 in "/opt/openfoam171/lib/linux64GccDPOpt/libOpenFOAM.so"
[3] #2 in "/opt/openfoam171/lib/linux64GccDPOpt/libOpenFOAM.so"
[4] #2 in "/opt/openfoam171/lib/linux64GccDPOpt/libOpenFOAM.so"
[6] #2 in "/opt/openfoam171/lib/linux64GccDPOpt/libOpenFOAM.so"
in "/opt/openfoam171/lib/linux64GccDPOpt/libOpenFOAM.so"
[1] #[0] #2 2 in "/lib/libc.so.6"
in "/lib/libc.so.6"
in "/lib/libc.so.6"
[3] #3 [2] #3 [5] #3 Foam::Time::adjustDeltaT()Foam::Time::adjustDeltaT ()Foam::Time::adjustDeltaT() in "/lib/libc.so.6"
[6] #3 Foam::Time::adjustDeltaT() in "/lib/libc.so.6"
[7] #3 Foam::Time::adjustDeltaT() in "/lib/libc.so.6"
[1] #3 Foam::Time::adjustDeltaT() in "/opt/openfoam171/lib/linux64GccDPOpt/libOpenFOAM.so"
[3] #4 in "/lib/libc.so.6"
[0] #3 Foam::Time::adjustDeltaT() in "/opt/openfoam171/lib/linux64GccDPOpt/libOpenFOAM.so"
[2] #4 in "/lib/libc.so.6"
[4] #3 Foam::Time::adjustDeltaT() in "/opt/openfoam171/lib/linux64GccDPOpt/libOpenFOAM.so"
[6] #4 in "/opt/openfoam171/lib/linux64GccDPOpt/libOpenFOAM.so"
[5] #4 in "/opt/openfoam171/lib/linux64GccDPOpt/libOpenFOAM.so"
[7] #4

in "/opt/openfoam171/lib/linux64GccDPOpt/libOpenFOAM.so"
[4] #4 in "/opt/openfoam171/lib/linux64GccDPOpt/libOpenFOAM.so"
[1] #4 in "/opt/openfoam171/lib/linux64GccDPOpt/libOpenFOAM.so"
[0] #4



[2] in "/opt/openfoam171/applications/bin/linux64GccDPOpt/interFoam"
[2] #5 __libc_start_main[3] in "/opt/openfoam171/applications/bin/linux64GccDPOpt/interFoam"
[3] #5 __libc_start_main
in "/lib/libc.so.6"
[2] #6
[5] in "/opt/openfoam171/applications/bin/linux64GccDPOpt/interFoam"
[5] #5 __libc_start_main[4] in "/opt/openfoam171/applications/bin/linux64GccDPOpt/interFoam"
[4] #5 __libc_start_main in "/lib/libc.so.6"
[3] #6 [7] in "/opt/openfoam171/applications/bin/linux64GccDPOpt/interFoam"
[7] #5 __libc_start_main[6] in "/opt/openfoam171/applications/bin/linux64GccDPOpt/interFoam"
[6] #5 __libc_start_main
in "/lib/libc.so.6"
[5] #6 [0] in "/opt/openfoam171/applications/bin/linux64GccDPOpt/interFoam"
[0] #5 __libc_start_main[1] in "/opt/openfoam171/applications/bin/linux64GccDPOpt/interFoam"
[1] #5 __libc_start_main
in "/lib/libc.so.6"
[4] #6
in "/lib/libc.so.6"
[6] #6 in "/lib/libc.so.6"
[0] #6 in "/lib/libc.so.6"
[1] #6 in "/lib/libc.so.6"
[7] #6
[2] in "/opt/openfoam171/applications/bin/linux64GccDPOpt/interFoam"
[Fine04:06300] *** Process received signal ***
[Fine04:06300] Signal: Floating point exception (8)
[Fine04:06300] Signal code: (-6)
[Fine04:06300] Failing at address: 0x3e90000189c
[Fine04:06300] [ 0] /lib/libc.so.6(+0x33c20) [0x7f70ee8a1c20]
[Fine04:06300] [ 1] /lib/libc.so.6(gsignal+0x35) [0x7f70ee8a1ba5]
[Fine04:06300] [ 2] /lib/libc.so.6(+0x33c20) [0x7f70ee8a1c20]
[Fine04:06300] [ 3] /opt/openfoam171/lib/linux64GccDPOpt/libOpenFOAM.so(_ZN4Foam4Time12adjustDeltaTEv+0x5d) [0x7f70ef70ee0d]
[Fine04:06300] [ 4] interFoam() [0x4222a5]
[Fine04:06300] [ 5] /lib/libc.so.6(__libc_start_main+0xfe) [0x7f70ee88cd8e]
[Fine04:06300] [ 6] interFoam() [0x41d319]
[Fine04:06300] *** End of error message ***
[5] in "/opt/openfoam171/applications/bin/linux64GccDPOpt/interFoam"
[Fine04:06303] *** Process received signal ***
[Fine04:06303] Signal: Floating point exception (8)
[Fine04:06303] Signal code: (-6)
[Fine04:06303] Failing at address: 0x3e90000189f
[Fine04:06303] [ 0] /lib/libc.so.6(+0x33c20) [0x7fa09d3e6c20]
[Fine04:06303] [ 1] /lib/libc.so.6(gsignal+0x35) [0x7fa09d3e6ba5]
[Fine04:06303] [ 2] /lib/libc.so.6(+0x33c20) [0x7fa09d3e6c20]
[Fine04:06303] [ 3] /opt/openfoam171/lib/linux64GccDPOpt/libOpenFOAM.so(_ZN4Foam4Time12adjustDeltaTEv+0x5d) [0x7fa09e253e0d]
[Fine04:06303] [ 4] interFoam() [0x4222a5]
[Fine04:06303] [ 5] /lib/libc.so.6(__libc_start_main+0xfe) [0x7fa09d3d1d8e]
[Fine04:06303] [ 6] interFoam() [0x41d319]
[Fine04:06303] *** End of error message ***


[3] in "/opt/openfoam171/applications/bin/linux64GccDPOpt/interFoam"
[Fine04:06301] *** Process received signal ***
[Fine04:06301] Signal: Floating point exception (8)
[Fine04:06301] Signal code: (-6)
[Fine04:06301] Failing at address: 0x3e90000189d
[Fine04:06301] [ 0] /lib/libc.so.6(+0x33c20) [0x7f7d76bd3c20]
[Fine04:06301] [ 1] /lib/libc.so.6(gsignal+0x35) [0x7f7d76bd3ba5]
[Fine04:06301] [ 2] /lib/libc.so.6(+0x33c20) [0x7f7d76bd3c20]
[Fine04:06301] [ 3] /opt/openfoam171/lib/linux64GccDPOpt/libOpenFOAM.so(_ZN4Foam4Time12adjustDeltaTEv+0x5d) [0x7f7d77a40e0d]
[Fine04:06301] [ 4] interFoam() [0x4222a5]
[Fine04:06301] [ 5] /lib/libc.so.6(__libc_start_main+0xfe) [0x7f7d76bbed8e]
[Fine04:06301] [ 6] interFoam() [0x41d319]
[Fine04:06301] *** End of error message ***


[0] in "/opt/openfoam171/applications/bin/linux64GccDPOpt/interFoam"
[Fine04:06298] *** Process received signal ***
[Fine04:06298] Signal: Floating point exception (8)
[Fine04:06298] Signal code: (-6)
[Fine04:06298] Failing at address: 0x3e90000189a
[1] in "/opt/openfoam171/applications/bin/linux64GccDPOpt/interFoam"
[Fine04:06298] [ 0] /lib/libc.so.6(+0x33c20) [0x7f7232432c20]
[Fine04:06298] [ 1] /lib/libc.so.6(gsignal+0x35) [0x7f7232432ba5]
[Fine04:06298] [ 2] /lib/libc.so.6(+0x33c20) [0x7f7232432c20]
[Fine04:06298] [ 3] /opt/openfoam171/lib/linux64GccDPOpt/libOpenFOAM.so(_ZN4Foam4Time12adjustDeltaTEv+0x5d) [0x7f723329fe0d]
[Fine04:06298] [ 4] interFoam() [0x4222a5]
[Fine04:06298] [ 5] /lib/libc.so.6(__libc_start_main+0xfe) [0x7f723241dd8e]
[Fine04:06298] [ 6] interFoam() [0x41d319]
[Fine04:06298] *** End of error message ***
[Fine04:06299] *** Process received signal ***
[Fine04:06299] Signal: Floating point exception (8)
[Fine04:06299] Signal code: (-6)
[Fine04:06299] Failing at address: 0x3e90000189b
[Fine04:06299] [ 0] /lib/libc.so.6(+0x33c20) [0x7f2bd0b78c20]
[Fine04:06299] [ 1] /lib/libc.so.6(gsignal+0x35) [0x7f2bd0b78ba5]
[Fine04:06299] [ 2] /lib/libc.so.6(+0x33c20) [0x7f2bd0b78c20]
[Fine04:06299] [ 3] /opt/openfoam171/lib/linux64GccDPOpt/libOpenFOAM.so(_ZN4Foam4Time12adjustDeltaTEv+0x5d) [0x7f2bd19e5e0d]
[Fine04:06299] [ 4] interFoam() [0x4222a5]
[Fine04:06299] [ 5] /lib/libc.so.6(__libc_start_main+0xfe) [0x7f2bd0b63d8e]
[Fine04:06299] [ 6] interFoam() [0x41d319]
[Fine04:06299] *** End of error message ***
[6] in "/opt/openfoam171/applications/bin/linux64GccDPOpt/interFoam"
[Fine04:06304] *** Process received signal ***
[Fine04:06304] Signal: Floating point exception (8)
[Fine04:06304] Signal code: (-6)
[Fine04:06304] Failing at address: 0x3e9000018a0
[Fine04:06304] [ 0] /lib/libc.so.6(+0x33c20) [0x7fa812007c20]
[Fine04:06304] [ 1] /lib/libc.so.6(gsignal+0x35) [0x7fa812007ba5]
[Fine04:06304] [ 2] /lib/libc.so.6(+0x33c20) [0x7fa812007c20]
[Fine04:06304] [ 3] /opt/openfoam171/lib/linux64GccDPOpt/libOpenFOAM.so(_ZN4Foam4Time12adjustDeltaTEv+0x5d) [0x7fa812e74e0d]
[Fine04:06304] [ 4] interFoam() [0x4222a5]
[Fine04:06304] [ 5] /lib/libc.so.6(__libc_start_main+0xfe) [0x7fa811ff2d8e]
[Fine04:06304] [ 6] interFoam() [0x41d319]
[Fine04:06304] *** End of error message ***
[7] in "/opt/openfoam171/applications/bin/linux64GccDPOpt/interFoam"
[Fine04:06305] *** Process received signal ***
[Fine04:06305] Signal: Floating point exception (8)
[Fine04:06305] Signal code: (-6)
[Fine04:06305] Failing at address: 0x3e9000018a1
[Fine04:06305] [ 0] /lib/libc.so.6(+0x33c20) [0x7fde01c7ec20]
[Fine04:06305] [ 1] /lib/libc.so.6(gsignal+0x35) [0x7fde01c7eba5]
[Fine04:06305] [ 2] /lib/libc.so.6(+0x33c20) [0x7fde01c7ec20]
[Fine04:06305] [ 3] /opt/openfoam171/lib/linux64GccDPOpt/libOpenFOAM.so(_ZN4Foam4Time12adjustDeltaTEv+0x5d) [0x7fde02aebe0d]
[Fine04:06305] [ 4] interFoam() [0x4222a5]
[Fine04:06305] [ 5] /lib/libc.so.6(__libc_start_main+0xfe) [0x7fde01c69d8e]
[Fine04:06305] [ 6] interFoam() [0x41d319]
[Fine04:06305] *** End of error message ***
--------------------------------------------------------------------------
mpirun noticed that process rank 2 with PID 6300 on node Fine04 exited on signal 8 (Floating point exception).
--------------------------------------------------------------------------

Can anyone help me with this?
Thanks!
chripp is offline   Reply With Quote

Old   April 7, 2011, 11:17
Default
  #93
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
Hello Christos,

The SigFpe-code says something about a division by zero (not sure; search this forum to check). Maybe your timestep was becoming too small?

The reason for interFoam to take such a small timestep is probably because of the Courantnumber limitation that you've implemented in the controlDict. This high number is caused by the pressure differences; that's why some people tried/are trying to get shipFoam running. This solver relaxes the pressure and should therefore be more stable. However, I'm trying to adopt this solver for OF 1.7.1 but there are still some bugs in there so far....

Well, good luck!

Ralph
__________________
CFD for marine applications? Go to http://www.marinecfd.com/ and join the OF Ship Hydromechanics Group: http://www.cfd-online.com/Forums/gro...mechanics.html
Ralph M is offline   Reply With Quote

Old   April 7, 2011, 11:42
Default
  #94
New Member
 
Ippokratis
Join Date: Nov 2010
Location: Athens, Greece
Posts: 13
Rep Power: 7
chripp is on a distinguished road
Hello Ralph and thanks for the quick reply.
Here's what i have on the controlDict:

FoamFile
{
version 2.0;
format ascii;

root "/home/egp11";
case "wigley";
instance "system";
local "";

class dictionary;
object controlDict;
}

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

application interFoam;

startFrom startTime;

startTime 0;

stopAt endTime;

endTime 60;

deltaT 0.001;

writeControl adjustableRunTime;

writeInterval 15;

purgeWrite 0;

writeFormat ascii;

writePrecision 6;

writeCompression uncompressed;

timeFormat general;

timePrecision 6;

graphFormat raw;

runTimeModifiable yes;

adjustTimeStep on;

maxCo 0.8;
maxAlphaCo 0.8;
maxDeltaT 1;


// ************************************************** *********************** //

functions
(
forces
{
type forces;
functionObjectLibs ("libforces.so"); //Lib to load
outputControl timeStep;
outputInterval 1;
patches (wall_patch0); // change to your patch name
rhoInf 1000; //Reference density for fluid
nuInf 1e-6; //Reference kinetic viscosity for fluid
CofR (0 0 0); //Origin for moment calculations
}

forceCoeffs
{
type forceCoeffs;
functionObjectLibs ("libforces.so");
outputControl timeStep;
outputInterval 1;
patches (wall_patch0); //change to your patch name
rhoInf 1000;
nuInf 1e-6;
CofR (0 0 0);
liftDir (0 0 1);
dragDir (-1 0 0);
pitchAxis (0 1 0);
magUInf 0.45;
lRef 1;
Aref 1;
}
);


Do you think i should change something there or somewhere else?
My timestep is becoming very small like i said in the previous post. What can i do to fix it?
So from what i can understrand the shipFoam is not ready to use right?
chripp is offline   Reply With Quote

Old   April 8, 2011, 02:33
Default
  #95
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
Good morning Christos,

Your timestep is being influenced by:

adjustTimeStep on;

maxCo 0.8;

The latter puts a maximum to your Courant number by changing the timestep. Setting "adjustTimeStep off" will result in a fixed timestep but I bet sooner or later your code will explode.

ShipFoam for OF 171 is not ready, but you can still use it within OF1.6 (it's written for 1.6). Although it's simply changing the pressure into the correct terms (p from 1.6 into p and p_rgh for 1.7) I didn't succeed in this task. Next days I'm going to install OF1.6 and see how it runs.

Regards,

Ralph
__________________
CFD for marine applications? Go to http://www.marinecfd.com/ and join the OF Ship Hydromechanics Group: http://www.cfd-online.com/Forums/gro...mechanics.html
Ralph M is offline   Reply With Quote

Old   April 8, 2011, 09:03
Default
  #96
New Member
 
Ippokratis
Join Date: Nov 2010
Location: Athens, Greece
Posts: 13
Rep Power: 7
chripp is on a distinguished road
Hello again Ralph,

I made some changes to my controlDict according to the shipFoam controlDict available in the Hydromechanics group.

The modifications i've made are:

startFrom latestTime
deltaT 0.01
writeInterval 0.1
maxCo 0.5
maxAlphaCo 0.5
maxDeltaT 0.01

It only runs for some hours now, but it's much faster than before. Also the force results so far are very satisfying. I hope it won't explode later though....!

Best regards
Ippokratis
chripp is offline   Reply With Quote

Old   April 10, 2011, 11:26
Default
  #97
New Member
 
Ippokratis
Join Date: Nov 2010
Location: Athens, Greece
Posts: 13
Rep Power: 7
chripp is on a distinguished road
Hello everyone,

I'm still having the same issues. Any more suggestions?

Regards
chripp is offline   Reply With Quote

Old   April 13, 2011, 14:14
Default
  #98
Senior Member
 
Pablo
Join Date: Mar 2009
Posts: 102
Rep Power: 9
pablodecastillo is on a distinguished road
How is your mesh quality?

Did you try to run in laminar first?
pablodecastillo is offline   Reply With Quote

Old   April 13, 2011, 16:07
Default
  #99
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 pablodecastillo View Post
How is your mesh quality?

Did you try to run in laminar first?
I think (actually quite sure) that this suggestion doesn't solve our problems. It can be read on this forum that problems in solvers most of have to be found in the source code or the model.

Cheers,

Ralph
__________________
CFD for marine applications? Go to http://www.marinecfd.com/ and join the OF Ship Hydromechanics Group: http://www.cfd-online.com/Forums/gro...mechanics.html
Ralph M is offline   Reply With Quote

Old   April 13, 2011, 16:24
Default
  #100
ngj
Senior Member
 
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Deltares, Delft, The Netherlands
Posts: 1,688
Rep Power: 27
ngj will become famous soon enoughngj will become famous soon enough
Hi

When I have been running VOF-methods, my experience is that you should have a Courant number of approximately 0.25 to keep out of problems. Much larger than that might be the reason the for problems you are seeing.

Furthermore, I have experience that using a large number of nAlphaSubCycles can result in solutions that are unstable. Setting this value to 1 typically solves that instability. Furthermore, I put nAlphaCorr to 1 as well.

On top of that I have experienced that poor mesh quality around the surface can induce rather large erroneous velocities in the air, hence it might be worthwhile to check the mesh quality as already suggested.

Good luck

Niels
Ellie likes this.
ngj 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
Free-Surface Ship Flow - Boundary Conditions James Date CFX 1 February 19, 2013 06:42
ship free-surface analysis Andrea Mercuri CD-adapco 0 September 28, 2004 11:01
Free Surface Flow for Ship sam FLUENT 6 October 24, 2003 05:29
viscous free surface flow past a ship hull lololo Main CFD Forum 0 June 12, 2002 23:02
meshing for surface ship flow boris FLUENT 0 April 24, 2002 20:27


All times are GMT -4. The time now is 08:17.