# Free Surface Ship Flow

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

October 6, 2010, 11:54
results at the same Fr numbers
#81
Senior Member

Emanuele
Join Date: Mar 2009
Posts: 110
Rep Power: 8
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
 totalForce_4_Fr.png (6.0 KB, 96 views)

Last edited by nuovodna; October 6, 2010 at 12:30.

 October 8, 2010, 03:40 #82 Senior Member   Join Date: Aug 2010 Location: Groningen, The Netherlands Posts: 216 Rep Power: 10 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.

 January 23, 2011, 03:26 #83 New Member   Ippokratis Join Date: Nov 2010 Location: Athens, Greece Posts: 13 Rep Power: 7 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

 March 11, 2011, 08:43 #85 New Member   Join Date: Feb 2011 Posts: 8 Rep Power: 6 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.

 March 24, 2011, 19:41 Wigley with Turbulence #86 New Member   Join Date: Jan 2010 Posts: 11 Rep Power: 7 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.

March 25, 2011, 04:00
#87
Senior Member

Ralph Moolenaar
Join Date: Aug 2010
Location: 's-Hertogenbosch, the Netherlands
Posts: 120
Rep Power: 7
Quote:
 Originally Posted by kolloff 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

April 5, 2011, 12:32
#88
New Member

Jianxi Yao
Join Date: Apr 2011
Posts: 15
Rep Power: 6
Quote:
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!

 April 6, 2011, 02:08 #89 Senior Member   Ralph Moolenaar Join Date: Aug 2010 Location: 's-Hertogenbosch, the Netherlands Posts: 120 Rep Power: 7 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

April 6, 2011, 09:58
#90
New Member

Jianxi Yao
Join Date: Apr 2011
Posts: 15
Rep Power: 6
Quote:
 Originally Posted by jianxiyao 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.

 April 6, 2011, 15:58 #91 Senior Member   Ralph Moolenaar Join Date: Aug 2010 Location: 's-Hertogenbosch, the Netherlands Posts: 120 Rep Power: 7 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

 April 7, 2011, 11:17 #93 Senior Member   Ralph Moolenaar Join Date: Aug 2010 Location: 's-Hertogenbosch, the Netherlands Posts: 120 Rep Power: 7 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

 April 7, 2011, 11:42 #94 New Member   Ippokratis Join Date: Nov 2010 Location: Athens, Greece Posts: 13 Rep Power: 7 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?

 April 8, 2011, 02:33 #95 Senior Member   Ralph Moolenaar Join Date: Aug 2010 Location: 's-Hertogenbosch, the Netherlands Posts: 120 Rep Power: 7 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

 April 8, 2011, 09:03 #96 New Member   Ippokratis Join Date: Nov 2010 Location: Athens, Greece Posts: 13 Rep Power: 7 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

 April 10, 2011, 11:26 #97 New Member   Ippokratis Join Date: Nov 2010 Location: Athens, Greece Posts: 13 Rep Power: 7 Hello everyone, I'm still having the same issues. Any more suggestions? Regards

 April 13, 2011, 14:14 #98 Senior Member   Pablo Join Date: Mar 2009 Posts: 102 Rep Power: 8 How is your mesh quality? Did you try to run in laminar first?

April 13, 2011, 16:07
#99
Senior Member

Ralph Moolenaar
Join Date: Aug 2010
Location: 's-Hertogenbosch, the Netherlands
Posts: 120
Rep Power: 7
Quote:
 Originally Posted by pablodecastillo 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

 April 13, 2011, 16:24 #100 Senior Member   Niels Gjoel Jacobsen Join Date: Mar 2009 Location: Deltares, Delft, The Netherlands Posts: 1,641 Rep Power: 25 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.

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post James Date CFX 1 February 19, 2013 06:42 Andrea Mercuri CD-adapco 0 September 28, 2004 11:01 sam FLUENT 6 October 24, 2003 05:29 lololo Main CFD Forum 0 June 12, 2002 23:02 boris FLUENT 0 April 24, 2002 20:27

All times are GMT -4. The time now is 10:38.