|
[Sponsors] |
October 4, 2009, 14:49 |
|
#101 |
Senior Member
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Copenhagen, Denmark
Posts: 1,903
Rep Power: 37 |
Hi Kjetil
It looks very unphysical to my, as it should be impossible to change the direction of the flow in the bend without having a resulting force [1], hence are you sure that you are using the model correctly? Have you tried solving the problem in a single-phase configuration to see, if you get a reasonable pressure distribution?!? Otherwise I do not think I am able to help you, as I have not used either 1.6 nor compressibleInterfoam Best regards, Niels [1] i.e. a larger pressure on the outer side of the bend that on the inner side of the bend. |
|
October 4, 2009, 15:01 |
|
#102 | |
Senior Member
Join Date: Mar 2009
Location: Norway
Posts: 138
Rep Power: 17 |
Quote:
Though, are there any other two-phase compressible solvers for OpenFOAM? I have a water and air flow, but have (so far) found compressibleInterFoam to be the only one for this use ... |
||
October 4, 2009, 15:17 |
|
#103 |
Senior Member
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Copenhagen, Denmark
Posts: 1,903
Rep Power: 37 |
Hi Kjetil
I am not aware of any other solver. However, if you are can share your setup, I will try to give it a look and see, if I can spot where this un-physical pressure originates from. Bests, Niels |
|
October 4, 2009, 16:07 |
|
#104 | |
Senior Member
Join Date: Mar 2009
Location: Norway
Posts: 138
Rep Power: 17 |
Quote:
Content of 0/U: Content of 0/P: internalField uniform 0;And a snippet from transportProperties: // liqBasically, I only "know" the outlet pressure - which should be 1 atm. The inlet is not pressurized from outside, but instead the (negative) hydrostatic pressure is supposed "pull the water" from the outside reservoir. I would very much appreciate any comments on how to improve this approach. Thanks. |
||
October 4, 2009, 17:17 |
|
#105 |
Senior Member
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Copenhagen, Denmark
Posts: 1,903
Rep Power: 37 |
Hi Kjetil
I have looked at your setup, and the reason behind your strange results might be due to several things, or more likely a combination of the items below. 1. You specify a pressure at the inlet and a zero gradient at the outlet, however you do not specify the flux in any way. Hence the model is not sufficiently constrained. There are two possible solutions to this: a: Specify an outlet pressure b: Specify a uniform or varying velocity field at the inlet (use uniform to start with just to simplify things) and set the pressure at the outlet with a zeroGradient of the pressure at the inlet. 2. You specify that the minimum pressure is 0, and the pressure at the inlet is zero as well. You will not be able to drive any flow from the inlet to the outlet in that way, as pressures below zero (everywhere else than at the inlet), will be set to zero, i.e. no resulting net forcing on the fluid volume. Regarding the above, I have a couple of comments (based on a assumption that the goal is to reach a steady state condition and one single phase): ad 1a: Specifying a pressure gradient as forcing yields an asymtotic convergence, which can be shown mathematically (cannot recall the reference), hence the time to reach steady state is considerable. ad 1b: Specifying the velocity at the inlet on the other hand is similar to enforce a certain flux, thus the time it will take to achieve steady state typically shorter, i.e. the development of the boundary layer. These thought will probably be influenced by the introduction of a second phase, but my intuition tells me that the general idea is still valid. Best regards and good luck, Niels |
|
October 4, 2009, 17:41 |
|
#106 |
Senior Member
Join Date: Mar 2009
Location: Norway
Posts: 138
Rep Power: 17 |
Thank you Niels,
on 1) : if I define an outlet pressure, wouldn't that also imply a pressure difference between inlet and outlet? Because I don't think I know that pressure, I believe I only know the outlet, which is ambient - or 1 atm. I think I tried setting an outlet pressure, and having zeroGradient as inlet - but then the flow started moving from the outlet and to the inlet. |
|
October 4, 2009, 18:37 |
|
#107 |
Senior Member
Join Date: Mar 2009
Location: Norway
Posts: 138
Rep Power: 17 |
... porting the case files to use interFoam solver instead, still using single phase (water), yields excellent results! That is, pressure field looks the way it should. Even when I used a fixed inlet velocity in previous case and compressibleInterFoam, the "pMin" seems to overrule any 'p', and it fixes entire internal pressure to the 'pMin'. But then, choosing interFoam instead, the problem is solved. For single phase. Very odd. And I cannot find anything about this pMin anywhere in the userguide or here on the forum ...
|
|
October 5, 2009, 03:22 |
|
#108 |
Senior Member
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Copenhagen, Denmark
Posts: 1,903
Rep Power: 37 |
Try setting pMin to some large negative value, e.g. -1e10, and see if you can solve the problem using compressibleInterfoam.
Bests Niels |
|
October 5, 2009, 05:52 |
|
#109 |
Senior Member
Join Date: Mar 2009
Location: Norway
Posts: 138
Rep Power: 17 |
There is something fishy going on here, because the behaviour of this solver is far from predictable. Regardless any low pressure - I tried both -2.5e5 (which I believe is just below the actual minimum pressure) and -1e10 - results in a continuing fluctuating pressure field. Like this: http://folk.ntnu.no/kjetilbi/openfoam/ani1.gif . The time step between each frame is 0.02sec.
Still, this is single phase, water only, and 1m/s inlet velocity. And to me this "shouldn't" be this difficult to set up ... |
|
October 6, 2009, 16:22 |
|
#110 |
Senior Member
Join Date: Mar 2009
Location: Norway
Posts: 138
Rep Power: 17 |
I did some investigation in the solver itself, and "everything" seems fine - even the velocity field. The only exception is this pMin. And reading the source file and pEqn.H, I find this
p.max(pMin); My C-skills are not that good to determine the exact purpose of this. But it is the only place that pMin occurs - at least in the files I have been looking through... |
|
October 7, 2009, 02:48 |
|
#111 |
Senior Member
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Copenhagen, Denmark
Posts: 1,903
Rep Power: 37 |
Hi Kjetil
One thought. Could it be that the compressibility needs to have the total pressure, hence a negative pressure would suggest something being un-physical. Try setting the pressure at the boundary to 1 atm and then rerun everything. Good luck, Niels |
|
October 8, 2009, 18:24 |
|
#112 |
Senior Member
Join Date: Mar 2009
Location: Norway
Posts: 138
Rep Power: 17 |
Thanks Niels, I really appreciate your suggestions here.
Though, it seems like what pressure that is being stored, is set to the pMin, no matter what the other pressures are. Though the flow acts perfectly and the velocity field is as it is supposed to - the pressured used in the simulation must be right... it is just not stored properly. May there be a way to disable this malfunctioning pMin feature you think? At the moment I am unable to continue a paused simulation using 'latestTime' .. as the pressure in the 'p' files is stored equivalent to the pMin, which then of course is wrong ... |
|
November 6, 2009, 07:58 |
|
#113 |
Member
Piotr Prusinski
Join Date: Oct 2009
Location: Warsaw, Poland
Posts: 67
Rep Power: 17 |
Could any one of you explain me shortly what is the meaning or difference between rho and rho0 in the transportProperties?
|
|
November 20, 2009, 05:02 |
|
#114 |
Member
Maruthamuthu Venkatraman
Join Date: Mar 2009
Location: Norway
Posts: 80
Rep Power: 17 |
Hello Marc,
Iam interested in studying the pressure field of a cylinder in crossflow which moves due to hydrodynamic forces after resolving Dynamic equations of Motion. The wall has to be moved once displacement is calculated for each time step. I found that you have some relevant experience in this job. SInce iam interested in deep SUbsea pipelines, i dont want to account the free surface effects on the calculation. Could you tell me how to proceed with. Actually i downloaded your code and try to compile them with ' wmake libso ' command and then run the demos. It says shipFoam : Command not found. Could you give me clear instructions How to run your demo Cases and compiling your code. Thanks |
|
November 20, 2009, 10:45 |
|
#115 |
Senior Member
Mark Couwenberg
Join Date: Mar 2009
Location: Netherlands
Posts: 130
Rep Power: 17 |
Hello Maruthamuthu,
To build the solver you should use wmake without libso. It is not a library. And the solver which is posted here only build under OF 1.5. I am working to adapt it for OF 1.6 as well and I intend to post it on the svn network instead of here on the forum. Anyway, you can use the pieces of code to build your own solver from 1-phase cases. It shall be transient solutions so you may want to use pisoFoam as starting point (not icoFoam because this does not have turbulence ability, which you probably want at some stage). You need to modify this code in three stages I think: 1. add hydrostatic pressure and gravity 2. add moving mesh posibilty 3. add the pieces of code from shipFoam. Basically I used interDyMFoam as starting point. So, some work to do! If you succeed, I am interested in the solver as well. Succes, Mark |
|
February 21, 2010, 16:17 |
running shipFoam1.6.2 in OpenFOAM-1.6.x
|
#116 |
New Member
John.B
Join Date: Mar 2009
Posts: 14
Rep Power: 17 |
Hello Mark and others,
I just complied shipFoam on my Mac OS X, running OpenFOAM 1.6.x By downloading the shipFoam solver from the svn network (available under Breeder_1.6). I have to add “-I$(LIB_SRC)/turbulenceModels/incompressible/turbulenceModel \” under EXE_INC in the options file in the Make folder, since this source was missing. When going throw the tutorials one also has to add “alpha1” (or alpha1.org~, used when running Allrun) in the 0 folder since this was also missing. I tested all three tutorials “drop”, “jar” and “roll” and all worked perfectly. Has someone tried shipFoam on other test cases? Or real ships? I would be very interesting to know. John |
|
April 11, 2010, 19:29 |
|
#117 | |
Member
Alex
Join Date: Apr 2010
Posts: 32
Rep Power: 16 |
Quote:
I have downloaded your test case, and I am trying to run the roll case of shipFoam tutorials, which I have compiled. ran blockMesh,snappyHexMesh, and setFields... Only when I try to run shipFoam, i get this message... Code:
alex@iskandhar:~/OpenFOAM/alex-1.6/Breeder_1.6/shipHydrodynamicIG/tutorials/shipFoamDemosL/roll$ shipFoam /*---------------------------------------------------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 1.5.x | | \\ / A nd | Web: http://www.OpenFOAM.org | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ Exec : shipFoam Date : Apr 11 2010 Time : 23:12:57 Host : iskandhar PID : 5245 Case : /home/alex/OpenFOAM/alex-1.6/Breeder_1.6/shipHydrodynamicIG/tutorials/shipFoamDemosL/roll nProcs : 1 // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Create mesh for time = 0 Selecting dynamicFvMesh dynamicMotionSolverFvMesh Selecting motion solver: velocityLaplacian Selecting motion diffusion: inverseDistance --> FOAM Warning : From function polyBoundaryMesh::patchSet(const wordList& patchNames) in file meshes/polyMesh/polyBoundaryMesh/polyBoundaryMesh.C at line 429 Cannot find any patch names matching Hull Reading environmentalProperties Reading field pd Reading field gamma Reading field U Reading/calculating face flux field phi Reading transportProperties Selecting incompressible transport model Newtonian Selecting incompressible transport model Newtonian Selecting RAS turbulence model laminar time step continuity errors : sum local = 0, global = 0, cumulative = 0 GAMGPCG: Solving for pcorr, Initial residual = 0, Final residual = 0, No Iterations 0 GAMGPCG: Solving for pcorr, Initial residual = 0, Final residual = 0, No Iterations 0 time step continuity errors : sum local = 0, global = 0, cumulative = 0 Courant Number mean: 0 max: 0 motionPatches : 1 ( Hull ) Selecting ODE solver RK Starting time loop Courant Number mean: 0 max: 0 deltaT = 0.00119048 Time = 0.00119048 --> FOAM Warning : From function polyBoundaryMesh::patchSet(const wordList& patchNames) in file meshes/polyMesh/polyBoundaryMesh/polyBoundaryMesh.C at line 429 Cannot find any patch names matching Hull DICPCG: Solving for cellMotionUx, Initial residual = 0, Final residual = 0, No Iterations 0 DICPCG: Solving for cellMotionUy, Initial residual = 0, Final residual = 0, No Iterations 0 DICPCG: Solving for cellMotionUz, Initial residual = 0, Final residual = 0, No Iterations 0 Execution time for mesh.update() = 0.34 s time step continuity errors : sum local = 0, global = 0, cumulative = 0 GAMGPCG: Solving for pcorr, Initial residual = 0, Final residual = 0, No Iterations 0 GAMGPCG: Solving for pcorr, Initial residual = 0, Final residual = 0, No Iterations 0 time step continuity errors : sum local = 0, global = 0, cumulative = 0 MULES: Solving for gamma MULES: Solving for gamma Liquid phase volume fraction = 0.6 Min(gamma) = 0 Max(gamma) = 1 smoothSolver: Solving for Ux, Initial residual = 1, Final residual = 2.31441e-07, No Iterations 1 smoothSolver: Solving for Uy, Initial residual = 1, Final residual = 2.32614e-07, No Iterations 1 smoothSolver: Solving for Uz, Initial residual = 1, Final residual = 6.37222e-07, No Iterations 1 GAMG: Solving for pd, Initial residual = 1, Final residual = 7.61252e-07, No Iterations 9 GAMG: Solving for pd, Initial residual = 3.34915e-07, Final residual = 3.34915e-07, No Iterations 0 Relaxation: pd = 0.2 time step continuity errors : sum local = 1.13473e-24, global = -3.77576e-25, cumulative = -3.77576e-25 GAMG: Solving for pd, Initial residual = 0.637657, Final residual = 4.85218e-07, No Iterations 9 GAMG: Solving for pd, Initial residual = 2.679e-07, Final residual = 2.679e-07, No Iterations 0 Relaxation: pd = 0.2 time step continuity errors : sum local = 9.07413e-25, global = -3.01253e-25, cumulative = -6.78829e-25 GAMG: Solving for pd, Initial residual = 0.438916, Final residual = 8.56251e-07, No Iterations 8 GAMGPCG: Solving for pd, Initial residual = 5.49046e-07, Final residual = 5.49046e-07, No Iterations 0 Relaxation: pd = 0.2 time step continuity errors : sum local = 1.86108e-24, global = -7.55025e-25, cumulative = -1.43385e-24 #0 Foam::error::printStack(Foam::Ostream&) in "/home/alex/OpenFOAM/OpenFOAM-1.5.x/lib/linux64GccDPOpt/libOpenFOAM.so" #1 Foam::sigSegv::sigSegvHandler(int) in "/home/alex/OpenFOAM/OpenFOAM-1.5.x/lib/linux64GccDPOpt/libOpenFOAM.so" #2 ?? in "/lib64/libc.so.6" #3 Foam::tmp<Foam::Field<Foam::innerProduct<Foam::Tensor<double>, Foam::Vector<double> >::type> > Foam::operator&<Foam::Tensor<double>, double, 9, Foam::Vector<double> >(Foam::VectorSpace<Foam::Tensor<double>, double, 9> const&, Foam::UList<Foam::Vector<double> > const&) in "/home/alex/OpenFOAM/alex-1.5.x/applications/bin/linux64GccDPOpt/shipFoam" #4 Foam::bodyMotion::forcesCalc() in "/home/alex/OpenFOAM/alex-1.5.x/applications/bin/linux64GccDPOpt/shipFoam" #5 main in "/home/alex/OpenFOAM/alex-1.5.x/applications/bin/linux64GccDPOpt/shipFoam" #6 __libc_start_main in "/lib64/libc.so.6" #7 _start at /glibc-tmp-f0634f2d3302f870d5141470b2abd3af/glibc-2.9-20090316/csu/../sysdeps/x86_64/elf/start.S:116 Segmentation fault Code:
alex@iskandhar:~/OpenFOAM/alex-1.6/Breeder_1.6/shipHydrodynamicIG/tutorials/shipFoamDemosL/roll$ clear alex@iskandhar:~/OpenFOAM/alex-1.6/Breeder_1.6/shipHydrodynamicIG/tutorials/shipFoamDemosL/roll$ ls 0 0.001 0.002 Hull_motion.txt constant system alex@iskandhar:~/OpenFOAM/alex-1.6/Breeder_1.6/shipHydrodynamicIG/tutorials/shipFoamDemosL/roll$ grep -nH 'Hull' 0/* 0/U:30: Hull 0/gamma.org~:28: Hull 0/pd:28: Hull 0/pointMotionU:30: Hull alex@iskandhar:~/OpenFOAM/alex-1.6/Breeder_1.6/shipHydrodynamicIG/tutorials/shipFoamDemosL/roll$ grep -nH 'Hull' 0.001/* 0.001/cellLevel:113983: Hull_region0 0.001/pointLevel:130536: Hull_region0 alex@iskandhar:~/OpenFOAM/alex-1.6/Breeder_1.6/shipHydrodynamicIG/tutorials/shipFoamDemosL/roll$ grep -nH 'Hull' 0.002/* 0.002/cellLevel:113983: Hull_region0 0.002/meshPhi:350294: Hull_region0 0.002/pointLevel:130536: Hull_region0 alex@iskandhar:~/OpenFOAM/alex-1.6/Breeder_1.6/shipHydrodynamicIG/tutorials/shipFoamDemosL/roll Code:
alex@iskandhar:~/OpenFOAM/alex-1.6/Breeder_1.6/shipHydrodynamicIG/tutorials/shipFoamDemosL/roll$ nano 0.001/cellLevel alex@iskandhar:~/OpenFOAM/alex-1.6/Breeder_1.6/shipHydrodynamicIG/tutorials/shipFoamDemosL/roll$ nano 0.001/pointLevel alex@iskandhar:~/OpenFOAM/alex-1.6/Breeder_1.6/shipHydrodynamicIG/tutorials/shipFoamDemosL/roll$ nano 0.002/cellLevel alex@iskandhar:~/OpenFOAM/alex-1.6/Breeder_1.6/shipHydrodynamicIG/tutorials/shipFoamDemosL/roll$ nano 0.002/pointLevel alex@iskandhar:~/OpenFOAM/alex-1.6/Breeder_1.6/shipHydrodynamicIG/tutorials/shipFoamDemosL/roll$ nano 0.002/meshPhi alex@iskandhar:~/OpenFOAM/alex-1.6/Breeder_1.6/shipHydrodynamicIG/tutorials/shipFoamDemosL/roll$ grep -nH 'Hull_region0' 0.002/* alex@iskandhar:~/OpenFOAM/alex-1.6/Breeder_1.6/shipHydrodynamicIG/tutorials/shipFoamDemosL/roll$ grep -nH 'Hull_region0' 0.001/* alex@iskandhar:~/OpenFOAM/alex-1.6/Breeder_1.6/shipHydrodynamicIG/tutorials/shipFoamDemosL/roll$ grep -nH 'Hull' 0.002/* 0.002/cellLevel:113983: Hull 0.002/meshPhi:350294: Hull 0.002/pointLevel:130536: Hull alex@iskandhar:~/OpenFOAM/alex-1.6/Breeder_1.6/shipHydrodynamicIG/tutorials/shipFoamDemosL/roll$ grep -nH 'Hull' 0.001/* 0.001/cellLevel:113983: Hull 0.001/pointLevel:130536: Hull alex@iskandhar:~/OpenFOAM/alex-1.6/Breeder_1.6/shipHydrodynamicIG/tutorials/shipFoamDemosL/roll$ shipFoam Code:
alex@iskandhar:~/OpenFOAM/alex-1.6/Breeder_1.6/shipHydrodynamicIG/tutorials/shipFoamDemosL/roll$ shipFoam /*---------------------------------------------------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 1.5.x | | \\ / A nd | Web: http://www.OpenFOAM.org | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ Exec : shipFoam Date : Apr 11 2010 Time : 23:22:58 Host : iskandhar PID : 5287 Case : /home/alex/OpenFOAM/alex-1.6/Breeder_1.6/shipHydrodynamicIG/tutorials/shipFoamDemosL/roll nProcs : 1 // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Create mesh for time = 0 Selecting dynamicFvMesh dynamicMotionSolverFvMesh Selecting motion solver: velocityLaplacian Selecting motion diffusion: inverseDistance --> FOAM Warning : From function polyBoundaryMesh::patchSet(const wordList& patchNames) in file meshes/polyMesh/polyBoundaryMesh/polyBoundaryMesh.C at line 429 Cannot find any patch names matching Hull Reading environmentalProperties Reading field pd Reading field gamma Reading field U Reading/calculating face flux field phi Reading transportProperties Selecting incompressible transport model Newtonian Selecting incompressible transport model Newtonian Selecting RAS turbulence model laminar time step continuity errors : sum local = 0, global = 0, cumulative = 0 GAMGPCG: Solving for pcorr, Initial residual = 0, Final residual = 0, No Iterations 0 GAMGPCG: Solving for pcorr, Initial residual = 0, Final residual = 0, No Iterations 0 time step continuity errors : sum local = 0, global = 0, cumulative = 0 Courant Number mean: 0 max: 0 motionPatches : 1 ( Hull ) Selecting ODE solver RK Starting time loop Courant Number mean: 0 max: 0 deltaT = 0.00119048 Time = 0.00119048 --> FOAM Warning : From function polyBoundaryMesh::patchSet(const wordList& patchNames) in file meshes/polyMesh/polyBoundaryMesh/polyBoundaryMesh.C at line 429 Cannot find any patch names matching Hull DICPCG: Solving for cellMotionUx, Initial residual = 0, Final residual = 0, No Iterations 0 DICPCG: Solving for cellMotionUy, Initial residual = 0, Final residual = 0, No Iterations 0 DICPCG: Solving for cellMotionUz, Initial residual = 0, Final residual = 0, No Iterations 0 Execution time for mesh.update() = 0.33 s time step continuity errors : sum local = 0, global = 0, cumulative = 0 GAMGPCG: Solving for pcorr, Initial residual = 0, Final residual = 0, No Iterations 0 GAMGPCG: Solving for pcorr, Initial residual = 0, Final residual = 0, No Iterations 0 time step continuity errors : sum local = 0, global = 0, cumulative = 0 MULES: Solving for gamma MULES: Solving for gamma Liquid phase volume fraction = 0.6 Min(gamma) = 0 Max(gamma) = 1 smoothSolver: Solving for Ux, Initial residual = 1, Final residual = 2.31441e-07, No Iterations 1 smoothSolver: Solving for Uy, Initial residual = 1, Final residual = 2.32614e-07, No Iterations 1 smoothSolver: Solving for Uz, Initial residual = 1, Final residual = 6.37222e-07, No Iterations 1 GAMG: Solving for pd, Initial residual = 1, Final residual = 7.61252e-07, No Iterations 9 GAMG: Solving for pd, Initial residual = 3.34915e-07, Final residual = 3.34915e-07, No Iterations 0 Relaxation: pd = 0.2 time step continuity errors : sum local = 1.13473e-24, global = -3.77576e-25, cumulative = -3.77576e-25 GAMG: Solving for pd, Initial residual = 0.637657, Final residual = 4.85218e-07, No Iterations 9 GAMG: Solving for pd, Initial residual = 2.679e-07, Final residual = 2.679e-07, No Iterations 0 Relaxation: pd = 0.2 time step continuity errors : sum local = 9.07413e-25, global = -3.01253e-25, cumulative = -6.78829e-25 GAMG: Solving for pd, Initial residual = 0.438916, Final residual = 8.56251e-07, No Iterations 8 GAMGPCG: Solving for pd, Initial residual = 5.49046e-07, Final residual = 5.49046e-07, No Iterations 0 Relaxation: pd = 0.2 time step continuity errors : sum local = 1.86108e-24, global = -7.55025e-25, cumulative = -1.43385e-24 #0 Foam::error::printStack(Foam::Ostream&) in "/home/alex/OpenFOAM/OpenFOAM-1.5.x/lib/linux64GccDPOpt/libOpenFOAM.so" #1 Foam::sigSegv::sigSegvHandler(int) in "/home/alex/OpenFOAM/OpenFOAM-1.5.x/lib/linux64GccDPOpt/libOpenFOAM.so" #2 ?? in "/lib64/libc.so.6" #3 Foam::tmp<Foam::Field<Foam::innerProduct<Foam::Tensor<double>, Foam::Vector<double> >::type> > Foam::operator&<Foam::Tensor<double>, double, 9, Foam::Vector<double> >(Foam::VectorSpace<Foam::Tensor<double>, double, 9> const&, Foam::UList<Foam::Vector<double> > const&) in "/home/alex/OpenFOAM/alex-1.5.x/applications/bin/linux64GccDPOpt/shipFoam" #4 Foam::bodyMotion::forcesCalc() in "/home/alex/OpenFOAM/alex-1.5.x/applications/bin/linux64GccDPOpt/shipFoam" #5 main in "/home/alex/OpenFOAM/alex-1.5.x/applications/bin/linux64GccDPOpt/shipFoam" #6 __libc_start_main in "/lib64/libc.so.6" #7 _start at /glibc-tmp-f0634f2d3302f870d5141470b2abd3af/glibc-2.9-20090316/csu/../sysdeps/x86_64/elf/start.S:116 Segmentation fault alex@iskandhar:~/OpenFOAM/alex-1.6/Breeder_1.6/shipHydrodynamicIG/tutorials/shipFoamDemosL/roll$ What am I doing wrong here...? Can I use shipFoam to evaluate the phugoid mode period of a subsonic aircraft...? Defining stiffness constants for roll, pitch and yaw motions about the main inertia axes as functions of the gain of the controlers ( sort of restoration forces ) ... Alex |
||
April 11, 2010, 20:05 |
trying Now shipFoam from OF-1.6 Breeder ...
|
#118 |
Member
Alex
Join Date: Apr 2010
Posts: 32
Rep Power: 16 |
I have also downloaded and Installed OpenFOAM-1.6 as well as Breeder_1.6 utilities solvers and tutorials... compiled shipFoam successfully...
Trying the roll tutorial now : Code:
alex@iskandhar:~/OpenFOAM/alex-1.6/Breeder_1.6/shipHydrodynamicIG/tutorials/shipFoam/roll$ ls -l total 16 drwxr-xr-x 2 alex users 4096 2010-01-04 07:52 0 -rw-r--r-- 1 alex users 505 2010-01-04 07:52 Allrun drwxr-xr-x 4 alex users 4096 2010-01-04 07:52 constant drwxr-xr-x 2 alex users 4096 2010-01-04 07:52 system alex@iskandhar:~/OpenFOAM/alex-1.6/Breeder_1.6/shipHydrodynamicIG/tutorials/shipFoam/roll$ cat Allrun #!/bin/sh # Source tutorial run functions . $WM_PROJECT_DIR/bin/tools/RunFunctions runApplication blockMesh runApplication snappyHexMesh -overwrite cat constant/polyMesh/boundary | sed 's/Hull.*/Hull/' > constant/polyMesh/boundary2 rm constant/polyMesh/boundary mv constant/polyMesh/boundary2 constant/polyMesh/boundary cp 0/alpha1.org~ 0/alpha1 runApplication setFields runApplication shipFoam runApplication foamToVTK # ----------------------------------------------------------------------------- trying ./Allrun now... Code:
alex@iskandhar:~/OpenFOAM/alex-1.6/Breeder_1.6/shipHydrodynamicIG/tutorials/shipFoam/roll$ ./Allrun Running blockMesh on /home/alex/OpenFOAM/alex-1.6/Breeder_1.6/shipHydrodynamicIG/tutorials/shipFoam/roll Running snappyHexMesh on /home/alex/OpenFOAM/alex-1.6/Breeder_1.6/shipHydrodynamicIG/tutorials/shipFoam/roll cp: cannot stat `0/alpha1.org~': No such file or directory Running setFields on /home/alex/OpenFOAM/alex-1.6/Breeder_1.6/shipHydrodynamicIG/tutorials/shipFoam/roll Running shipFoam on /home/alex/OpenFOAM/alex-1.6/Breeder_1.6/shipHydrodynamicIG/tutorials/shipFoam/roll Running foamToVTK on /home/alex/OpenFOAM/alex-1.6/Breeder_1.6/shipHydrodynamicIG/tutorials/shipFoam/roll alex@iskandhar:~/OpenFOAM/alex-1.6/Breeder_1.6/shipHydrodynamicIG/tutorials/shipFoam/roll$ Code:
Running setFields on /home/alex/OpenFOAM/alex-1.6/Breeder_1.6/shipHydrodynamicIG/tutorials/shipFoam/roll Running shipFoam on /home/alex/OpenFOAM/alex-1.6/Breeder_1.6/shipHydrodynamicIG/tutorials/shipFoam/roll Running foamToVTK on /home/alex/OpenFOAM/alex-1.6/Breeder_1.6/shipHydrodynamicIG/tutorials/shipFoam/roll alex@iskandhar:~/OpenFOAM/alex-1.6/Breeder_1.6/shipHydrodynamicIG/tutorials/shipFoam/roll$ ls 0 Allrun VTK constant log.blockMesh log.foamToVTK log.setFields log.shipFoam log.snappyHexMesh system alex@iskandhar:~/OpenFOAM/alex-1.6/Breeder_1.6/shipHydrodynamicIG/tutorials/shipFoam/roll$ rm -rf log* VTK alex@iskandhar:~/OpenFOAM/alex-1.6/Breeder_1.6/shipHydrodynamicIG/tutorials/shipFoam/roll$ ls 0 U p pointMotionU alex@iskandhar:~/OpenFOAM/alex-1.6/Breeder_1.6/shipHydrodynamicIG/tutorials/shipFoam/roll$ What can I do to run a shipFoam demo successfully...? Alex |
|
April 11, 2010, 20:09 |
Trying again in OF-1.6
|
#119 |
Member
Alex
Join Date: Apr 2010
Posts: 32
Rep Power: 16 |
Removed content
Last edited by Alexvader; April 11, 2010 at 20:10. Reason: Double Posting accidentally... |
|
April 11, 2010, 21:27 |
|
#120 |
New Member
Julius
Join Date: Mar 2009
Posts: 27
Rep Power: 17 |
Hello Alexvader,
I guess that after all your changes you "forgot" to change the boundary file (constant/polyMesh/boundary) where the "hull" patch should appear instead of hull_region0. Normally it would be more elegant to change the name of the motion patch in the dynamicMeshDict (constant/dynamicMeshDict) so that only one modification is necessary. The mentioned line could look like this: diffusivity inverseDistance 1(hull_region0); Good Luck |
|
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
hydrostatic pressure | Amanda | FLUENT | 6 | April 20, 2016 12:00 |
Hydrostatic pressure(rho*g*h) | Pranesh | FloEFD, FloWorks & FloTHERM | 3 | October 17, 2008 07:18 |
hydrostatic pressure | multiphase | FLUENT | 0 | May 18, 2003 16:16 |
Hydrostatic pressure in 5.5 | Jens | CFX | 3 | August 21, 2002 12:05 |
Hydrostatic Pressure | Rhydar | CFX | 3 | March 6, 2002 10:54 |