[ngj]

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.

[kjetil]

Originally Posted by ngj

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

Well, this is in fact a single-phase case at the moment, using water only. Apart from that I totally agree on this being "unphysical". The tutorial file on solver compressibleInterFoam is terribly incomplete and does not display any proper use of it. I have tried to make this case as straight forward as possible, and at the moment everything seems "ok" - except from this pressure field.

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 ...

[ngj]

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

[kjetil]

Originally Posted by ngj

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.

Thanks. Well, I paste here what I believe is most crucial. If needed the entire case tree can be found online here http://folk.ntnu.no/kjetilbi/openfoam/nr5-auto2/ .

Content of 0/U:

internalField uniform (0 0 0);

boundaryField

{
inlet
{
type zeroGradient;
}
outlet
{
type zeroGradient;
}
pipewall
{
type fixedValue;
value uniform (0 0 0);
}
}

Content of 0/P:

internalField uniform 0;

boundaryField
{
inlet
{
type fixedValue;
value uniform 0;
}
outlet
{
type zeroGradient;
}
pipewall
{
type zeroGradient;

}
}

And a snippet from transportProperties:

// liq
phase2
{
transportModel Newtonian;
nu nu [0 2 -1 0 0 0 0] 1e-6;
rho rho [1 -3 0 0 0 0 0] 1000;
rho0 rho0 [1 -3 0 0 0 0 0] 1000;
psi psi [ 0 -2 2 0 0 ] 1e-05;
}

// gas
phase1
{
transportModel Newtonian;
nu nu [0 2 -1 0 0 0 0] 1.2e-5;
rho rho [1 -3 0 0 0 0 0] 1.2;
rho0 rho0 [1 -3 0 0 0 0 0] 1.2;
psi psi [ 0 -2 2 0 0 ] 1e-05;
}

pMin pMin [ 1 -1 -2 0 0 0 0 ] 0;

sigma sigma [ 1 0 -2 0 0 0 0 ] 0.07;

Basically, 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.

[ngj]

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

[kjetil]

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.

[kjetil]

... 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 ...

[ngj]

Try setting pMin to some large negative value, e.g. -1e10, and see if you can solve the problem using compressibleInterfoam.

Bests

Niels

[kjetil]

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 ...

[kjetil]

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...

[ngj]

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

[kjetil]

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 ...

[piprus]

Could any one of you explain me shortly what is the meaning or difference between rho and rho0 in the transportProperties?

[maruthamuthu_venkatraman]

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

[markc]

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

[johnb]

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

[Alexvader]

Originally Posted by markc

O ja,

the demo cases are run using:
1. blockMesh
2. snappyHexMesh
3. setFields
4. shipFoam

Mark

Hi, I am interested in 3d ship motion simulation, and I have installed OpenFOAM-1.5

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...

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

grepping a little bit, i found this :

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

so I have changed all occurrences of 'Hull_region0' in the refered files to 'Hull', trying again :

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

No avail....

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

[Alexvader]

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 :

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...

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$

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

[Alexvader]

Removed content

[juliuslein]

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