Error trying to compile new solver.C

LThomes · June 20, 2017, 10:11

Hello,
I'm trying to control the Courrant number and my ajustTimeStep is not working. So I think i have to modify the icoFoam.C to be able to make it work. However, I'm facing some trouble.
I'm following this tutorial http://www.tfd.chalmers.se/~hani/kur...tersReport.pdf to create a new solver "myIcoFoam".
So I've done these steps:
_____________________________________

Code:

sol
cp -r incompressible/icoFoam/ $WM_PROJECT_USER_DIR/applications/solvers/
cd $WM_PROJECT_USER_DIR/applications/solvers
mv icoFoam myIcoFoam
cd myIcoFoam
mv icoFoam.C myIcoFoam.C
sed -i s/icoFoam/myIcoFoam/g myIcoFoam.C
sed -i s/icoFoam/myIcoFoam/g Make/files

To set the library path right, do following change in Make/files:
change
EXE = $(FOAM_APPBIN)/icoFoam
to
EXE = $(FOAM_USER_APPBIN)/myIcoFoam
And also change in Make/options:
-I../dieselEngineFoam \
to
-I$(LIB_SRC)/../applications/solvers/combustion/dieselEngineFoam \
____________________________________________

I did not understand this last step very well, so I wrote this:

Code:

EXE_INC = \
    -I$(LIB_SRC)/finiteVolume/applications/solvers/lnInclude \
    -I$(LIB_SRC)/meshTools/applications/solvers/lnInclude

EXE_LIBS = \
    -lfiniteVolume \
    -lmeshTools

The previous "options" was:

Code:

EXE_INC = \
    -I$(LIB_SRC)/finiteVolume/lnInclude \
    -I$(LIB_SRC)/meshTools/lnInclude

EXE_LIBS = \
    -lfiniteVolume \
    -lmeshTools

Finally, I'm getting the following error:

Code:

[ofuser@default myIcoFoam]$ wmake
Making dependency list for source file myIcoFoam.C
could not open file fvCFD.H for source file myIcoFoam.C due to No such file or directory
could not open file pisoControl.H for source file myIcoFoam.C due to No such file or directory
could not open file createPhi.H for source file myIcoFoam.C due to No such file or directory
could not open file initContinuityErrs.H for source file myIcoFoam.C due to No such file or directory
could not open file CourantNo.H for source file myIcoFoam.C due to No such file or directory
could not open file continuityErrs.H for source file myIcoFoam.C due to No such file or directory
g++ -std=c++11 -m64 -DOPENFOAM_PLUS=1612 -Dlinux64 -DWM_ARCH_OPTION=64 -DWM_DP -DWM_LABEL_SIZE=32 -Wall -Wextra -Wold-style-cast -Wnon-virtual-dtor -Wno-unused-parameter -Wno-invalid-offsetof -O3  -DNoRepository -ftemplate-depth-100 -I/opt/OpenFOAM/OpenFOAM-v1612+/src/finiteVolume/applications/solvers/lnInclude -I/opt/OpenFOAM/OpenFOAM-v1612+/src/meshTools/applications/solvers/lnInclude -IlnInclude -I. -I/opt/OpenFOAM/OpenFOAM-v1612+/src/OpenFOAM/lnInclude -I/opt/OpenFOAM/OpenFOAM-v1612+/src/OSspecific/POSIX/lnInclude   -fPIC -c myIcoFoam.C -o Make/linux64GccDPInt32Opt/myIcoFoam.o
myIcoFoam.C:63:19: fatal error: fvCFD.H: No such file or directory
 #include "fvCFD.H"

Can anybody help me? I'm using OpenFOAM for Windows, so I'm fiding it a little bit difficult to modify these things

floquation · June 20, 2017, 10:31

Quote:

Originally Posted by LThomes

I did not understand this last step very well, so I wrote this:

That's why it goes wrong there.

Quote:

Originally Posted by LThomes

Code:

EXE_INC = \
    -I$(LIB_SRC)/finiteVolume/applications/solvers/lnInclude \
    -I$(LIB_SRC)/meshTools/applications/solvers/lnInclude

EXE_LIBS = \
    -lfiniteVolume \
    -lmeshTools

The previous "options" was:

Code:

EXE_INC = \
    -I$(LIB_SRC)/finiteVolume/lnInclude \
    -I$(LIB_SRC)/meshTools/lnInclude

EXE_LIBS = \
    -lfiniteVolume \
    -lmeshTools

Clearly, the directory I put in bold does not exist, so you are bound to get an error!
The -I option should link to the directory that contains some common OF headers... This should be exactly the same for both icoFoam and my_icoFoam, so it is very simple what you need to do there: don't touch anything.

This replacement:

Code:

-I../dieselEngineFoam \
to
-I$(LIB_SRC)/../applications/solvers/combustion/dieselEngineFoam \

links your copied solver to the original solver, allowing you to use its header files, rather than copying them.
Clearly, this is a nicer thing to do (as you don't have to duplicate unnecessary things), but I recommend you don't do so, as you are not yet comfortable with making those judgment calls.

Quote:

Originally Posted by LThomes

Can anybody help me? I'm using OpenFOAM for Windows, so I'm fiding it a little bit difficult to modify these things

Disclaimer: I don't know about using OpenFOAM on Windows.
Whereas I like Windows for the "normal" things, Linux beats Windows by far when we talk about software development.

LThomes · June 21, 2017, 09:29

floquation,
Thanks for your prompt reply. But if I don't touch anything in the "options", I have the following error:

Code:

[ofuser@default myIcoFoam]$ wmake
Making dependency list for source file myIcoFoam.C
g++ -std=c++11 -m64 -DOPENFOAM_PLUS=1612 -Dlinux64 -DWM_ARCH_OPTION=64 -DWM_DP -DWM_LABEL_SIZE=32 -Wall -Wextra -Wold-style-cast -Wnon-virtual-dtor -Wno-unused-parameter -Wno-invalid-offsetof -O3  -DNoRepository -ftemplate-depth-100 -I/opt/OpenFOAM/OpenFOAM-v1612+/src/finiteVolume/lnInclude -I/opt/OpenFOAM/OpenFOAM-v1612+/src/meshTools/lnInclude -IlnInclude -I. -I/opt/OpenFOAM/OpenFOAM-v1612+/src/OpenFOAM/lnInclude -I/opt/OpenFOAM/OpenFOAM-v1612+/src/OSspecific/POSIX/lnInclude   -fPIC -c myIcoFoam.C -o Make/linux64GccDPInt32Opt/myIcoFoam.o
g++ -std=c++11 -m64 -DOPENFOAM_PLUS=1612 -Dlinux64 -DWM_ARCH_OPTION=64 -DWM_DP -DWM_LABEL_SIZE=32 -Wall -Wextra -Wold-style-cast -Wnon-virtual-dtor -Wno-unused-parameter -Wno-invalid-offsetof -O3  -DNoRepository -ftemplate-depth-100 -I/opt/OpenFOAM/OpenFOAM-v1612+/src/finiteVolume/lnInclude -I/opt/OpenFOAM/OpenFOAM-v1612+/src/meshTools/lnInclude -IlnInclude -I. -I/opt/OpenFOAM/OpenFOAM-v1612+/src/OpenFOAM/lnInclude -I/opt/OpenFOAM/OpenFOAM-v1612+/src/OSspecific/POSIX/lnInclude   -fPIC -Xlinker --add-needed -Xlinker --no-as-needed Make/linux64GccDPInt32Opt/myIcoFoam.o -L/opt/OpenFOAM/OpenFOAM-v1612+/platforms/linux64GccDPInt32Opt/lib \
            -lfiniteVolume -lmeshTools -lOpenFOAM -ldl  \
             -lm -o /home/ofuser/OpenFOAM/ofuser-v1612+/platforms/linux64GccDPInt32Opt/bin/myIcoFoam

Quote:

Whereas I like Windows for the "normal" things, Linux beats Windows by far when we talk about software development.

It's not my choice to use Windows xD

floquation · June 21, 2017, 10:16

That's not an error.

When a compiler is called, it shows you the entire command. That's what the Makefile does.

The three lines you see right there do the following:

It finds the dependencies of myIcoFoam, such that it can compile the dependencies before compiling myIcoFoam. You have no dependencies that need compilation, so it then proceeds with:
It compiles myIcoFoam.C to Make/.../myIcoFoam.o
It links Make/.../myIcoFoam.o, which gives you the executable myIcoFoam in $FOAM_USER_APPBIN

If you'd now type "wmake" again, it will show you "myIcoFoam is up to date", which indicates that everything was successful.

LThomes · June 22, 2017, 07:04

Thank you so much. I'm so used to getting error messages, that I thought it was another one

akidess · June 22, 2017, 07:23

Did you go through all these hoops just to control the time step? Why not use pimpleFoam?

LThomes · June 23, 2017, 06:24

Quote:

Originally Posted by akidess

Did you go through all these hoops just to control the time step? Why not use pimpleFoam?

I didn't know that the ajustTimeStep would work with pimpleFoam, if it works it's a great idea indeed. Thank you.

LThomes · June 23, 2017, 10:24

Hello again,
Now I'm trying to modify the myIcoFoam.C file to enable the ajustTimeStep. This is what I did:

Code:

int main(int argc, char *argv[])
{
    #include "setRootCase.H"
    #include "createTime.H"
    #include "createMesh.H"

    pisoControl piso(mesh);

    #include "createFields.H"
    #include "initContinuityErrs.H"
	

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

    Info<< "\nStarting time loop\n" << endl;

    //while (runTime.loop())	// dropped
	while (runTime.run())       // added
    {
		#include "readTimeControls.H"	// added
		#include "setDeltaT.H" // added

        runTime++;            // added
		
        Info<< "Time = " << runTime.timeName() << nl << endl;
		

        #include "CourantNo.H"

        // Momentum predictor

        fvVectorMatrix UEqn
        (
             .
             .
             .

But when I try to compile it, this message appears:

Code:

[ofuser@default myPisoFoam]$ wmake
g++ -std=c++11 -m64 -DOPENFOAM_PLUS=1612 -Dlinux64 -DWM_ARCH_OPTION=64 -DWM_DP -DWM_LABEL_SIZE=32 -Wall -Wextra -Wold-style-cast -Wnon-virtual-dtor -Wno-unused-parameter -Wno-invalid-offsetof -O3  -DNoRepository -ftemplate-depth-100 -I/opt/OpenFOAM/OpenFOAM-v1612+/src/TurbulenceModels/turbulenceModels/lnInclude -I/opt/OpenFOAM/OpenFOAM-v1612+/src/TurbulenceModels/incompressible/lnInclude -I/opt/OpenFOAM/OpenFOAM-v1612+/src/transportModels -I/opt/OpenFOAM/OpenFOAM-v1612+/src/transportModels/incompressible/singlePhaseTransportModel -I/opt/OpenFOAM/OpenFOAM-v1612+/src/finiteVolume/lnInclude -I/opt/OpenFOAM/OpenFOAM-v1612+/src/meshTools/lnInclude -I/opt/OpenFOAM/OpenFOAM-v1612+/src/sampling/lnInclude -IlnInclude -I[ofuser@default myIcoFoam]$ wmake
Making dependency list for source file myIcoFoam.C
g++ -std=c++11 -m64 -DOPENFOAM_PLUS=1612 -Dlinux64 -DWM_ARCH_OPTION=64 -DWM_DP -DWM_LABEL_SIZE=32 -Wall -Wextra -Wold-style-cast -Wnon-virtual-dtor -Wno-unused-parameter -Wno-invalid-offsetof -O3  -DNoRepository -ftemplate-depth-100 -I/opt/OpenFOAM/OpenFOAM-v1612+/src/finiteVolume/lnInclude -I/opt/OpenFOAM/OpenFOAM-v1612+/src/meshTools/lnInclude -IlnInclude -I. -I/opt/OpenFOAM/OpenFOAM-v1612+/src/OpenFOAM/lnInclude -I/opt/OpenFOAM/OpenFOAM-v1612+/src/OSspecific/POSIX/lnInclude   -fPIC -c myIcoFoam.C -o Make/linux64GccDPInt32Opt/myIcoFoam.o
In file included from myIcoFoam.C:79:0:
/opt/OpenFOAM/OpenFOAM-v1612+/src/finiteVolume/lnInclude/readTimeControls.H: In function ‘int main(int, char**)’:
/opt/OpenFOAM/OpenFOAM-v1612+/src/finiteVolume/lnInclude/readTimeControls.H:32:1: error: ‘adjustTimeStep’ was not declared in this scope
 adjustTimeStep =
 ^
/opt/OpenFOAM/OpenFOAM-v1612+/src/finiteVolume/lnInclude/readTimeControls.H:35:1: error: ‘maxCo’ was not declared in this scope
 maxCo =
 ^
/opt/OpenFOAM/OpenFOAM-v1612+/src/finiteVolume/lnInclude/readTimeControls.H:38:1: error: ‘maxDeltaT’ was not declared in this scope
 maxDeltaT =
 ^
In file included from myIcoFoam.C:90:0:
/opt/OpenFOAM/OpenFOAM-v1612+/src/finiteVolume/lnInclude/setDeltaT.H:36:35: error: ‘CoNum’ was not declared in this scope
     scalar maxDeltaTFact = maxCo/(CoNum + SMALL);
                                   ^
make: *** [Make/linux64GccDPInt32Opt/myIcoFoam.o] Error 1

The readTimeControls.H has the following lines:

Code:

adjustTimeStep =
    runTime.controlDict().lookupOrDefault("adjustTimeStep", false);

maxCo =
    runTime.controlDict().lookupOrDefault<scalar>("maxCo", 1.0);

maxDeltaT =
    runTime.controlDict().lookupOrDefault<scalar>("maxDeltaT", GREAT);

Could anybody help me fix this error?

floquation · June 23, 2017, 10:29

You are missing

Code:

    #include "createTimeControls.H"

next to createTime.H etc.

You can easily figure that out by opening a solver that supports this, like pimpleFoam or interFoam.

LThomes · June 26, 2017, 08:44

Quote:

You can easily figure that out by opening a solver that supports this, like pimpleFoam or interFoam.

I actually did that, I can't believe I missed that line, I'm sorry >.< . Thank you very much for your patience.

Saleh Abuhanieh · November 28, 2017, 09:54

Quote:

Originally Posted by floquation

That's not an error.

When a compiler is called, it shows you the entire command. That's what the Makefile does.

The three lines you see right there do the following:

It finds the dependencies of myIcoFoam, such that it can compile the dependencies before compiling myIcoFoam. You have no dependencies that need compilation, so it then proceeds with:
It compiles myIcoFoam.C to Make/.../myIcoFoam.o
It links Make/.../myIcoFoam.o, which gives you the executable myIcoFoam in $FOAM_USER_APPBIN

If you'd now type "wmake" again, it will show you "myIcoFoam is up to date", which indicates that everything was successful.

Hi Kevin, Actually what LThomes did (modifying the Make/option file)is one of the solution posted in web to solve the errors which are related to compiling new solver. I almost tried all the ways!
now, I am trying to compile new solver (first exercise only changing the name and the Make/file) and when I execute the wmake command, I receive the following error:

make: *** No rule to make target '/opt/OpenFOAM-dev-debug/platforms/linux64GccDPInt32Debug/applications/solvers/incompressible/my_icoFoam/my_icoFoam.C.dep', needed by '/opt/OpenFOAM-dev-debug/platforms/linux64GccDPInt32Debug/applications/solvers/incompressible/my_icoFoam/my_icoFoam.o'. Stop."

Thank you in advance

jiahui_93 · May 16, 2018, 09:42

Quote:

Originally Posted by floquation

That's not an error.

When a compiler is called, it shows you the entire command. That's what the Makefile does.

The three lines you see right there do the following:

It finds the dependencies of myIcoFoam, such that it can compile the dependencies before compiling myIcoFoam. You have no dependencies that need compilation, so it then proceeds with:
It compiles myIcoFoam.C to Make/.../myIcoFoam.o
It links Make/.../myIcoFoam.o, which gives you the executable myIcoFoam in $FOAM_USER_APPBIN

If you'd now type "wmake" again, it will show you "myIcoFoam is up to date", which indicates that everything was successful.

Hi, your explanation made me at least understand the main steps of compilation

thx
i am facing a problem when trying to compile my own modified movingConeTopFvMesh which existed in openfoam4 and 5. I followed the steps to change the name of C and H file, their contents, as well as edit Make/file and run wmake. But it output errors:

When I run wmake in openfoam4,

Code:

wmakeLnInclude: linking include files to ./lnInclude
make: *** No rule to make target '/opt/openfoam4/platforms/linux64GccDPInt32Opt/applications/topoChangerFvMesh/topoChangerFvMesh/topoChangerFvMesh2.C.dep', needed by '/opt/openfoam4/platforms/linux64GccDPInt32Opt/applications/topoChangerFvMesh/topoChangerFvMesh/topoChangerFvMesh2.o'.  Stop.

When i run wmake libso in openfoam5,

Code:

wmakeLnInclude: linking include files to ./lnInclude
make: *** No rule to make target 'Make/linux64GccDPInt32Opt/topoChangerFvMesh/JH_topoChangerFvMesh.C.dep', needed by 'Make/linux64GccDPInt32Opt/topoChangerFvMesh/JH_topoChangerFvMesh.o'.  Stop.

i tried to wclean and allwmake in src dir, and got some error output at the end of compilation.

Code:

/opt/openfoam4/src/parallel/decompose/scotchDecomp
Making dependency list for source file scotchDecomp.C
could not open file scotch.h for source file scotchDecomp.C due to No such file or directory
g++ -std=c++0x -m64 -Dlinux64 -DWM_ARCH_OPTION=64 -DWM_DP -DWM_LABEL_SIZE=32 -Wall -Wextra -Wold-style-cast -Wnon-virtual-dtor -Wno-unused-parameter -Wno-invalid-offsetof -O3  -DNoRepository -ftemplate-depth-100 -DOMPI_SKIP_MPICXX -I/usr/lib/openmpi/include/openmpi/opal/mca/event/libevent2021/libevent -I/usr/lib/openmpi/include/openmpi/opal/mca/event/libevent2021/libevent/include -I/usr/lib/openmpi/include -I/usr/lib/openmpi/include/openmpi -pthread -I/include -I/opt/ThirdParty-4.1/platforms/linux64GccDPInt32/scotch_6.0.3/include -I/usr/include/scotch -I../decompositionMethods/lnInclude -IlnInclude -I. -I/opt/openfoam4/src/OpenFOAM/lnInclude -I/opt/openfoam4/src/OSspecific/POSIX/lnInclude   -fPIC -c scotchDecomp.C -o /opt/openfoam4/platforms/linux64GccDPInt32Opt/src/parallel/decompose/scotchDecomp/scotchDecomp.o
scotchDecomp.C:36:20: fatal error: scotch.h: No such file or directory
compilation terminated.
/opt/openfoam4/wmake/rules/General/transform:8: recipe for target '/opt/openfoam4/platforms/linux64GccDPInt32Opt/src/parallel/decompose/scotchDecomp/scotchDecomp.o' failed
make: *** [/opt/openfoam4/platforms/linux64GccDPInt32Opt/src/parallel/decompose/scotchDecomp/scotchDecomp.o] Error 1

I tried uninstall and re install openfoam4, and even tried compiling my new class to openfoam5. But both of them didn't work.

May i get some advice here on how to solve this? thanks a lot

jiahui_93 · May 26, 2018, 23:55

Quote:

Originally Posted by Saleh Abuhanieh

Hi Kevin, Actually what LThomes did (modifying the Make/option file)is one of the solution posted in web to solve the errors which are related to compiling new solver. I almost tried all the ways!
now, I am trying to compile new solver (first exercise only changing the name and the Make/file) and when I execute the wmake command, I receive the following error:

make: *** No rule to make target '/opt/OpenFOAM-dev-debug/platforms/linux64GccDPInt32Debug/applications/solvers/incompressible/my_icoFoam/my_icoFoam.C.dep', needed by '/opt/OpenFOAM-dev-debug/platforms/linux64GccDPInt32Debug/applications/solvers/incompressible/my_icoFoam/my_icoFoam.o'. Stop."

Thank you in advance

hi, i'm getting the exactly same message as you. Do you solve your problem? Do you mind to share here? thanks

SHANRU · May 2, 2020, 15:34

Quote:

Originally Posted by jiahui_93

hi, i'm getting the exactly same message as you. Do you solve your problem? Do you mind to share here? thanks

you need to replace the icoFoam with my_icoFoam in the my_icoFoam.C
sed -i 's/icoFoam/my_icoFoam/g' my_icoFoam.C

neko2650 · May 8, 2020, 04:44

I tried to customise the linearSpring restrain to mylinearSpring and to make the source file readable by any solver I provided the path for executable in files

Code:

mylinearSpring.C

LIB = $(FOAM_USER_LIBBIN)/libmylinearSpring

and in the options, I gave flags as follows

Code:

    -I$(LIB_SRC)/thermophysicalModels/basic/lnInclude \
    -I$(LIB_SRC)/transportModels \
    -I$(LIB_SRC)/transportModels/compressible/lnInclude \
    -I$(LIB_SRC)/TurbulenceModels/turbulenceModels/lnInclude \
    -I$(LIB_SRC)/TurbulenceModels/incompressible/lnInclude \
    -I$(LIB_SRC)/TurbulenceModels/compressible/lnInclude \
    -I$(LIB_SRC)/finiteVolume/lnInclude \
    -I$(LIB_SRC)/meshTools/lnInclude \
    -I$(LIB_SRC)/dynamicMesh/lnInclude \
    -I$(WM_PROJECT_DIR)/src/functionObjects/forces/lnInclude \
    -I$(WM_PROJECT_DIR)/src/sixDoFRigidBodyMotion/lnInclude

LIB_LIBS = \
    -lfluidThermophysicalModels \
    -lincompressibleTransportModels \
    -lcompressibleTransportModels \
    -lturbulenceModels \
    -lincompressibleTurbulenceModels \
    -lcompressibleTurbulenceModels \
    -lspecie \
    -lfileFormats \
    -lfiniteVolume \
    -lmeshTools \

The make file compiled and provided .so file which I added to controlDict in floatingObject example and while running simulation blockMesh, topoSet, subsetMesh, setFields are compiled and while compiling interFoam it gave me the following error

Code:

sreekanth@sreekanth-VirtualBox:~/OpenFOAM/sreekanth-7/run/floatingObject$ interFoam 
/*---------------------------------------------------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Version:  7
     \\/     M anipulation  |
\*---------------------------------------------------------------------------*/
Build  : 7-1ff648926f77
Exec   : interFoam
Date   : May 06 2020
Time   : 09:45:05
Host   : "sreekanth-VirtualBox"
PID    : 2589
I/O    : uncollated
Case   : /home/sreekanth/OpenFOAM/sreekanth-7/run/floatingObject
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 10)
allowSystemOperations : Allowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

--> FOAM Warning : 
    From function void* Foam::dlOpen(const Foam::fileName&, bool)
    in file POSIX.C at line 1251
    dlopen error : /home/sreekanth/OpenFOAM/sreekanth-7/platforms/linux64GccDPInt32Opt/lib/libmylinearSpring.so: undefined symbol: _ZTIN4Foam30sixDoFRigidBodyMotionRestraintE
--> FOAM Warning : 
    From function bool Foam::dlLibraryTable::open(const Foam::fileName&, bool)
    in file db/dynamicLibrary/dlLibraryTable/dlLibraryTable.C at line 105
    could not load "libmylinearSpring.so"
Create mesh for time = 0

Using #calcEntry at line 50 in file "/home/sreekanth/OpenFOAM/sreekanth-7/run/floatingObject/constant/dynamicMeshDict.rigidBodyMotionCoeffs.bodies.floatingObject"
Using #codeStream with "/home/sreekanth/OpenFOAM/sreekanth-7/run/floatingObject/dynamicCode/platforms/linux64GccDPInt32Opt/lib/libcodeStream_96bd56ab6d599ebbc648462330c624ef71f2258c.so"
Selecting dynamicFvMesh dynamicMotionSolverFvMesh
Using #calcEntry at line 50 in file "/home/sreekanth/OpenFOAM/sreekanth-7/run/floatingObject/constant/dynamicMeshDict.rigidBodyMotionCoeffs.bodies.floatingObject"
Selecting motion solver: rigidBodyMotion


--> FOAM FATAL ERROR: 
Unknown restraint type mylinearSpring

Valid restraint types are : 
4
(
linearAxialAngularSpring
linearDamper
linearSpring
sphericalAngularDamper
)
    From function static Foam::autoPtr<Foam::RBD::restraint> Foam::RBD::restraint::New(const Foam::word&, const Foam::dictionary&, const Foam::RBD::rigidBodyModel&)
    in file restraints/restraint/rigidBodyRestraintNew.C at line 45.

FOAM exiting

While checking the code I found that there is a error in loading sixDoFRigidBodyMotionRestraint library using

Code:

 ldd <library path>

In the next step, I added sixDoFRigidBodyMotion in the options

Code:

 EXE_INC = \
    -I$(LIB_SRC)/fileFormats/lnInclude \
    -I$(LIB_SRC)/thermophysicalModels/basic/lnInclude \
    -I$(LIB_SRC)/transportModels \
    -I$(LIB_SRC)/transportModels/compressible/lnInclude \
    -I$(LIB_SRC)/TurbulenceModels/turbulenceModels/lnInclude \
    -I$(LIB_SRC)/TurbulenceModels/incompressible/lnInclude \
    -I$(LIB_SRC)/TurbulenceModels/compressible/lnInclude \
    -I$(LIB_SRC)/finiteVolume/lnInclude \
    -I$(LIB_SRC)/meshTools/lnInclude \
    -I$(LIB_SRC)/dynamicMesh/lnInclude \
    -I$(WM_PROJECT_DIR)/src/functionObjects/forces/lnInclude \
    -I$(WM_PROJECT_DIR)/src/sixDoFRigidBodyMotion/lnInclude

LIB_LIBS = \
    -lfluidThermophysicalModels \
    -lincompressibleTransportModels \
    -lcompressibleTransportModels \
    -lturbulenceModels \
    -lincompressibleTurbulenceModels \
    -lcompressibleTurbulenceModels \
    -lspecie \
    -lfileFormats \
    -lfiniteVolume \
    -lmeshTools \
    -lsixDoFRigidBodyMotion \

and checked again mylinearSpring.so libraries for the included libsixDoFRigidBodyMotion.so library using

Code:

 ldd <library path>

Code:

 sreekanth@sreekanth-VirtualBox:~$ ldd /home/sreekanth/OpenFOAM/sreekanth-7/platforms/linux64GccDPInt32Opt/lib/libmylinearSpring.so
	linux-vdso.so.1 =>  (0x00007ffea23ef000)
	libfluidThermophysicalModels.so => /opt/openfoam7/platforms/linux64GccDPInt32Opt/lib/libfluidThermophysicalModels.so (0x00007f45475ef000)
	libincompressibleTransportModels.so => /opt/openfoam7/platforms/linux64GccDPInt32Opt/lib/libincompressibleTransportModels.so (0x00007f454734d000)
	libcompressibleTransportModels.so => /opt/openfoam7/platforms/linux64GccDPInt32Opt/lib/libcompressibleTransportModels.so (0x00007f4547149000)
	libturbulenceModels.so => /opt/openfoam7/platforms/linux64GccDPInt32Opt/lib/libturbulenceModels.so (0x00007f4546d10000)
	libincompressibleTurbulenceModels.so => /opt/openfoam7/platforms/linux64GccDPInt32Opt/lib/libincompressibleTurbulenceModels.so (0x00007f4546853000)
	libcompressibleTurbulenceModels.so => /opt/openfoam7/platforms/linux64GccDPInt32Opt/lib/libcompressibleTurbulenceModels.so (0x00007f45463af000)
	libspecie.so => /opt/openfoam7/platforms/linux64GccDPInt32Opt/lib/libspecie.so (0x00007f4545caf000)
	libfileFormats.so => /opt/openfoam7/platforms/linux64GccDPInt32Opt/lib/libfileFormats.so (0x00007f4545a24000)
	libfiniteVolume.so => /opt/openfoam7/platforms/linux64GccDPInt32Opt/lib/libfiniteVolume.so (0x00007f4543d1a000)
	libmeshTools.so => /opt/openfoam7/platforms/linux64GccDPInt32Opt/lib/libmeshTools.so (0x00007f4543659000)
	libsixDoFRigidBodyMotion.so => /opt/openfoam7/platforms/linux64GccDPInt32Opt/lib/libsixDoFRigidBodyMotion.so (0x00007f45433cd000)
	libstdc++.so.6 => /usr/lib/x86_64-linux-gnu/libstdc++.so.6 (0x00007f454304b000)
	libm.so.6 => /lib/x86_64-linux-gnu/libm.so.6 (0x00007f4542d42000)
	libgcc_s.so.1 => /lib/x86_64-linux-gnu/libgcc_s.so.1 (0x00007f4542b2c000)
	libc.so.6 => /lib/x86_64-linux-gnu/libc.so.6 (0x00007f4542762000)
	libOpenFOAM.so => /opt/openfoam7/platforms/linux64GccDPInt32Opt/lib/libOpenFOAM.so (0x00007f4541bc1000)
	libthermophysicalProperties.so => /opt/openfoam7/platforms/linux64GccDPInt32Opt/lib/libthermophysicalProperties.so (0x00007f45418aa000)
	libPstream.so => /opt/openfoam7/platforms/linux64GccDPInt32Opt/lib/openmpi-system/libPstream.so (0x00007f454169a000)
	libtwoPhaseMixture.so => /opt/openfoam7/platforms/linux64GccDPInt32Opt/lib/libtwoPhaseMixture.so (0x00007f454147a000)
	libsolidThermo.so => /opt/openfoam7/platforms/linux64GccDPInt32Opt/lib/libsolidThermo.so (0x00007f4541198000)
	libsolidSpecie.so => /opt/openfoam7/platforms/linux64GccDPInt32Opt/lib/libsolidSpecie.so (0x00007f4540f6e000)
	libtriSurface.so => /opt/openfoam7/platforms/linux64GccDPInt32Opt/lib/libtriSurface.so (0x00007f4540ccd000)
	libsurfMesh.so => /opt/openfoam7/platforms/linux64GccDPInt32Opt/lib/libsurfMesh.so (0x00007f45409c0000)
	libforces.so => /opt/openfoam7/platforms/linux64GccDPInt32Opt/lib/libforces.so (0x00007f454074e000)
	libdynamicMesh.so => /opt/openfoam7/platforms/linux64GccDPInt32Opt/lib/libdynamicMesh.so (0x00007f453ffe8000)
	/lib64/ld-linux-x86-64.so.2 (0x00007f4547d8a000)
	libz.so.1 => /lib/x86_64-linux-gnu/libz.so.1 (0x00007f453fdce000)
	libpthread.so.0 => /lib/x86_64-linux-gnu/libpthread.so.0 (0x00007f453fbb1000)
	libmpi.so.12 => /usr/lib/libmpi.so.12 (0x00007f453f8db000)
	libreactionThermophysicalModels.so => /opt/openfoam7/platforms/linux64GccDPInt32Opt/lib/libreactionThermophysicalModels.so (0x00007f453ed2c000)
	libextrudeModel.so => /opt/openfoam7/platforms/linux64GccDPInt32Opt/lib/libextrudeModel.so (0x00007f453eb0c000)
	libibverbs.so.1 => /usr/lib/libibverbs.so.1 (0x00007f453e8fd000)
	libopen-rte.so.12 => /usr/lib/libopen-rte.so.12 (0x00007f453e683000)
	libopen-pal.so.13 => /usr/lib/libopen-pal.so.13 (0x00007f453e3e6000)
	libdl.so.2 => /lib/x86_64-linux-gnu/libdl.so.2 (0x00007f453e1e2000)
	libhwloc.so.5 => /usr/lib/x86_64-linux-gnu/libhwloc.so.5 (0x00007f453dfa8000)
	librt.so.1 => /lib/x86_64-linux-gnu/librt.so.1 (0x00007f453dda0000)
	libutil.so.1 => /lib/x86_64-linux-gnu/libutil.so.1 (0x00007f453db9d000)
	libnuma.so.1 => /usr/lib/x86_64-linux-gnu/libnuma.so.1 (0x00007f453d992000)
	libltdl.so.7 => /usr/lib/x86_64-linux-gnu/libltdl.so.7 (0x00007f453d788000)

Now using the above mylinearSpring.so library file when I try to run my floatingObject example it give me error in blockMesh utility

Code:

sreekanth@sreekanth-VirtualBox:~/OpenFOAM/sreekanth-7/run/floatingObject$ !block
blockMesh 
/*---------------------------------------------------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Version:  7
     \\/     M anipulation  |
\*---------------------------------------------------------------------------*/
Build  : 7-1ff648926f77
Exec   : blockMesh
Date   : May 07 2020
Time   : 13:47:33
Host   : "sreekanth-VirtualBox"
PID    : 19301
I/O    : uncollated
Case   : /home/sreekanth/OpenFOAM/sreekanth-7/run/floatingObject
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 10)
allowSystemOperations : Allowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

#0  Foam::error::printStack(Foam::Ostream&) at ??:?
#1  Foam::sigSegv::sigHandler(int) at ??:?
#2  ? in "/lib/x86_64-linux-gnu/libc.so.6"
#3  Foam::Hasher(void const*, unsigned long, unsigned int) at ??:?
#4  Foam::HashTable<Foam::autoPtr<Foam::sixDoFRigidBodyMotionRestraint> (*)(Foam::word const&, Foam::dictionary const&), Foam::word, Foam::string::hash>::set(Foam::word const&, Foam::autoPtr<Foam::sixDoFRigidBodyMotionRestraint> (* const&)(Foam::word const&, Foam::dictionary const&), bool) at ??:?
#5  Foam::sixDoFRigidBodyMotionRestraint::adddictionaryConstructorToTable<Foam::sixDoFRigidBodyMotionRestraints::linearAxialAngularSpring>::adddictionaryConstructorToTable(Foam::word const&) at ??:?
#6  ? at linearAxialAngularSpring.C:?
#7  ? in "/lib64/ld-linux-x86-64.so.2"
#8  ? in "/lib64/ld-linux-x86-64.so.2"
#9  ? in "/lib64/ld-linux-x86-64.so.2"
#10  ? in "/lib64/ld-linux-x86-64.so.2"
#11  ? in "/lib64/ld-linux-x86-64.so.2"
#12  ? in "/lib/x86_64-linux-gnu/libdl.so.2"
#13  ? in "/lib64/ld-linux-x86-64.so.2"
#14  ? in "/lib/x86_64-linux-gnu/libdl.so.2"
#15  dlopen in "/lib/x86_64-linux-gnu/libdl.so.2"
#16  Foam::dlOpen(Foam::fileName const&, bool) at ??:?
#17  Foam::dlLibraryTable::open(Foam::fileName const&, bool) at ??:?
#18  Foam::dlLibraryTable::open(Foam::dictionary const&, Foam::word const&) at ??:?
#19  Foam::Time::Time(Foam::word const&, Foam::argList const&, Foam::word const&, Foam::word const&) at ??:?
#20  ? at ??:?
#21  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#22  ? at ??:?
Segmentation fault (core dumped)

How should I proceed? Any suggestions will be very helpful

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
ATTN ALL: SOLUTON TO UDF COMPILE PROBLEM	Rizwan	Fluent UDF and Scheme Programming	40	March 18, 2018 06:05
How to compile OpenFOAM-1.7.x on CrunchBang linux 10	gwierink	OpenFOAM Installation	0	April 5, 2011 04:38
PV3FoamReader compile error....	PEM_GUY	OpenFOAM Installation	6	April 5, 2010 17:22
Error compile file udf	czfluent	Fluent UDF and Scheme Programming	24	September 26, 2009 13:24
Can someone PLEASE document the development version installation	bernd	OpenFOAM Installation	76	November 14, 2008 21:51

June 21, 2017, 10:16		#4
floquation Senior Member Kevin van As Join Date: Sep 2014 Location: TU Delft, The Netherlands Posts: 252 Rep Power: 20	That's not an error. When a compiler is called, it shows you the entire command. That's what the Makefile does. The three lines you see right there do the following: It finds the dependencies of myIcoFoam, such that it can compile the dependencies before compiling myIcoFoam. You have no dependencies that need compilation, so it then proceeds with: It compiles myIcoFoam.C to Make/.../myIcoFoam.o It links Make/.../myIcoFoam.o, which gives you the executable myIcoFoam in $FOAM_USER_APPBIN If you'd now type "wmake" again, it will show you "myIcoFoam is up to date", which indicates that everything was successful. jiahui_93 and ARTisticCFD like this.

June 22, 2017, 07:04		#5
LThomes Member Join Date: May 2017 Posts: 47 Rep Power: 8	Thank you so much. I'm so used to getting error messages, that I thought it was another one Last edited by LThomes; June 23, 2017 at 06:25.

June 22, 2017, 07:23		#6
akidess Senior Member Anton Kidess Join Date: May 2009 Location: Germany Posts: 1,377 Rep Power: 29	Did you go through all these hoops just to control the time step? Why not use pimpleFoam? __________________ On twitter @akidTwit Spend as much time formulating your questions as you expect people to spend on their answer.

June 23, 2017, 10:29		#9
floquation Senior Member Kevin van As Join Date: Sep 2014 Location: TU Delft, The Netherlands Posts: 252 Rep Power: 20	You are missing Code: #include "createTimeControls.H" next to createTime.H etc. You can easily figure that out by opening a solver that supports this, like pimpleFoam or interFoam.