Using adjustableTimeStep in pisoFoam

odellar · February 26, 2014, 04:33

Hi,

I've found a couple of pages online documenting where to add code in the pisoFoam solver code such that using:

Code:

adjustTimeStep  yes;

maxCo         1;

maxDeltaT    0.5;

in the controlDict file will work (as the pisoFoam doesn't originally support adjustable timestep) - but it's still not particularly clear.

For a start I don't actually know how to get to the solver.c file (which I believe is where I need to add code?)

If anyone could give me some step-by-step instructions of exactly what to do that would be much appreciated.

Thanks, Olie

odellar · February 26, 2014, 09:06

If it helps, I *think* I've put the right code in the right place within pisoFoam.C, thanks to this tutorial: http://www.idurun.com/?p=371

This involved me editing the pisoFoam.C file using

Code:

sudo gedit pisoFoam.C

as it initially told me I don't have permission for some reason. But when I try to compile it using

Code:

wmake

I get this:

Code:

mkdir: cannot create directory `linux64GccDPOpt': Permission denied
/bin/sh: 1: cannot create linux64GccDPOpt/options: Directory nonexistent
make: *** [linux64GccDPOpt/options] Error 2
/opt/openfoam221/wmake/MakefileFiles:40: linux64GccDPOpt/options: No such file or directory
make: *** No rule to make target `linux64GccDPOpt/options'. Stop.
wmake error: file 'Make/linux64GccDPOpt/objectFiles' could not be created in /opt/openfoam221/applications/solvers/incompressible/pisoFoam

Any ideas?

Thanks

sfmoabdu · June 1, 2014, 15:06

it may be too late to reply but let me do it just for anyone will have the same problem.
adding adjustable time step to pisoFoam is not that big issue, just google the tutorial "adding temprature to icofoam" and instead of temprature you will add two headers in the pisoFoam.C (or whatever you will call it)

After:
# include "initContinuityErrs.H"
add this:
# include "readTimeControls.H"

and after:
# include "CourantNo.H"
add this:
# include "setDeltaT.H"

and run wmake.

in system/controlDict add these lines.

adjustTimeStep on;
maxCo 0.3;

and in fvSchemes add linear as following:

interpolationSchemes
{
default linear;
.
.
.
}

Enjoy!!

bentkj · April 13, 2018, 07:48

Quote:

Originally Posted by sfmoabdu

it may be too late to reply but let me do it just for anyone will have the same problem.
adding adjustable time step to pisoFoam is not that big issue, just google the tutorial "adding temprature to icofoam" and instead of temprature you will add two headers in the pisoFoam.C (or whatever you will call it)

After:
# include "initContinuityErrs.H"
add this:
# include "readTimeControls.H"

and after:
# include "CourantNo.H"
add this:
# include "setDeltaT.H"

and run wmake.

in system/controlDict add these lines.

adjustTimeStep on;
maxCo 0.3;

and in fvSchemes add linear as following:

interpolationSchemes
{
default linear;
.
.
.
}

Enjoy!!

Hi, sorry if this is late but after I add the 2 headers and do wmake, i get the errors:

Quote:

Making dependency list for source file my_pisoFoam.C
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 -I/opt/openfoam4/src/TurbulenceModels/turbulenceModels/lnInclude -I/opt/openfoam4/src/TurbulenceModels/incompressible/lnInclude -I/opt/openfoam4/src/transportModels -I/opt/openfoam4/src/transportModels/incompressible/singlePhaseTransportModel -I/opt/openfoam4/src/finiteVolume/lnInclude -I/opt/openfoam4/src/meshTools/lnInclude -I/opt/openfoam4/src/sampling/lnInclude -IlnInclude -I. -I/opt/openfoam4/src/OpenFOAM/lnInclude -I/opt/openfoam4/src/OSspecific/POSIX/lnInclude -fPIC -c my_pisoFoam.C -o Make/linux64GccDPInt32Opt/my_pisoFoam.o
In file included from my_pisoFoam.C:57:0:
/opt/openfoam4/src/finiteVolume/lnInclude/readTimeControls.H: In function ‘int main(int, char**)’:
/opt/openfoam4/src/finiteVolume/lnInclude/readTimeControls.H:32:1: error: ‘adjustTimeStep’ was not declared in this scope
adjustTimeStep =
^
/opt/openfoam4/src/finiteVolume/lnInclude/readTimeControls.H:35:1: error: ‘maxCo’ was not declared in this scope
maxCo =
^
/opt/openfoam4/src/finiteVolume/lnInclude/readTimeControls.H:38:1: error: ‘maxDeltaT’ was not declared in this scope
maxDeltaT =
^
/opt/openfoam4/wmake/rules/General/transform:8: recipe for target 'Make/linux64GccDPInt32Opt/my_pisoFoam.o' failed
make: *** [Make/linux64GccDPInt32Opt/my_pisoFoam.o] Error 1

any idea?

*EDIT: turns out another header file was missing. this is #include "createTimeControls.H"
adding that in solved the problem. Thank you.

Source: Error trying to compile new solver.C

caoxuxiang · November 13, 2018, 21:50

Quote:

Originally Posted by bentkj

Hi, sorry if this is late but after I add the 2 headers and do wmake, i get the errors:

any idea?

*EDIT: turns out another header file was missing. this is #include "createTimeControls.H"
adding that in solved the problem. Thank you.

Source: Error trying to compile new solver.C

i have the same problem now. maybe i can give you some advices. when i found the pisoFoam.c, there no # include "readTimeControls.H" and # include "setDeltaT.H" . i just done the same steps as you, then i got wrong information too.

“the variable was not declared” is tell me that it was not declared before to use it. so i added the #include "createTimeControls.H" after #include "createControl.H", it works well.

p.s of-4.0

clapointe · November 14, 2018, 15:20

For future reference, pimpleFoam can be run essentially as pisoFoam by setting nOuterCorrectors to 1. This alleviates any coding problem. pimpleFoam supports adjustable timestep.

Caelan

amuzeshi · September 30, 2020, 11:14

Quote:

Originally Posted by odellar

Hi,

I've found a couple of pages online documenting where to add code in the pisoFoam solver code such that using:

Code:

adjustTimeStep  yes;

maxCo         1;

maxDeltaT    0.5;

in the controlDict file will work (as the pisoFoam doesn't originally support adjustable timestep) - but it's still not particularly clear.

For a start I don't actually know how to get to the solver.c file (which I believe is where I need to add code?)

If anyone could give me some step-by-step instructions of exactly what to do that would be much appreciated.

Thanks, Olie

Hi,
In order to make it possible to use adjustable time step in pisoFoam, in OpenFOAM v2006, follow these steps:

Code:

mkdir -p  $WM_PROJECT_USER_DIR/solvers/incompressible
cp -r $FOAM_SOLVERS/incompressible/pisoFoam  $WM_PROJECT_USER_DIR/solvers/incompressible/myPisoFoam
cd $WM_PROJECT_USER_DIR/solvers/incompressible/myPisoFoam
mv pisoFoam myPisoFoam
sed -i s/pisoFoam/myPisoFoam/g Make/files

Then add the red lines to myPisoFoam.C:

Code:

...
    #include "createFields.H"								   
    #include "initContinuityErrs.H"							  
    #include "CourantNo.H"							    
    #include "createTimeControls.H"						    
    #include "setInitialDeltaT.H"
...
	Info<< "Time = " << runTime.timeName() << nl << endl;				      

        #include "CourantNo.H"								        
	#include "setDeltaT.H"
...

Now execute:

Code:

wclean
wmake

Make sure that you are in myPisoFoam directory when you issue these two commands.

Ali

sourav90 · February 23, 2021, 12:03

Quote:

Originally Posted by amuzeshi

Hi,
In order to make it possible to use adjustable time step in pisoFoam, in OpenFOAM v2006, follow these steps:

Code:

mkdir -p  $WM_PROJECT_USER_DIR/solvers/incompressible
cp -r $FOAM_SOLVERS/incompressible/pisoFoam  $WM_PROJECT_USER_DIR/solvers/incompressible/myPisoFoam
cd $WM_PROJECT_USER_DIR/solvers/incompressible/myPisoFoam
mv pisoFoam.C myPisoFoam.C
sed -i s/pisoFoam/myPisoFoam/g Make/files

...

Ali

Hi Ali & others, thanks very much for adding this

. I confirm this works with openFOAM version 8 also, but with the small modification of the commands shown in green.

wolfindark · October 14, 2022, 19:19

It gives me following error: Any idea?

Code:

/home/kano/OpenFOAM/OpenFOAM-10/src/finiteVolume/lnInclude/setDeltaT.H: In function ‘int main(int, char**)’:
/home/kano/OpenFOAM/OpenFOAM-10/src/finiteVolume/lnInclude/setDeltaT.H:37:34: error: expected primary-expression before ‘.’ token
   37 |     deltaT = min(deltaT, fvModels.maxDeltaT());
      |                                  ^
make: *** [/home/kano/OpenFOAM/OpenFOAM-10/wmake/rules/General/transform:26: Make/linux64GccDPInt32Debug/mymhdFoam.o] Error 1

amuzeshi · October 26, 2022, 22:00

Quote:

Originally Posted by wolfindark

It gives me following error: Any idea?

Code:

/home/kano/OpenFOAM/OpenFOAM-10/src/finiteVolume/lnInclude/setDeltaT.H: In function ‘int main(int, char**)’:
/home/kano/OpenFOAM/OpenFOAM-10/src/finiteVolume/lnInclude/setDeltaT.H:37:34: error: expected primary-expression before ‘.’ token
   37 |     deltaT = min(deltaT, fvModels.maxDeltaT());
      |                                  ^
make: *** [/home/kano/OpenFOAM/OpenFOAM-10/wmake/rules/General/transform:26: Make/linux64GccDPInt32Debug/mymhdFoam.o] Error 1

Which version of OF?

wolfindark · October 27, 2022, 05:21

Quote:

Originally Posted by amuzeshi

Which version of OF?

OpenFOAM-10

amuzeshi · October 30, 2022, 17:26

Quote:

Originally Posted by wolfindark

OpenFOAM-10

In Make/files, change

Code:

FOAM_APPBIN

to

Code:

FOAM_USER_APPBIN

In myPisoFoam

Code:

mv pisoFoam myPisoFoam

I successfully compiled it, and the turbulent cavity (pisoFoam/RAS) is successfully run when adjustTimeStep is true.

Simone81 · June 12, 2023, 18:57

Hi,

I am trying to implement adjustTimeStep in the solver shallowWaterFoam in openFOAM-10, following the instruction from the previous posts. I do the following

Code:

mkdir -p  $WM_PROJECT_USER_DIR/solvers/incompressible
cp -r $FOAM_SOLVERS/incompressible/shallowWater  $WM_PROJECT_USER_DIR/solvers/incompressible/myShallowWater
cd $WM_PROJECT_USER_DIR/solvers/incompressible/myShallowWater
mv shallowWaterFoam.C myShallowWaterFoam.C
sed -i s/shallowWaterFoam/myShallowWaterFoam/g Make/files

then in the file myShallowWaterFoam.C I have included the files in red:

Code:

#include "fvCFD.H"
#include "pimpleControl.H"
#include "fvModels.H"
#include "fvConstraints.H"
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

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

    #include "setRootCaseLists.H"
    #include "createTime.H"
    #include "createMesh.H"
    #include "createControl.H"
    #include "createFields.H"
							  
    #include "CourantNo.H"							    
    #include "createTimeControls.H"						    
    #include "setInitialDeltaT.H"

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

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

    while (pimple.loop(runTime))
    {
        Info<< "\n Time = " << runTime.timeName() << nl << endl;

        #include "CourantNo.H"
        #include "setDeltaT.H"

Then I compile

Code:

wclean
wmake

and I get the following error:

Code:

/opt/openfoam10/src/finiteVolume/lnInclude/setDeltaT.H: In function ‘int main(int, char**)’:
/opt/openfoam10/src/finiteVolume/lnInclude/setDeltaT.H:37:34: error: expected primary-expression before ‘.’ token
   37 |     deltaT = min(deltaT, fvModels.maxDeltaT());
      |                                  ^
make: *** [/opt/openfoam10/wmake/rules/General/transform:26: Make/linux64GccDPInt32Opt/myShallowWaterFoam.o] Error 1

I also replaced

Code:

FOAM_APPBIN

with

Code:

FOAM_USER_APPBIN

but I get the same error as wolfindark in the post #9. What am I doing wrong?
Thank you!

February 26, 2014, 04:33	Using adjustableTimeStep in pisoFoam	#1
odellar Member Olie Join Date: Oct 2013 Posts: 51 Rep Power: 13	Hi, I've found a couple of pages online documenting where to add code in the pisoFoam solver code such that using: Code: adjustTimeStep yes; maxCo 1; maxDeltaT 0.5; in the controlDict file will work (as the pisoFoam doesn't originally support adjustable timestep) - but it's still not particularly clear. For a start I don't actually know how to get to the solver.c file (which I believe is where I need to add code?) If anyone could give me some step-by-step instructions of exactly what to do that would be much appreciated. Thanks, Olie amuzeshi, Kummi and sourav90 like this.

June 1, 2014, 15:06		#3
sfmoabdu New Member Join Date: Feb 2014 Posts: 9 Rep Power: 12	it may be too late to reply but let me do it just for anyone will have the same problem. adding adjustable time step to pisoFoam is not that big issue, just google the tutorial "adding temprature to icofoam" and instead of temprature you will add two headers in the pisoFoam.C (or whatever you will call it) After: # include "initContinuityErrs.H" add this: # include "readTimeControls.H" and after: # include "CourantNo.H" add this: # include "setDeltaT.H" and run wmake. in system/controlDict add these lines. adjustTimeStep on; maxCo 0.3; and in fvSchemes add linear as following: interpolationSchemes { default linear; . . . } Enjoy!! rajibroy likes this.

November 14, 2018, 15:20		#6
clapointe Senior Member Join Date: Aug 2015 Posts: 494 Rep Power: 15	For future reference, pimpleFoam can be run essentially as pisoFoam by setting nOuterCorrectors to 1. This alleviates any coding problem. pimpleFoam supports adjustable timestep. Caelan utkunun likes this.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Differences in solution method for pisoFoam and buoyantBoussinesqPisoFoam	mchurchf	OpenFOAM	7	August 6, 2023 10:12
why pisoFoam take such a long time to converge?	izna	OpenFOAM Running, Solving & CFD	51	October 25, 2013 03:28
Error DURING pisoFoam execution	Pj.	OpenFOAM Running, Solving & CFD	0	September 14, 2013 05:28
pisoFoam, pimpleFoam - Fluent user's questions	RodriguezFatz	OpenFOAM Running, Solving & CFD	0	September 4, 2013 05:26
pisoFoam compiling error with OF 1.7.1 on MAC OSX	Greg Givogue	OpenFOAM Programming & Development	3	March 4, 2011 18:18