[lg88]

Hello everyone
I am simulating a FSI problem with multiregionsolver.In my case,there are only two regions, solid and fluid.Now I want to use the function setFields to set a quantity ,for example initial volume fraction, in fluid region.
I tried to put the setFieldsDict file in system/fluid floder,then run

setFields -region solid

or

setFields

And it failed.

The following is the details of the file setFieldsDict in my case:
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

defaultFieldValues
(
volScalarFieldValue sigma 2
);

regions
(
boxToCell
{
box (-1.1 -1.1 0) (-1.0 1.1 5);
fieldValues
(
volScalarFieldValue sigma 0.01
);
}

boxToCell
{
box (1.0 -1.1 0) (1.1 1.1 5);
fieldValues
(
volScalarFieldValue sigma 0.01
);
}
);

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

So where should I put the setFieldsDict and how to modified it?

regards!

lg88

[ghas]

Hi Jack,

To do that, follow the following steps:

1- cd $WM_PROJECT_DIR/applications/utilities/preProcessing
2- cp -r setFields $WM_PROJECT_USER_DIR/applications/utilities/preProcessing
3- Rename the directory and the source file name, clean all the dependancies and
> mv setFields mysetFields
> cd mysetFields
> mv setFields.C mysetFields.C
> wclean

5- Add the region option to mysetFields.C file by

# include "addRegionOption.H"

6- Replace the line

# include "createMesh.H"

by:

# include "createNamedPolyMesh.H"

7- Open Make/files and modify it as follows:
mysetFields.C
EXE = $(FOAM_USER_APPBIN)/mysetFields

8- Compile the utility by wmake

9- Now your utility is ready to be ued:

> mysetFields -region solid



Best regards

Ghassan

[lg88]

Hi Ghassan

I have done as you said and it works correctly.Thank you very much!
By the way,do you know how to convert the result data of different regions to tecplot360?
I use the following command,but the converted data can not work in tecplot.

foamToTecplot360 -region fluid
foamToTecplot360 -region solid

regards!

lg88

[ghas]

Hi jack,

The foamTotecplot supports the multi-region option and I think that there is another proplem in your run. what's the error message ?

Best regards,

Ghassan

[lg88]

Hi Ghassan
I have found my problem and it can run now.Thank you all the same!

regards!

jack

[karlvirgil]

For OpenFOAM-2.1.x the setFields can be made multiregional if the following changes are made to setFields.C

$ )git diff setFields.C

diff --git a/applications/utilities/preProcessing/setFields/setFields.C b/applications/utilities/preProcessing/setFields/setFields.C
index 0930468..d9a53ee 100644
--- a/applications/utilities/preProcessing/setFields/setFields.C
+++ b/applications/utilities/preProcessing/setFields/setFields.C
@@ -331,9 +331,10 @@ public:

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

[aujamal20]

Dear
I am using OF 2.1.0 and I am trying to modify setFields utility to work on multiRegion and I have followed the same steps which are given but I am facing error

SOURCE=mysetFields.C ; g++ -m64 -Dlinux64 -DWM_DP -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3 -DNoRepository -ftemplate-depth-100 -I/opt/OpenFOAM/OpenFOAM-2.1.0/src/finiteVolume/lnInclude -I/opt/OpenFOAM/OpenFOAM-2.1.0/src/meshTools/lnInclude -IlnInclude -I. -I/opt/OpenFOAM/OpenFOAM-2.1.0/src/OpenFOAM/lnInclude -I/opt/OpenFOAM/OpenFOAM-2.1.0/src/OSspecific/POSIX/lnInclude -fPIC -c $SOURCE -o Make/linux64GccDPOpt/mysetFields.o
In file included from mysetFields.C:37:0:
/opt/OpenFOAM/OpenFOAM-2.1.0/src/OpenFOAM/lnInclude/addRegionOption.H:6:5: error: expected constructor, destructor, or type conversion before '(' token
mysetFields.C: In function 'int main(int, char**)':
mysetFields.C:343:6: error: 'Get' was not declared in this scope
mysetFields.C:343:10: error: expected ';' before 'times'
mysetFields.C:369:62: error: no matching function for call to 'setCellField::iNew::iNew(Foam:olyMesh&, Foam::labelList)'
mysetFields.C:369:62: note: candidates are:
mysetFields.C:133:9: note: setCellField::iNew::iNew(const Foam::fvMesh&, const labelList&)
mysetFields.C:133:9: note: no known conversion for argument 1 from 'Foam:olyMesh' to 'const Foam::fvMesh&'
mysetFields.C:126:11: note: setCellField::iNew::iNew(const setCellField::iNew&)
mysetFields.C:126:11: note: candidate expects 1 argument, 2 provided
mysetFields.C:404:63: error: no matching function for call to 'setCellField::iNew::iNew(Foam:olyMesh&, Foam::List<int>)'
mysetFields.C:404:63: note: candidates are:
mysetFields.C:133:9: note: setCellField::iNew::iNew(const Foam::fvMesh&, const labelList&)
mysetFields.C:133:9: note: no known conversion for argument 1 from 'Foam:olyMesh' to 'const Foam::fvMesh&'
mysetFields.C:126:11: note: setCellField::iNew::iNew(const setCellField::iNew&)
mysetFields.C:126:11: note: candidate expects 1 argument, 2 provided
mysetFields.C:425:63: error: no matching function for call to 'setFaceField::iNew::iNew(Foam:olyMesh&, Foam::List<int>)'
mysetFields.C:425:63: note: candidates are:
mysetFields.C:295:9: note: setFaceField::iNew::iNew(const Foam::fvMesh&, const labelList&)
mysetFields.C:295:9: note: no known conversion for argument 1 from 'Foam:olyMesh' to 'const Foam::fvMesh&'
mysetFields.C:288:11: note: setFaceField::iNew::iNew(const setFaceField::iNew&)
mysetFields.C:288:11: note: candidate expects 1 argument, 2 provided
make: *** [Make/linux64GccDPOpt/mysetFields.o] Error 1

Help me out to fix this error.

Regards,
Jamal

[ghas]

Originally Posted by aujamal20

Dear
I am using OF 2.1.0 and I am trying to modify setFields utility to work on multiRegion and I have followed the same steps which are given but I am facing error



Help me out to fix this error.

Regards,
Jamal

Hi Jamal,

I think that you uncommented "// Get times list" by the ommision of "//" . You can find the modified code of setFields in the attached file.

Best Regards,
Ghassan

[aujamal20]

Dear ghas

So nice of you, it helped me to solve the problem...

Thanks

[Ben UWIHANGANYE]

Originally Posted by ghas

Hi Jack,

To do that, follow the following steps:

1- cd $WM_PROJECT_DIR/applications/utilities/preProcessing
2- cp -r setFields $WM_PROJECT_USER_DIR/applications/utilities/preProcessing
3- Rename the directory and the source file name, clean all the dependancies and
> mv setFields mysetFields
> cd mysetFields
> mv setFields.C mysetFields.C
> wclean

5- Add the region option to mysetFields.C file by

# include "addRegionOption.H"

6- Replace the line

# include "createMesh.H"

by:

# include "createNamedPolyMesh.H"

7- Open Make/files and modify it as follows:
mysetFields.C
EXE = $(FOAM_USER_APPBIN)/mysetFields

8- Compile the utility by wmake

9- Now your utility is ready to be ued:

> mysetFields -region solid



Best regards

Ghassan

I was trying the same procedure but failed, the following is the error msg i got. May you help please.



/opt/openfoam4/applications/utilities/preProcessing/mysetFields
mkdir: cannot create directory ‘/opt/openfoam4/platforms/linux64GccDPInt32Opt/applications’: Permission denied
/bin/sh: 1: cannot create /opt/openfoam4/platforms/linux64GccDPInt32Opt/applications/utilities/preProcessing/mysetFields/options: Directory nonexistent
make: *** No rule to make target '/opt/openfoam4/platforms/linux64GccDPInt32Opt/applications/utilities/preProcessing/mysetFields/options'. Stop.
/bin/sh: 1: cannot create /opt/openfoam4/platforms/linux64GccDPInt32Opt/applications/utilities/preProcessing/mysetFields/options: Directory nonexistent
make: *** No rule to make target '/opt/openfoam4/platforms/linux64GccDPInt32Opt/applications/utilities/preProcessing/mysetFields/options', needed by 'all'. Stop.
wmake error: file '/opt/openfoam4/platforms/linux64GccDPInt32Opt/applications/utilities/preProcessing/mysetFields/sourceFiles' could not be created in /opt/openfoam4/applications/utilities/preProcessing/mysetFields




Regard!

[ghas]

You need to modify the location of the binary executable file mysetFields(or run wmake as a super user). To do so, you can just repalce the last line of Make/files:



EXE = $(FOAM_APPBIN)/mysetFields



by



EXE = $(FOAM_USER_APPBIN)/mysetFields




regards

[Ben UWIHANGANYE]

Thank you for quick feedback.




That one i did as it has been instructed :

May be that of running it as super user is what i didn't. How is it done(run as super user.)?






Regard!

[ghas]

> sudo su
> enter your password
> source /opt/openfoam4/etc/bashrc
> cd /opt/openfoam4/applications/utilities/preProcessing/mysetFields
> wmake


Regards

[Ben UWIHANGANYE]

Originally Posted by lg88

Hello everyone
I am simulating a FSI problem with multiregionsolver.In my case,there are only two regions, solid and fluid.Now I want to use the function setFields to set a quantity ,for example initial volume fraction, in fluid region.
I tried to put the setFieldsDict file in system/fluid floder,then run

setFields -region solid

or

setFields

And it failed.

The following is the details of the file setFieldsDict in my case:
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

defaultFieldValues
(
volScalarFieldValue sigma 2
);

regions
(
boxToCell
{
box (-1.1 -1.1 0) (-1.0 1.1 5);
fieldValues
(
volScalarFieldValue sigma 0.01
);
}

boxToCell
{
box (1.0 -1.1 0) (1.1 1.1 5);
fieldValues
(
volScalarFieldValue sigma 0.01
);
}
);

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

So where should I put the setFieldsDict and how to modified it?

regards!

lg88

Hello,

Did you succeed with this case, may you share the setup and results you got?

is it possible to replace the boxTocell with a cylinder?


Thank you!

[Ben UWIHANGANYE]

Hello Foamers,

I would like to ask how the modified setFieldsDict is used in FSI simulation.

Indeed, I want to simulate flow over a cylinder(stationary and oscillating). I have used toposetDict to map that cylinder in fluid Cartesian domain.

Let: eta=1 solid region, eta=0 fluid region.
Then i have a c++ code that gives me a value of eta each time step. The eta's value alternate from 0 to 1 and from 1 to 0. C++ code prints eta values in .dat format.

I am asking if it is possible to use setFieldsDict to move (oscillating motion) that cylinder as eta changes.

what should be my code looking like?

I will be happy to hear from you!

Regard!

[vivek05]

Hi
i am facing problem in setFields usage. simulating spray using interFoam solver .when i run setFields command it doesnt make any changes in 0/alpha.water folder. i am using boxTocell (0 0.1 -1) (0.06 0.1 1) these dimension are my fuel inlet coordinates.

[Brodenson]

Originally Posted by ghas

Hi Jack,

To do that, follow the following steps:

1- cd $WM_PROJECT_DIR/applications/utilities/preProcessing
2- cp -r setFields $WM_PROJECT_USER_DIR/applications/utilities/preProcessing
3- Rename the directory and the source file name, clean all the dependancies and
> mv setFields mysetFields
> cd mysetFields
> mv setFields.C mysetFields.C
> wclean

5- Add the region option to mysetFields.C file by

# include "addRegionOption.H"

6- Replace the line

# include "createMesh.H"

by:

# include "createNamedPolyMesh.H"

7- Open Make/files and modify it as follows:
mysetFields.C
EXE = $(FOAM_USER_APPBIN)/mysetFields

8- Compile the utility by wmake

9- Now your utility is ready to be ued:

> mysetFields -region solid



Best regards

Ghassan

I tried to use this in OF ESI 2112 and it didn't work but I discovered that using only setFields -region <your region name> works fine!

Greetings!