[rolando]

Hi all,
I´m intending to do some turbomachinery calculations.
For that simulations I´m looking for an appropriate outlet boundary condition for the pressure. I´m looking for an alternative to the fixedValue condition.
I know something like a "mean pressure condition" for that kind of problem. Is something like that available in OpenFOAM?
Any other suggestions are welcome too.

Rolando

[hjasak]

Yeah, I know what you mean. I have implemented fixedMeanValue a while back and it behaves much better than "simple" fixed value. You can find it in the dev-version SVN:

fixedMeanValue boundary condition

The setup is straightforward: just add

type fixedMeanValue;
meanValue 3.3;

or similar.

Enjoy,

Hrv

[rolando]

Thanks a lot Hrvoje,
it seems to be what I am looking for.

Rolando

[msrinath80]

Hrv, what exactly is the advantage when we use this 'fixedMeanValue' B/C instead of a constant static pressure at the outlet?

Thanks!

[hjasak]

The advantage of fixedMeanValue boundary condition is a much smaller flow distortion on the boundary. Basically, you get the same behaviour as the fixed pressure outlter, but the local variation next to the boundary around the prescribed mean is picked up from the cells next to it.

If you want to see the effect, try any flow with the vortices leaving the domain through a pressure boundary, a stratified flow or something similar.

I now use fixed mean pressure almost exclusively in "real life" runs.

Enjoy,

Hrv

[msrinath80]

Thanks Hrv. I check the difference in my vortex shedding simulations and get back to you.

[msrinath80]

Hi Hrv,

I added the fixedMeanValue folder from the svn repo onto my OF 1.4.1 installation and rebuilt libfiniteVolume.so. It went without any problems. However, when ever I try to use the B/C, I get this error:

--> FOAM FATAL ERROR :
gradientInternalCoeffs cannot be called for a defaultFvPatchField (actual type fixedMeanValue)
on patch poutlet of field p in file "/home/madhavan/square_cylinder/re1002d_refined_fmvbc/0/p"
You are probably trying to solve for a field with a default boundary condition.

From function defaultFvPatchField<type>::gradientInternalCoeffs( ) const
in file fields/fvPatchFields/basic/default/defaultFvPatchField.C at line 694.

FOAM exiting

Is there something else that I need to build?

[hjasak]

You didn't rebuild it properly or you mis-spelled the name - the code picks up the default patch field instead.

Edit the ~/.OpenFOAM-1.4.1-dev/controlDict and set:

disallowDefaultFvPatchField 1;

If the code fails, it will give you the list of available patch fields. fixedMeanValue should be on the list and it probably isn't. For the record, you should have the following entry in Make/files:

$(derivedFvPatchFields)/fixedMeanValue/fixedMeanValueFvPatchFields.C

Also, check that the file actually compiled - touch it and try again. Then check you are picking up the right library... etc etc.

Hrv

[msrinath80]

Problem solved! Thanks a lot Hrv. I added the entry in Make/files and did a wmake libso finiteVolume and all was well

[mcjicpm2]

Hi
1-I did copy the files in this directory:
/home/sf/OpenFOAM/sf-1.5/applications/fixedMeanValue

2-then I did:

[sf@ls55cb1028 fixedMeanValue]$ wmakeFilesAndOptions
wmakeFilesAndOptions: Creating files
wmakeFilesAndOptions: Creating options

3- this happend:
wmake
SOURCE=fixedMeanValueFvPatchField.C ; g++ -m64 -Dlinux64 -DDP -Wall -Wno-strict-aliasing -Wextra -Wno-unused-parameter -Wold-style-cast -march=opteron -O3 -DNoRepository -ftemplate-depth-40 -I/home/sf/OpenFOAM/OpenFOAM-1.5/src/finiteVolume/lnInclude -IlnInclude -I. -I/home/sf/OpenFOAM/OpenFOAM-1.5/src/OpenFOAM/lnInclude -I/home/sf/OpenFOAM/OpenFOAM-1.5/src/OSspecific/Unix/lnInclude -fPIC -c $SOURCE -o Make/linux64GccDPOpt/fixedMeanValueFvPatchField.o
fixedMeanValueFvPatchField.C:42: error: redefinition of âFoam::fixedMeanValueFvPatchField<Type>::fixedMean ValueFvPatchField(const Foam::fvPatch&, const Foam:imensionedField<Type, Foam::volMesh>&)â
fixedMeanValueFvPatchField.C:42: error: âFoam::fixedMeanValueFvPatchField<Type>::fixedMean ValueFvPatchField(const Foam::fvPatch&, const Foam:imensionedField<Type, Foam::volMesh>&)â previously declared here
fixedMeanValueFvPatchField.C:57: error: redefinition of âFoam::fixedMeanValueFvPatchField<Type>::fixedMean ValueFvPatchField(const Foam::fixedMeanValueFvPatchField<Type>&, const Foam::fvPatch&, const Foam:imensionedField<Type, Foam::volMesh>&, const Foam::fvPatchFieldMapper&)â
fixedMeanValueFvPatchField.C:57: error: âFoam::fixedMeanValueFvPatchField<Type>::fixedMean ValueFvPatchField(const Foam::fixedMeanValueFvPatchField<Type>&, const Foam::fvPatch&, const Foam:imensionedField<Type, Foam::volMesh>&, const Foam::fvPatchFieldMapper&)â previously declared here
fixedMeanValueFvPatchField.C:71: error: redefinition of âFoam::fixedMeanValueFvPatchField<Type>::fixedMean ValueFvPatchField(const Foam::fvPatch&, const Foam:imensionedField<Type, Foam::volMesh>&, const Foam::dictionary&)â
fixedMeanValueFvPatchField.C:71: error: âFoam::fixedMeanValueFvPatchField<Type>::fixedMean ValueFvPatchField(const Foam::fvPatch&, const Foam:imensionedField<Type, Foam::volMesh>&, const Foam::dictionary&)â previously declared here
fixedMeanValueFvPatchField.C:96: error: redefinition of âFoam::fixedMeanValueFvPatchField<Type>::fixedMean ValueFvPatchField(const Foam::fixedMeanValueFvPatchField<Type>&, const Foam:imensionedField<Type, Foam::volMesh>&)â
fixedMeanValueFvPatchField.C:96: error: âFoam::fixedMeanValueFvPatchField<Type>::fixedMean ValueFvPatchField(const Foam::fixedMeanValueFvPatchField<Type>&, const Foam:imensionedField<Type, Foam::volMesh>&)â previously declared here
fixedMeanValueFvPatchField.C:111: error: redefinition of âvoid Foam::fixedMeanValueFvPatchField<Type>::autoMap(co nst Foam::fvPatchFieldMapper&)â
fixedMeanValueFvPatchField.C:111: error: âvirtual void Foam::fixedMeanValueFvPatchField<Type>::autoMap(co nst Foam::fvPatchFieldMapper&)â previously declared here
fixedMeanValueFvPatchField.C:123: error: redefinition of âvoid Foam::fixedMeanValueFvPatchField<Type>::rmap(const Foam::fvPatchField<Type>&, const Foam::labelList&)â
fixedMeanValueFvPatchField.C:123: error: âvirtual void Foam::fixedMeanValueFvPatchField<Type>::rmap(const Foam::fvPatchField<Type>&, const Foam::labelList&)â previously declared here
fixedMeanValueFvPatchField.C:131: error: redefinition of âvoid Foam::fixedMeanValueFvPatchField<Type>::updateCoef fs()â
fixedMeanValueFvPatchField.C:131: error: âvirtual void Foam::fixedMeanValueFvPatchField<Type>::updateCoef fs()â previously declared here
fixedMeanValueFvPatchField.C:155: error: redefinition of âvoid Foam::fixedMeanValueFvPatchField<Type>::write(Foam ::Ostream&) constâ
fixedMeanValueFvPatchField.C:155: error: âvirtual void Foam::fixedMeanValueFvPatchField<Type>::write(Foam ::Ostream&) constâ previously declared here
make: *** [Make/linux64GccDPOpt/fixedMeanValueFvPatchField.o] Error 1


Am I doing something wrong??

can anyone help me?

[heavy_user]

Hi mcjicpm2,

i am getting the exact same error...just for fun I commented every definition but one...and he still brings me the error for just the ONE definition.
I am using OF 1.6. ..

Did you solve the Problem??

regards!

[heavy_user]

Ok I just figured it out...

in files it needs to be:

fixedMeanValueFvPatchFields.C

LIB = $(FOAM_USER_LIBBIN)/libfixedMeanValue

so WITH the "s.C" at the end. The file without the s is the wrong one ..

The options file needs only:

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

LIB_LIBS = \ 
       -lfiniteVolume

in the control dict you need to add:

libs ( "libfixedMeanValue.so" ) ;

[jml]

Hello,

I've seen that the boundary "fixedMeanValue" is available in OpenFOAM 1.5 (/src/finiteVolume/fields/fvPatchFields/derived/fixedMeanValue). However when I try to use it with the next set up

------------------------------
type fixedMeanValue;
meanValue 100000;
------------------------------

the next message appear:

------------------------------
Cannot find 'value' entry on patch salida of field p in file "/... /0/p"
which is required to set the values of the generic patch field.
(Actual type fixedMeanValue)
------------------------------


Why does Openfoam demand 'value'? Is not enough with 'meanValue'?

[siddharameshwara]

hello to all,

Could you please tell me how to add the following code in the controldict file

libs ( "libfixedMeanValue.so" ) ;

[/QUOTE

Thanks

[siddharameshwara]

Hello to all,

Could you please tell me how to calculate the meanvalue in the below example. I am using this for outlet boundary condition for velocity.

type fixedMeanValue;
meanValue 3.3;

Thanks to all.

[mohsen cheraghi]

Hello to all
I'm a new user of OpenFoam and I'm looking for a boundary condition like outflow B.C like Fluent. Help me please.

[chegdan]

Hello All,

I usually go back and forth between the ext and openCFD version of openfoam and I need to use the fixedMeanValue condition in the OpenCFD version. In earlier versions of 2.0.x I was able to compile the code provided above without any changes. However, now that my administrator has spent all this time getting 2.1.x set up on a small cluster...i cannot compile fixedMeanValue (not even on a recently updated version of 2.0.x). My errors are too long to include and are attached in a separate file.

Thoughts?

[falke126]

Hi to all,

i also need the fixedMeanValue bc in the regular OF version 2.1.0 ...
i´ve read that this bc was available in former versions (eg 1.5).

Is there a specific reason, why this kind of bc is´nt available any more?
Eg in cfx the average static pressure bc is very common...

[chegdan]

Originally Posted by falke126

Hi to all,

i also need the fixedMeanValue bc in the regular OF version 2.1.0 ...
i´ve read that this bc was available in former versions (eg 1.5).

Is there a specific reason, why this kind of bc isn't available any more?
Eg in cfx the average static pressure bc is very common...

I didn't answer my own post, but it turns out to be easy enough to compile in 2.1.x. I couldn't get it as a standalone library using wmake libso, but I just put the fixedMeanValue BC in with the other BCs in

$FOAM_SRC/finiteVolume/fields/fvPatchFields/derived

and then added the lines

$(derivedFvPatchFields)/fixedMeanValue/fixedMeanValueFvPatchFields.C

below the line

$(derivedFvPatchFields)/waveSurfacePressure/waveSurfacePressureFvPatchScalarField.C

in the file

$FOAM_SRC/finiteVolume/Make/files

and then an Allwmake in the $FOAM_INST_DIR to recompile everything again and grabbed a coffee. Hope this helps.

[Industrial_CFD]

Hi guys,

I tried to implement fixedMeanValue at the outlet, and I get the followng error:

file: /home/adam/OpenFOAM/adam-2.1.0/run/tutorials/incompressible/pimpleFoam/hvles/0/p::boundaryField::OUTLET from line 30 to line 32.

From function fvPatchField<Type>::New(const fvPatch&, const DimensionedField<Type, volMesh>&, const dictionary&)
in file /opt/openfoam210/src/finiteVolume/lnInclude/fvPatchFieldNew.C at line 135.

FOAM exiting

Obviously even though I re-compiled after putting fixedMeanValue in the BCs it did not take.

Help?

Cheers: Adam