|
[Sponsors] |
October 23, 2007, 09:42 |
Hi all,
I´m intending to do s
|
#1 |
Member
Rolando Maier
Join Date: Mar 2009
Posts: 89
Rep Power: 17 |
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 |
|
October 23, 2007, 09:53 |
Yeah, I know what you mean. I
|
#2 |
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,907
Rep Power: 33 |
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
__________________
Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk |
|
October 23, 2007, 10:07 |
Thanks a lot Hrvoje,
it seems
|
#3 |
Member
Rolando Maier
Join Date: Mar 2009
Posts: 89
Rep Power: 17 |
Thanks a lot Hrvoje,
it seems to be what I am looking for. Rolando |
|
December 14, 2007, 15:22 |
Hrv, what exactly is the advan
|
#4 |
Senior Member
Srinath Madhavan (a.k.a pUl|)
Join Date: Mar 2009
Location: Edmonton, AB, Canada
Posts: 703
Rep Power: 21 |
Hrv, what exactly is the advantage when we use this 'fixedMeanValue' B/C instead of a constant static pressure at the outlet?
Thanks! |
|
December 15, 2007, 11:13 |
The advantage of fixedMeanValu
|
#5 |
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,907
Rep Power: 33 |
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
__________________
Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk |
|
December 15, 2007, 16:37 |
Thanks Hrv. I check the differ
|
#6 |
Senior Member
Srinath Madhavan (a.k.a pUl|)
Join Date: Mar 2009
Location: Edmonton, AB, Canada
Posts: 703
Rep Power: 21 |
Thanks Hrv. I check the difference in my vortex shedding simulations and get back to you.
|
|
December 20, 2007, 17:04 |
Hi Hrv,
I added the fixedMe
|
#7 |
Senior Member
Srinath Madhavan (a.k.a pUl|)
Join Date: Mar 2009
Location: Edmonton, AB, Canada
Posts: 703
Rep Power: 21 |
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? |
|
December 20, 2007, 17:29 |
You didn't rebuild it properly
|
#8 |
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,907
Rep Power: 33 |
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: $(derivedFvPatchFields)/fixedMeanValue/fixedMeanValueFvPatchFields.C Also, check that the file actually compiled - touch it and try again. Then check you are picking up the right library... etc etc. Hrv
__________________
Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk |
|
December 20, 2007, 17:52 |
Problem solved! Thanks a lot H
|
#9 |
Senior Member
Srinath Madhavan (a.k.a pUl|)
Join Date: Mar 2009
Location: Edmonton, AB, Canada
Posts: 703
Rep Power: 21 |
Problem solved! Thanks a lot Hrv. I added the entry in Make/files and did a wmake libso finiteVolume and all was well
|
|
May 11, 2009, 09:57 |
Question
|
#10 |
New Member
parham momeni
Join Date: Mar 2009
Location: glasgow, uk
Posts: 25
Rep Power: 16 |
Hi
1-I did copy the files in this directory: /home/sf/OpenFOAM/sf-1.5/applications/fixedMeanValue 2-then I did: [sf@ls55cb1028 fixedMeanValue]$ 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? |
|
May 20, 2010, 13:06 |
|
#11 |
Senior Member
Join Date: Dec 2009
Posts: 112
Rep Power: 17 |
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! |
|
May 20, 2010, 14:26 |
|
#12 |
Senior Member
Join Date: Dec 2009
Posts: 112
Rep Power: 17 |
Ok I just figured it out...
in files it needs to be: Code:
fixedMeanValueFvPatchFields.C LIB = $(FOAM_USER_LIBBIN)/libfixedMeanValue The options file needs only: Code:
EXE_INC = \ -I$(LIB_SRC)/finiteVolume/lnInclude LIB_LIBS = \ -lfiniteVolume Code:
libs ( "libfixedMeanValue.so" ) ; |
|
October 7, 2010, 13:19 |
|
#13 |
New Member
Jml
Join Date: Mar 2009
Posts: 23
Rep Power: 17 |
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'? |
|
November 30, 2010, 06:32 |
fixedMeanvalue adding code
|
#14 |
Member
Join Date: Sep 2010
Posts: 36
Rep Power: 17 |
hello to all,
Could you please tell me how to add the following code in the controldict file Code:
libs ( "libfixedMeanValue.so" ) ; Thanks |
|
November 30, 2010, 10:30 |
how to calculate fixedMeanvalue
|
#15 |
Member
Join Date: Sep 2010
Posts: 36
Rep Power: 17 |
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. |
|
March 6, 2011, 07:55 |
Outflow boundary condition
|
#16 |
New Member
mohsen cheraghi
Join Date: Jun 2010
Location: Switzerland
Posts: 28
Rep Power: 16 |
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. |
|
January 12, 2012, 19:40 |
fixedMeanValue in 2.1.x?
|
#17 |
Senior Member
Daniel P. Combest
Join Date: Mar 2009
Location: St. Louis, USA
Posts: 621
Rep Power: 0 |
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? |
|
April 25, 2012, 17:50 |
|
#18 |
New Member
Hannes
Join Date: Oct 2011
Posts: 19
Rep Power: 15 |
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... |
|
April 25, 2012, 18:22 |
|
#19 | |
Senior Member
Daniel P. Combest
Join Date: Mar 2009
Location: St. Louis, USA
Posts: 621
Rep Power: 0 |
Quote:
Code:
$FOAM_SRC/finiteVolume/fields/fvPatchFields/derived Code:
$(derivedFvPatchFields)/fixedMeanValue/fixedMeanValueFvPatchFields.C Code:
$(derivedFvPatchFields)/waveSurfacePressure/waveSurfacePressureFvPatchScalarField.C Code:
$FOAM_SRC/finiteVolume/Make/files |
||
February 2, 2013, 13:06 |
Help fixedMeanValue Outlet
|
#20 |
Member
Anonymous
Join Date: Jan 2012
Location: Canada
Posts: 65
Rep Power: 14 |
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 |
|
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Outlet pressure boundary condition | adamsview | OpenFOAM Running, Solving & CFD | 2 | November 7, 2011 14:07 |
pressure outlet boundary condition | Sastry | FLUENT | 4 | February 19, 2011 02:33 |
Pressure outlet boundary condition | jubs | FLUENT | 0 | February 8, 2007 01:27 |
Pressure outlet boundary condition | Rizwan | FLUENT | 1 | March 6, 2006 08:07 |
Pressure outlet condition? | David | FLUENT | 3 | March 19, 2004 05:40 |