CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

Parabolic inlet velocity profile

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree5Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   December 11, 2007, 17:14
Default If you are interested, I wrote
  #61
Senior Member
 
Håkan Nilsson
Join Date: Mar 2009
Location: Gothenburg, Sweden
Posts: 193
Rep Power: 8
hani is on a distinguished road
If you are interested, I wrote a small tutorial on how to add the parabolic velocity boundary condition from OpenFOAM-1.4.1-dev into the distribution by OpenCFD by using dlopen.

Here you have the temporary link (I plan to move it in the future). Tell me if you find it useful or not.

http://openfoamwiki.net/index.php/Tutorials#How_to_implement_a_new_boundary_cond ition_.28OF-1.4.1.29

Håkan.
hani is offline   Reply With Quote

Old   December 11, 2007, 17:32
Default Håkan, Does the parabolic inle
  #62
Senior Member
 
Srinath Madhavan (a.k.a pUl|)
Join Date: Mar 2009
Location: Edmonton, AB, Canada
Posts: 698
Rep Power: 12
msrinath80 is on a distinguished road
Håkan, Does the parabolic inlet B/C (explained nicely in the wiki) work for both 3D and 2D cases?
msrinath80 is offline   Reply With Quote

Old   December 11, 2007, 18:32
Default Hi Håkan, Thanks for the li
  #63
New Member
 
inddzen
Join Date: Mar 2009
Posts: 4
Rep Power: 8
inddzen is on a distinguished road
Hi Håkan,

Thanks for the link, great stuff and well explained.

I did exactly as you wrote, and I made a simple test case on icoFoam which apparently worked, but I need to view the results to be sure

The problem is that I got this error while trying to run paraFOAM!

[lhassa@localhost ~]$ paraFoam $FOAM_RUN/tutorials/icoFoam poiseuille_2D
--> FOAM Warning :
From function dlLibraryTable::open(const fileName& functionLibName)
in file db/dlLibraryTable/dlLibraryTable.C at line 79
could not load /home/lhassa/OpenFOAM/lhassa-1.4.1/lib/linux64GccDPOpt/libParaBC.so: undefined symbol: _ZN4Foam6VectorIdE8typeNameE


--> FOAM FATAL IO ERROR :
Cannot find 'value' entry on patch inlet of field U in file "/home/lhassa/OpenFOAM/lhassa-1.4.1/run/tutorials/icoFoam/poiseuille_2D/0/U"
which is required to set the values of the default patch field.
(Actual type parabolicVelocity)

Please add the 'value' entry to the write function of the user-defined boundary-condition
or link the boundary-condition into libfoamUtil.so

file: /home/lhassa/OpenFOAM/lhassa-1.4.1/run/tutorials/icoFoam/poiseuille_2D/0/U::inle t from line 42 to line 45.

From function defaultFvPatchField<type>::defaultFvPatchField(con st fvPatch&, const Field<type>&, const dictionary&)
in file fields/fvPatchFields/basic/default/defaultFvPatchField.C at line 77.

FOAM exiting

Any idea???
inddzen is offline   Reply With Quote

Old   December 11, 2007, 19:27
Default inddzen, I remember seeing a s
  #64
Senior Member
 
Srinath Madhavan (a.k.a pUl|)
Join Date: Mar 2009
Location: Edmonton, AB, Canada
Posts: 698
Rep Power: 12
msrinath80 is on a distinguished road
inddzen, I remember seeing a similar error in this forum. The simplest fix is to comment out the libs ("libmyBCs.so"); section in controlDict and then start paraFoam. This should let you visualize the velocity field without problems. The entry in controlDict is required only when running icoFoam.
msrinath80 is offline   Reply With Quote

Old   December 12, 2007, 02:54
Default inddzen, paraFoam does not rec
  #65
Senior Member
 
Håkan Nilsson
Join Date: Mar 2009
Location: Gothenburg, Sweden
Posts: 193
Rep Power: 8
hani is on a distinguished road
inddzen, paraFoam does not recognize your new boundary condition. I don't know how to do that at the moment. However, if you run your case until you write out a new time directory you can see that there is also a 'value' entry in the boundary condition. paraFoam will open the boundary condition as a default patch field and apply that value. There is however still a problem: you must make sure that there is a 'value' entry for the boundary condition also for the '0' directory. Add the following to your boundary condition:

value uniform (0 0 0);

Then of course the visualization of the boundary condition at time 0 will show no velocity at the inlet. Another way to do this is simply to remove the '0' directory when you have any new time directory. In any way, you should now be able to see the boundary condition in paraFoam for times > 0.

Srinath, This parabolic boundary condition should work also for 3D cases with 2D inlets, but the profile is still a 1D function in a cartesian coordinate system. Have a look at the source code.

Håkan.
hani is offline   Reply With Quote

Old   February 22, 2008, 07:01
Default Hi everybody! Håkan, your tut
  #66
New Member
 
Marzio Lettich
Join Date: Mar 2009
Posts: 14
Rep Power: 8
marziolettich is on a distinguished road
Hi everybody!
Håkan, your tutorial is simply great and has proved very useful (not only for the parabolic profile, but especially for future personal BC implementation), so I wanted to thank you (and every people that provide useful modifications). Can you explain the syntax in the line libs("lib_name") ? OF searches directly in $FOAM_USER_LIBBIN? It would work equally well if the library were in another directory?
I apologize in advance if my question is obvious...
thank you again and bye,
Marzio
marziolettich is offline   Reply With Quote

Old   February 24, 2008, 04:38
Default Hi Marzio, Yes, OF searches
  #67
Senior Member
 
Håkan Nilsson
Join Date: Mar 2009
Location: Gothenburg, Sweden
Posts: 193
Rep Power: 8
hani is on a distinguished road
Hi Marzio,

Yes, OF searches for the library in $FOAM_USER_LIBBIN. Without testing, I think that you should be able to locate your library anywhere as long as you add that path to your $LD_LIBRARY_PATH. Try it yourself.

Håkan.
hani is offline   Reply With Quote

Old   February 25, 2008, 04:58
Default Thanks Håkan! It may seems str
  #68
New Member
 
Marzio Lettich
Join Date: Mar 2009
Posts: 14
Rep Power: 8
marziolettich is on a distinguished road
Thanks Håkan! It may seems strange to those familiar with OF but these details are sometimes the part in which we newbies get stuck!
Now it's my turn to give a little contribution: the source file "parabolicVelocityFvPatchVectorField.C" (whose link is in your tutorial) contains a little error in the row in which the patch coordinate is computed. As it is, it gives a local coordinate that varies from -0.5 to +0.5 but we obviously need a -1 to +1 coordinate, so it is sufficient to multiply coord by two.
Well, now I get back to work (I have to make some little modification to obtain a parabolic profile only on a part of the patch, but it shouldn't be a difficult task!)
Thanks again for your answer and bye,
Marzio
marziolettich is offline   Reply With Quote

Old   February 28, 2008, 15:26
Default Hi, Is there a way to modif
  #69
New Member
 
J. T.
Join Date: Mar 2009
Posts: 12
Rep Power: 8
cpplabs is on a distinguished road
Hi,
Is there a way to modify the boundary condition inside the application? For example, I have a function to calculate the velocity profile of non-Newtonian flow at the inlet, and need to set the values on the inlet patch. How to directly modify the values on a patch ?
Thanks!
cpplabs is offline   Reply With Quote

Old   February 28, 2008, 18:32
Default Hi J.T! You might want to l
  #70
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,914
Rep Power: 40
gschaider will become famous soon enoughgschaider will become famous soon enough
Hi J.T!

You might want to look for the dicussion on the timeVaryingMappedFixedValue-boundary condition. It might do what you want to do (but I havn't used it myself yet). In the worst case it might be a good starting point for your own developments

Bernhard
__________________
Note: I don't use "Friend"-feature on this forum out of principle. Ah. And by the way: I'm not on Facebook either. So don't be offended if I don't accept your invitation/friend request
gschaider is offline   Reply With Quote

Old   February 29, 2008, 07:51
Default Hello, I have a question ab
  #71
kar
Senior Member
 
Kārlis Repsons
Join Date: Mar 2009
Location: Latvia
Posts: 111
Rep Power: 8
kar is on a distinguished road
Hello,

I have a question about parabolicVelocityFvPatchVectorField and similar patch fields - they have one or two virtual functions:

virtual void updateCoeffs();
virtual void evaluate();

I observe, for field T updateCoeffs is called 3 times (I have only 2 relevant boundaries) before solving and evaluate after.

My question is: what and when do those function calls?
kar is offline   Reply With Quote

Old   March 22, 2008, 12:45
Default Hello, I've been reading th
  #72
leo
New Member
 
Lars Olson
Join Date: Mar 2009
Location: Milwaukee, Wisconsin, US
Posts: 1
Rep Power: 0
leo is on a distinguished road
Hello,

I've been reading this discussion board for some time and wish to sincerely thank all who contributed! Also great thanks to Hrv and others for this awesome open source CFD code.

I've implemented a variant of the parabolic velocity BC from Hrv and others. It works great for a simple cylindrical steady laminar flow problem using simplefoam.

My problem comes in when I try to implement it with an input with several blocks in it (10 to be exact). I get the following error message:


Starting time loop

Time = 1



--> FOAM FATAL ERROR :
gradientInternalCoeffs cannot be called for a defaultFvPatchField (actual type parabolicVelocity)
on patch inlet1 of field U in file "/home/leo/bif032208a/0/U"
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

I tried it where I declared just one input with 10 blocks or as 10 separate blocks in blockMeshDict and /0/U and /0/p. Same error.

I'm sort of committed to this 10 block idea, so I'm stuck and need some guidance.

I'm an absolute rookie on C++ (be gentle). The relevant member function of my parab....C file follows:

void parabolicVelocityFvPatchVectorField::updateCoeffs( )
{

const vectorField& c = patch().Cf();
scalarField cy = c.component(vector::Y);
scalarField cx = c.component(vector::X);
scalarField coord = (cx*cx+cy*cy)/0.0001;
vectorField::operator=(n_*maxValue_*(1.0 - (coord)));
}

(my radius is 0.01)


If anyone could help me, I'd be very grateful. If you need more stuff, too, I can pack it up and send it.

Thanks,

LEO
leo is offline   Reply With Quote

Old   March 25, 2008, 06:22
Default hi all, i am very new to Open
  #73
Member
 
davey david
Join Date: Mar 2009
Posts: 54
Rep Power: 8
suredross is on a distinguished road
hi all,
i am very new to OpenFoam and needs an explanation on how to get the cell expansion ratios(simple grading)correct in icoFoam?i am working on a case with 2 inlets and one outlet with a no. of cells approx. 100,000.it is 2-d.
thanks in advance

david
suredross is offline   Reply With Quote

Old   March 25, 2008, 18:17
Default Read this --> http://www.openc
  #74
Senior Member
 
Srinath Madhavan (a.k.a pUl|)
Join Date: Mar 2009
Location: Edmonton, AB, Canada
Posts: 698
Rep Power: 12
msrinath80 is on a distinguished road
Read this --> http://www.opencfd.co.uk/openfoam/do...-1680006.3.1.3

and then tell us what you don't understand?
msrinath80 is offline   Reply With Quote

Old   June 5, 2008, 07:15
Default I try to wmake parabolicVelo
  #75
Member
 
Ivan Lau
Join Date: Mar 2009
Location: Hong Kong
Posts: 56
Rep Power: 8
ivanwhlau is on a distinguished road
I try to wmake parabolicVelo
city any times, but I keep getting error....
Would someone give me a complete zip files?
In fact, I am trying to make a nonuniform wind profile, is this program the good one to modify?
Thanks a lot.

Making dependency list for source file parabolicVelocityFvPatchVectorField.C
SOURCE=parabolicVelocityFvPatchVectorField.C ; g++ -m32 -Dlinux -DDP -Wall -Wno
-strict-aliasing -Wextra -Wno-unused-parameter -Wold-style-cast -O3 -DNoReposit
ory -ftemplate-depth-40 -I/home/ivanlau/OpenFOAM/OpenFOAM-1.4.1/src/finiteVolume
/lnInclude -IlnInclude -I. -I/home/ivanlau/OpenFOAM/OpenFOAM-1.4.1/src/OpenFOAM/
lnInclude -fPIC -pthread -c $SOURCE -o Make/linuxGccDPOpt/parabolicVelocityFvP
atchVectorField.o
parabolicVelocityFvPatchVectorField.C: In constructor 'Foam::parabolicVelocityFv
PatchVectorField::parabolicVelocityFvPatchVectorFi eld(const Foam::fvPatch&, cons
t Foam::vectorField&)':
parabolicVelocityFvPatchVectorField.C:49: error: no matching function for call t
o 'Foam::fixedValueFvPatchField<foam::vector<double> >::fixedValueFvPatchField(c
onst Foam::fvPatch&, const Foam::Field<foam::vector<double> >&)'
/home/ivanlau/OpenFOAM/OpenFOAM-1.4.1/src/finiteVolume/lnInclude/fixedValueFvPat
chField.C:87: note: candidates are: Foam::fixedValueFvPatchField<type>::fixedVal
ueFvPatchField(const Foam::fixedValueFvPatchField<type>&, const Foam::Dimensione
dField<type,>&) [with Type = Foam::Vector<double>]
/home/ivanlau/OpenFOAM/OpenFOAM-1.4.1/src/finiteVolume/lnInclude/fixedValueFvPat
chField.C:76: note: Foam::fixedValueFvPatchField<type>::fixedVal
ueFvPatchField(const Foam::fixedValueFvPatchField<type>&) [with Type = Foam::Vec
tor<double>]
/home/ivanlau/OpenFOAM/OpenFOAM-1.4.1/src/finiteVolume/lnInclude/fixedValueFvPat
chField.C:66: note: Foam::fixedValueFvPatchField<type>::fixedVal
ueFvPatchField(const Foam::fixedValueFvPatchField<type>&, const Foam::fvPatch&,
const Foam::DimensionedField<type,>&, const Foam::fvPatchFieldMapp
er&) [with Type = Foam::Vector<double>]
/home/ivanlau/OpenFOAM/OpenFOAM-1.4.1/src/finiteVolume/lnInclude/fixedValueFvPat
chField.C:53: note: Foam::fixedValueFvPatchField<type>::fixedVal
ueFvPatchField(const Foam::fvPatch&, const Foam::DimensionedField<Type, Foam::vo
lMesh>&, const Foam::dictionary&) [with Type = Foam::Vector<double>]
/home/ivanlau/OpenFOAM/OpenFOAM-1.4.1/src/finiteVolume/lnInclude/fixedValueFvPat
chField.C:41: note: Foam::fixedValueFvPatchField<type>::fixedVal
ueFvPatchField(const Foam::fvPatch&, const Foam::DimensionedField<Type, Foam::vo
lMesh>&) [with Type = Foam::Vector<double>]
parabolicVelocityFvPatchVectorField.C: In constructor 'Foam::parabolicVelocityFv
PatchVectorField::parabolicVelocityFvPatchVectorFi eld(const Foam::parabolicVeloc
ityFvPatchVectorField&, const Foam::fvPatch&, const Foam::vectorField&, const Fo
am::fvPatchFieldMapper&)':
parabolicVelocityFvPatchVectorField.C:64: error: no matching function for call t
o 'Foam::fixedValueFvPatchField<foam::vector<double> >::fixedValueFvPatchField(c
onst Foam::parabolicVelocityFvPatchVectorField&, const Foam::fvPatch&, const Foa
m::Field<foam::vector<double> >&, const Foam::fvPatchFieldMapper&)'
/home/ivanlau/OpenFOAM/OpenFOAM-1.4.1/src/finiteVolume/lnInclude/fixedValueFvPat
chField.C:87: note: candidates are: Foam::fixedValueFvPatchField<type>::fixedVal
ueFvPatchField(const Foam::fixedValueFvPatchField<type>&, const Foam::Dimensione
dField<type,>&) [with Type = Foam::Vector<double>]
/home/ivanlau/OpenFOAM/OpenFOAM-1.4.1/src/finiteVolume/lnInclude/fixedValueFvPat
chField.C:76: note: Foam::fixedValueFvPatchField<type>::fixedVal
ueFvPatchField(const Foam::fixedValueFvPatchField<type>&) [with Type = Foam::Vec
tor<double>]
/home/ivanlau/OpenFOAM/OpenFOAM-1.4.1/src/finiteVolume/lnInclude/fixedValueFvPat
chField.C:66: note: Foam::fixedValueFvPatchField<type>::fixedVal
ueFvPatchField(const Foam::fixedValueFvPatchField<type>&, const Foam::fvPatch&,
const Foam::DimensionedField<type,>&, const Foam::fvPatchFieldMapp
er&) [with Type = Foam::Vector<double>]
/home/ivanlau/OpenFOAM/OpenFOAM-1.4.1/src/finiteVolume/lnInclude/fixedValueFvPat
chField.C:53: note: Foam::fixedValueFvPatchField<type>::fixedVal
ueFvPatchField(const Foam::fvPatch&, const Foam::DimensionedField<Type, Foam::vo
lMesh>&, const Foam::dictionary&) [with Type = Foam::Vector<double>]
/home/ivanlau/OpenFOAM/OpenFOAM-1.4.1/src/finiteVolume/lnInclude/fixedValueFvPat
chField.C:41: note: Foam::fixedValueFvPatchField<type>::fixedVal
ueFvPatchField(const Foam::fvPatch&, const Foam::DimensionedField<Type, Foam::vo
lMesh>&) [with Type = Foam::Vector<double>]
parabolicVelocityFvPatchVectorField.C: In constructor 'Foam::parabolicVelocityFv
PatchVectorField::parabolicVelocityFvPatchVectorFi eld(const Foam::fvPatch&, cons
t Foam::vectorField&, const Foam::dictionary&)':
parabolicVelocityFvPatchVectorField.C:78: error: no matching function for call t
o 'Foam::fixedValueFvPatchField<foam::vector<double> >::fixedValueFvPatchField(c
onst Foam::fvPatch&, const Foam::Field<foam::vector<double> >&)'
/home/ivanlau/OpenFOAM/OpenFOAM-1.4.1/src/finiteVolume/lnInclude/fixedValueFvPat
chField.C:87: note: candidates are: Foam::fixedValueFvPatchField<type>::fixedVal
ueFvPatchField(const Foam::fixedValueFvPatchField<type>&, const Foam::Dimensione
dField<type,>&) [with Type = Foam::Vector<double>]
/home/ivanlau/OpenFOAM/OpenFOAM-1.4.1/src/finiteVolume/lnInclude/fixedValueFvPat
chField.C:76: note: Foam::fixedValueFvPatchField<type>::fixedVal
ueFvPatchField(const Foam::fixedValueFvPatchField<type>&) [with Type = Foam::Vec
tor<double>]
/home/ivanlau/OpenFOAM/OpenFOAM-1.4.1/src/finiteVolume/lnInclude/fixedValueFvPat
chField.C:66: note: Foam::fixedValueFvPatchField<type>::fixedVal
ueFvPatchField(const Foam::fixedValueFvPatchField<type>&, const Foam::fvPatch&,
const Foam::DimensionedField<type,>&, const Foam::fvPatchFieldMapp
er&) [with Type = Foam::Vector<double>]
/home/ivanlau/OpenFOAM/OpenFOAM-1.4.1/src/finiteVolume/lnInclude/fixedValueFvPat
chField.C:53: note: Foam::fixedValueFvPatchField<type>::fixedVal
ueFvPatchField(const Foam::fvPatch&, const Foam::DimensionedField<Type, Foam::vo
lMesh>&, const Foam::dictionary&) [with Type = Foam::Vector<double>]
/home/ivanlau/OpenFOAM/OpenFOAM-1.4.1/src/finiteVolume/lnInclude/fixedValueFvPat
chField.C:41: note: Foam::fixedValueFvPatchField<type>::fixedVal
ueFvPatchField(const Foam::fvPatch&, const Foam::DimensionedField<Type, Foam::vo
lMesh>&) [with Type = Foam::Vector<double>]
parabolicVelocityFvPatchVectorField.C: In constructor 'Foam::parabolicVelocityFv
PatchVectorField::parabolicVelocityFvPatchVectorFi eld(const Foam::parabolicVeloc
ityFvPatchVectorField&, const Foam::vectorField&)':
parabolicVelocityFvPatchVectorField.C:103: error: no matching function for call
to 'Foam::fixedValueFvPatchField<foam::vector<double> >::fixedValueFvPatchField(
const Foam::parabolicVelocityFvPatchVectorField&, const Foam::Field<Foam::Vector
<double> >&)'
/home/ivanlau/OpenFOAM/OpenFOAM-1.4.1/src/finiteVolume/lnInclude/fixedValueFvPat chField.C:87: note: candidates are: Foam::fixedValueFvPatchField<type>::fixedVal ueFvPatchField(const Foam::fixedValueFvPatchField<type>&, const Foam::Dimensione dField<type,>&) [with Type = Foam::Vector<double>]
/home/ivanlau/OpenFOAM/OpenFOAM-1.4.1/src/finiteVolume/lnInclude/fixedValueFvPat chField.C:76: note: Foam::fixedValueFvPatchField<type>::fixedVal ueFvPatchField(const Foam::fixedValueFvPatchField<type>&) [with Type = Foam::Vec tor<double>]
/home/ivanlau/OpenFOAM/OpenFOAM-1.4.1/src/finiteVolume/lnInclude/fixedValueFvPat chField.C:66: note: Foam::fixedValueFvPatchField<type>::fixedVal ueFvPatchField(const Foam::fixedValueFvPatchField<type>&, const Foam::fvPatch&, const Foam::DimensionedField<type,>&, const Foam::fvPatchFieldMapp er&) [with Type = Foam::Vector<double>]
/home/ivanlau/OpenFOAM/OpenFOAM-1.4.1/src/finiteVolume/lnInclude/fixedValueFvPat chField.C:53: note: Foam::fixedValueFvPatchField<type>::fixedVal ueFvPatchField(const Foam::fvPatch&, const Foam::DimensionedField<type,>&, const Foam::dictionary&) [with Type = Foam::Vector<double>]
/home/ivanlau/OpenFOAM/OpenFOAM-1.4.1/src/finiteVolume/lnInclude/fixedValueFvPat chField.C:41: note: Foam::fixedValueFvPatchField<type>::fixedVal ueFvPatchField(const Foam::fvPatch&, const Foam::DimensionedField<type,>&) [with Type = Foam::Vector<double>]
make: *** [Make/linuxGccDPOpt/parabolicVelocityFvPatchVectorField.o] Error 1
ivanwhlau is offline   Reply With Quote

Old   June 25, 2008, 11:34
Default Hello again. Is any of thes
  #76
Senior Member
 
sega's Avatar
 
Sebastian Gatzka
Join Date: Mar 2009
Location: Frankfurt, Germany
Posts: 729
Rep Power: 11
sega is on a distinguished road
Hello again.

Is any of these tools capable of setting a parabolic inlet velocity in y-direction?
One of the first messages stated, that this is setting a profile in x-direction ...

I need a parabolic inflow boundary in U for my nucleate boiling case. The gas is flowing through a hole in the bottom, so I don't have to simulate the evaporation itself ...

http://therealsega.th.funpic.de/openfoam/nb.mpg
__________________
Schrödingers wife: "What did you do to the cat? It's half dead!"
sega is offline   Reply With Quote

Old   June 25, 2008, 13:40
Default There are two options: - yo
  #77
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,914
Rep Power: 40
gschaider will become famous soon enoughgschaider will become famous soon enough
There are two options:
- you turn your geometry so that the inlet points in the right direction
- you replace Y wit X and vice versa in the utility (it's not THAT hard)
But writing (and publishing) a separate utility for every direction in space sems a bit of an overkill to me

Bernhard
__________________
Note: I don't use "Friend"-feature on this forum out of principle. Ah. And by the way: I'm not on Facebook either. So don't be offended if I don't accept your invitation/friend request
gschaider is offline   Reply With Quote

Old   June 26, 2008, 05:02
Default Hello! For switching Y and
  #78
Senior Member
 
sega's Avatar
 
Sebastian Gatzka
Join Date: Mar 2009
Location: Frankfurt, Germany
Posts: 729
Rep Power: 11
sega is on a distinguished road
Hello!

For switching Y and X inside the utility I will have to take a closer look at it. Unfortunately I haven't worked with C++ before. But I will try.

Meanwhile: Do you think I can manage a parabolic distribution with your funkySetFields tool?
Or is it restricted for "internal" fields?
__________________
Schrödingers wife: "What did you do to the cat? It's half dead!"
sega is offline   Reply With Quote

Old   June 26, 2008, 05:15
Default hi, i am trying to run a case
  #79
Member
 
davey david
Join Date: Mar 2009
Posts: 54
Rep Power: 8
suredross is on a distinguished road
hi,
i am trying to run a case(modified icoFoam)which reads an electric field values of the cells immediately next to the boundary onto the boundary itself.anytime i try to run it i get this error:


Exec : jxnFoam OpenFOAM/OpenFOAM-1.4.1/tutorials/junctionFoam/ rectCy_c
Date : Jun 26 2008
Time : 10:59:47
Host : sm-pc16-linux.bcinet-uni-dortmund.de
PID : 5785
Root : OpenFOAM/OpenFOAM-1.4.1/tutorials/junctionFoam/
Case : rectCy_c
Nprocs : 1
Create time

Create mesh for time = 0

Reading Inputparameters

Reading transportProperties

Reading field psi


Starting time loop

Time = 5e-06

DICPCG: Solving for psi, Initial residual = 1, Final residual = 8.11687e-21, No Iterations 61
ExecutionTime = 0.01 s ClockTime = 0 s

Time = 1e-05

DICPCG: Solving for psi, Initial residual = 2.09005e-15, Final residual = 5.05535e-21, No Iterations 27
ExecutionTime = 0.01 s ClockTime = 0 s

Time = 1.5e-05

DICPCG: Solving for psi, Initial residual = 8.55857e-16, Final residual = 7.53713e-21, No Iterations 26
ExecutionTime = 0.01 s ClockTime = 0 s

*** glibc detected *** jxnFoam: munmap_chunk(): invalid pointer: 0x0839f310 ***
======= Backtrace: =========
/lib/libc.so.6(cfree+0x1bb)[0x63021b]
/home/cfd/OpenFOAM/linux/gcc-4.2.1/lib/libstdc++.so.6(_ZdlPv+0x21)[0x540a71]
/home/cfd/OpenFOAM/linux/gcc-4.2.1/lib/libstdc++.so.6(_ZdaPv+0x1d)[0x540acd]
/home/cfd/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libfiniteVolume.so(_ZN4Foam1 8cyclicFvPatchFieldIdED0Ev+0x62)[0xd3a042]
jxnFoam(_ZN4Foam14GeometricFieldIdNS_12fvPatchFiel dENS_7volMeshEED1Ev+0x92)[0x80 53052]
jxnFoam[0x80514fe]
/lib/libc.so.6(__libc_start_main+0xe0)[0x5d9390]
jxnFoam(_ZN4Foam11regIOobject14readIfModifiedEv+0x 18d)[0x804fef1]
======= Memory map: ========
00110000-00111000 r-xp 00110000 00:00 0 [vdso]
00111000-00479000 r-xp 00000000 08:05 5737105 /home/cfd/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libOpenFOAM.so
00479000-00481000 r-xp 00367000 08:05 5737105 /home/cfd/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libOpenFOAM.so
00481000-00484000 rwxp 0036f000 08:05 5737105 /home/cfd/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libOpenFOAM.so
00484000-00488000 rwxp 00484000 00:00 0
00488000-0048b000 r-xp 00000000 08:02 2035025 /lib/libdl-2.7.so
0048b000-0048c000 r-xp 00002000 08:02 2035025 /lib/libdl-2.7.so
0048c000-0048d000 rwxp 00003000 08:02 2035025 /lib/libdl-2.7.so
0048d000-0056b000 r-xp 00000000 08:05 5800989 /home/cfd/OpenFOAM/linux/gcc-4.2.1/lib/libstdc++.so.6.0.9
0056b000-0056f000 r-xp 000dd000 08:05 5800989 /home/cfd/OpenFOAM/linux/gcc-4.2.1/lib/libstdc++.so.6.0.9
0056f000-00570000 rwxp 000e1000 08:05 5800989 /home/cfd/OpenFOAM/linux/gcc-4.2.1/lib/libstdc++.so.6.0.9
00570000-00576000 rwxp 00570000 00:00 0
00576000-0059d000 r-xp 00000000 08:02 2035027 /lib/libm-2.7.so
0059d000-0059e000 r-xp 00026000 08:02 2035027 /lib/libm-2.7.so
0059e000-0059f000 rwxp 00027000 08:02 2035027 /lib/libm-2.7.so
0059f000-005a9000 r-xp 00000000 08:05 5800979 /home/cfd/OpenFOAM/linux/gcc-4.2.1/lib/libgcc_s.so.1
005a9000-005aa000 rwxp 00009000 08:05 5800979 /home/cfd/OpenFOAM/linux/gcc-4.2.1/lib/libgcc_s.so.1
005aa000-005bf000 r-xp 00000000 08:02 2035031 /lib/libpthread-2.7.so
005bf000-005c0000 r-xp 00014000 08:02 2035031 /lib/libpthread-2.7.so
005c0000-005c1000 rwxp 00015000 08:02 2035031 /lib/libpthread-2.7.so
005c1000-005c3000 rwxp 005c1000 00:00 0
005c3000-00716000 r-xp 00000000 08:02 2035024 /lib/libc-2.7.so
00716000-00718000 r-xp 00153000 08:02 2035024 /lib/libc-2.7.so
00718000-00719000 rwxp 00155000 08:02 2035024 /lib/libc-2.7.so
00719000-0071c000 rwxp 00719000 00:00 0
0071c000-0079c000 r-xp 00000000 08:05 5737086 /home/cfd/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libtriSurface.so
0079c000-0079d000 r-xp 00080000 08:05 5737086 /home/cfd/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libtriSurface.so
0079d000-0079e000 rwxp 00081000 08:05 5737086 /home/cfd/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libtriSurface.so
0079e000-00903000 r-xp 00000000 08:05 5737069 /home/cfd/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libmeshTools.so
00903000-00905000 r-xp 00164000 08:05 5737069 /home/cfd/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libmeshTools.so
00905000-00907000 rwxp 00166000 08:05 5737069 /home/cfd/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libmeshTools.so
00907000-0090e000 r-xp 00000000 08:05 5767172 /home/cfd/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/openmpi-1.2.3/libPstream.so
0090e000-0090f000 r-xp 00006000 08:05 5767172 /home/cfd/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/openmpi-1.2.3/libPstream.so
0090f000-00910000 rwxp 00007000 08:05 5767172 /home/cfd/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/openmpi-1.2.3/libPstream.so
00910000-00922000 r-xp 00000000 08:05 5737070 /home/cfd/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libz.so
00922000-00923000 r-xp 00011000 08:05 5737070 /home/cfd/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libz.so
00923000-00924000 rwxp 00012000 08:05 5737070 /home/cfd/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libz.so
00924000-00926000 r-xp 00000000 08:05 5737057 /home/cfd/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/liblagrangian.so
00926000-00927000 r-xp 00001000 08:05 5737057 /home/cfd/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/liblagrangian.so
00927000-00928000 rwxp 00002000 08:05 5737057 /home/cfd/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/liblagrangian.so
00928000-00996000 r-xp 00000000 08:05 5538744 /home/cfd/OpenFOAM/OpenFOAM-1.4.1/src/openmpi-1.2.3/platforms/linuxGccDPOpt/lib/ libmpi.so.0.0.0
00996000-00997000 r-xp 0006d000 08:05 5538744 /home/cfd/OpenFOAM/OpenFOAM-1.4.1/src/openmpi-1.2.3/platforms/linuxGccDPOpt/lib/ libmpi.so.0.0.0
00997000-0099e000 rwxp 0006e000 08:05 5538744 /home/cfd/OpenFOAM/OpenFOAM-1.4.1/src/openmpi-1.2.3/platforms/linuxGccDPOpt/lib/ libmpi.so.0.0.0
0099e000-009a4000 rwxp 0099e000 00:00 0
009a4000-009f3000 r-xp 00000000 08:05 5538753 /home/cfd/OpenFOAM/OpenFOAM-1.4.1/src/openmpi-1.2.3/platforms/linuxGccDPOpt/lib/ libopen-rte.so.0.0.0
009f3000-009f4000 r-xp 0004f000 08:05 5538753 /home/cfd/OpenFOAM/OpenFOAM-1.4.1/src/openmpi-1.2.3/platforms/linuxGccDPOpt/lib/ libopen-rte.so.0.0.0
009f4000-009f6000 rwxp 00050000 08:05 5538753 /home/cfd/OpenFOAM/OpenFOAM-1.4.1/src/openmpi-1.2.3/platforms/linuxGccDPOpt/lib/ libopen-rte.so.0.0.0
009f6000-00a0b000 r-xp 00000000 08:02 2035036 /lib/libnsl-2.7.so
00a0b000-00a0c000 r-xp 00014000 08:02 2035036 /lib/libnsl-2.7.so
00a0c000-00a0d000 rwxp 00015000 08:02 2035036 /lib/libnsl-2.7.so
00a0d000-00a0f000 rwxp 00a0d000 00:00 0
00a0f000-00a11000 r-xp 00000000 08:02 2035043 /lib/libutil-2.7.so
00a11000-00a12000 r-xp 00001000 08:02 2035043 /lib/libutil-2.7.so
00a12000-00a13000 rwxp 00002000 08:02 2035043 /lib/libutil-2.7.so
00a2d000-00a48000 r-xp 00000000 08:02 2034710 /lib/ld-2.7.so
00a48000-00a49000 r-xp 0001a000 08:02 2034710 /lib/ld-2.7.so
00a49000-00a4a000 rwxp 0001b000 08:02 2034710 /lib/ld-2.7.so
00a4a000-014f5000 r-xp 00000000 08:05 5737061 /home/cfd/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libfiniteVolume.so
014f5000-0150d000 r-xp 00aaa000 08:05 5737061 /home/cfd/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libfiniteVolume.so
0150d000-01511000 rwxp 00ac2000 08:05 5737061 /home/cfd/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libfiniteVolume.so
01511000-01514000 rwxp 01511000 00:00 0
02d56000-02d8a000 r-xp 00000000 08:05 5538751 /home/cfd/OpenFOAM/OpenFOAM-1.4.1/src/openmpi-1.2.3/platforms/linuxGccDPOpt/lib/ libopen-pal.so.0.0.0
02d8a000-02d8b000 r-xp 00033000 08:05 5538751 /home/cfd/OpenFOAM/OpenFOAM-1.4.1/src/openmpi-1.2.3/platforms/linuxGccDPOpt/lib/ libopen-pal.so.0.0.0
02d8b000-02d8c000 rwxp 00034000 08:05 5538751 /home/cfd/OpenFOAM/OpenFOAM-1.4.1/src/openmpi-1.2.3/platforms/linuxGccDPOpt/lib/ libopen-pal.so.0.0.0
02d8c000-02dae000 rwxp 02d8c000 00:00 0
08048000-0806c000 r-xp 00000000 08:05 5800997 /home/cfd/OpenFOAM/OpenFOAM-1.4.1/applications/bin/linuxGccDPOpt/jxnFoam
0806c000-0806d000 rw-p 00024000 08:05 5800997 /home/cfd/OpenFOAM/OpenFOAM-1.4.1/applications/bin/linuxGccDPOpt/jxnFoam
0831b000-083e1000 rw-p 0831b000 00:00 0
b7efb000-b7f30000 r--s 00000000 08:02 1968471 /var/db/nscd/passwd
b7f30000-b7f36000 rw-p b7f30000 00:00 0
b7f51000-b7f53000 rw-p b7f51000 00:00 0
bfc6e000-bfc84000 rw-p bffe9000 00:00 0 [stack]
Aborted

can anyone help me to know what is amiss?
thanks in advance

davey
suredross is offline   Reply With Quote

Old   June 26, 2008, 05:23
Default Ok, from my point of view I ha
  #80
Senior Member
 
sega's Avatar
 
Sebastian Gatzka
Join Date: Mar 2009
Location: Frankfurt, Germany
Posts: 729
Rep Power: 11
sega is on a distinguished road
Ok, from my point of view I have to modify the C-File like the following - have a look:

http://therealsega.th.funpic.de/open...bolicInlet.pdf

At the marked positions I have to change y into x anx Y into X. Am I guessing right?
__________________
Schrödingers wife: "What did you do to the cat? It's half dead!"
sega is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
2D air parabolic velocity profile ilker FLUENT 2 November 12, 2008 09:43
UDF Unsteady velocity parabolic profile Rashad FLUENT 2 February 29, 2008 03:36
parabolic velocity profile? bssdyl FLUENT 4 March 22, 2006 12:32
problem in 3d parabolic velocity profile Lokesh FLUENT 8 August 11, 2005 05:36
Parabolic temperature Inlet Profile in a tube majestywzh FLUENT 0 April 9, 2003 06:37


All times are GMT -4. The time now is 11:02.