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

Rotation Boundary Condition

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

Like Tree1Likes
  • 1 Post By rswbroers

Reply
 
LinkBack Thread Tools Display Modes
Old   May 15, 2007, 04:28
Default Using the help of the forum (
  #1
rswbroers
Guest
 
Posts: n/a
Using the help of the forum ( http://www.cfd-online.com/OpenFOAM_D...ges/1/174.html ), I've managed to set up a case with a rotation boundary condition by adding the following lines to simpleFoam.C, just ahead of the start of the time loop:

/***********************************************/
label patchID = mesh.boundaryMesh().findPatchID("WHEEL");
const polyPatch& cPatch = mesh.boundaryMesh()[patchID];
const vectorField& FaceCentres = cPatch.faceCentres();

point origin(0.5, 0.20, 0.5);
vector axis(0, 0, 1);
scalar radPerSecond(5);

const vectorField& tempRotation = radPerSecond * axis ^ (FaceCentres - origin);
U.boundaryField()[patchID] == tempRotation;
/***********************************************/

This does exactly what I want it to do, except for the fact that the rotation specification (i.e. origin, axis, radPerSecond and the patch name this is applied to) is hard coded into the executable.

What I am looking for is way of reading the rotation specification in from file. For example from the file 0/U (or similar):

boundaryField
{

WHEEL
{
type rotation;
origin (0.5 0.2 0.5);
axis (0 0 1);
radPerSecond (5);
}

Is such a thing possible? Where should I look for examples this?

Thank you very much.

best regards,
Roland
  Reply With Quote

Old   May 15, 2007, 06:34
Default Hello, Roland! I did it in
  #2
New Member
 
Normunds Jekabsons
Join Date: Mar 2009
Location: Riga, Latvia
Posts: 10
Rep Power: 8
normunds is on a distinguished road
Hello, Roland!

I did it in that way, see code in


ftp://ftp.jesystems.eu/pub/OpenFoam/...ionFoam.tar.gz


and the case

ftp://ftp.jesystems.eu/pub/OpenFoam/...ionFoam.tar.gz

result is

ftp://ftp.jesystems.eu/pub/OpenFoam/...n/rotation.tif

Well, it is my "development version"
of rotation boundary condition,
please check it before serious use!

You may split my vectorial
w0 to axis and angular
rotation frequency.


best regards

/Normunds
normunds is offline   Reply With Quote

Old   May 15, 2007, 07:21
Default Normunds, It looks interest
  #3
rswbroers
Guest
 
Posts: n/a
Normunds,

It looks interesting. I will study it.

Thanks,
Roland
  Reply With Quote

Old   May 15, 2007, 08:29
Default you may also find different ut
  #4
Member
 
rafal zietara
Join Date: Mar 2009
Location: Manchester, UK
Posts: 60
Rep Power: 8
rafal is on a distinguished road
you may also find different utility useful.
one i wrote for mixer3D. it is on the
basis of patchAverage utility and has
the same syntax. it sets velocity on
specified patch. it reads all necessary
rotation parameters from dynamicMeshDict
of dynamic mesh (similar to mixer2D case
in OpenFOAM-1.3).
I used it with fixedValue BC.
invoke it once at the beginning and then
solve everything later like with
standard fixedValue not bothered to think if
my patch is doing right job or not.

patchMixerSetVel.tar.gz

hope that helps.
rafal

(note: this code could be better written
and cleaner but it is doing job well
so I left it as it is. feel free to modify
it )
rafal is offline   Reply With Quote

Old   May 21, 2007, 04:54
Default Normunds, Rafal, Thank you
  #5
rswbroers
Guest
 
Posts: n/a
Normunds, Rafal,

Thank you for your codes. Both do what I was looking for, each in a different manner. Unfortunately both also have a (different) drawback that prevents me from using it for practical applications.

With Normunds' code you specify the rotation b.c. in the startTime U file, as you would with an ordinary moving wall. This works perfectly.
However it is not possible to restart a run as the rotation specification is not copied to any new time directories, which is serious drawback.

Attached below is my modification of Normunds' code. I compiled it with simpleFOAM by adding uniformAxialRotation.C to simpleFOAM/Make/files. Also included is an example U file.

Would it be possible to copy the rotation specification to new time directories? Or would, perhaps, another approach would be better?

/attach{uniformAxialRotation.tar.gz}

Rafals code works by creating a nonuniform list before running a case. It does not modify any of the solvers, which makes it nice and simple. When running on my pc it works perfectly. However when I try to run it on our cluster it crashes with a segmentation fault. On both computers I tried with two different cases (one small, one large) with the same result.

Attached below is my version of Rafal's code. Included is an example rotationBCDict file that needs to be placed in the constant directory.
The segmentation fault occurs on line 109. Uncommenting line 110 would also cause a segmentation fault. Line 111 would run without a problem. Again, the segmentation fault does not occur on all machines.

Does anyone have an idea what is going wrong here?

/attach{rotationBC.tar.gz}

best regards,
Roland
  Reply With Quote

Old   May 21, 2007, 04:57
Default Sorry, the following links sho
  #6
rswbroers
Guest
 
Posts: n/a
Sorry, the following links should work:

uniformAxialRotation.tar.gz
rotationBC.tar.gz

regards,
Roland
giuli@ likes this.
  Reply With Quote

Old   May 21, 2007, 10:34
Default seems result is calculated not
  #7
Member
 
rafal zietara
Join Date: Mar 2009
Location: Manchester, UK
Posts: 60
Rep Power: 8
rafal is on a distinguished road
seems result is calculated not properly.
spit out _omega, _axis, faceCentres, _centre.
and see if the values are correct.
My code it was fast simple implementation for
my specific case of rotating plain surface. it
may be buggy for other cases and certainly do not support to be applied on moving wall for this you need to update variables every time step.
rafal
rafal is offline   Reply With Quote

Old   May 22, 2007, 03:58
Default Rafal, The calculation of r
  #8
rswbroers
Guest
 
Posts: n/a
Rafal,

The calculation of result looks exactly as it should be on the working machine. And on both machines _omega, _axis, _centre and faceCentres look identical, so I doubt this is causing the trouble.

Actually I think your code is suitable for what I am trying to do. As type remains fixedValue (for U), the nonuniform List is copied to each timestep/iteration without alterations. It is no different, at least to my limited knowledge of OF, to specifying a uniformly moving wall using 'value uniform (1 0 0);'.

best regards,
Roland
  Reply With Quote

Old   May 22, 2007, 08:13
Default Setting a rotation boundary co
  #9
rswbroers
Guest
 
Posts: n/a
Setting a rotation boundary condition now works on both machines by changing line 108 from

const vectorField& result = _omega * _axis ^ (faceCentres - _centre);

to

vectorField result = _omega * _axis ^ (faceCentres - _centre);

I have absolutely no idea why the original line failed to work on one machine and worked perfectly on another.

best regards,
Roland
  Reply With Quote

Old   May 22, 2007, 13:48
Default The original line should never
  #10
Senior Member
 
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 12
eugene is on a distinguished road
The original line should never work! In fact I'm surprised it compiles.

"const vectorField&" is is a constant reference to an existing vector field object.
eugene is offline   Reply With Quote

Old   May 28, 2007, 08:01
Default Eugene is right. Actually I am
  #11
Member
 
rafal zietara
Join Date: Mar 2009
Location: Manchester, UK
Posts: 60
Rep Power: 8
rafal is on a distinguished road
Eugene is right. Actually I am also surprised that compiler didt pick this obvious mistake on all machines.
rafal is offline   Reply With Quote

Old   July 9, 2007, 05:23
Default Hi all, this monday morning,
  #12
Senior Member
 
Cedric DUPRAT
Join Date: Mar 2009
Location: Belgium
Posts: 179
Rep Power: 8
cedric_duprat is on a distinguished road
Hi all,
this monday morning, I'm using the rotationBC which is describe upper,
but .... an error is coming while runing OF:
keyword type is undefined in dictionary "/craya/big/duprat/OpenFOAM/duprat-1.3/duprat-1.3.ori/run/ESSAI2/0/U::walldyna"
so, I would like to know if did well :
1- installing and compilling rotationBC in utilities/preporocessing/
I also correct the mistake describe upper
2- changing my 0/U adding the rotation in my patch walldyna (omega, axis, center) by hand (no FoamX)
which is not running.
then try adding the rotationDict in mycase/system/
but, it is also not runing.

As Srinath propose, I don't use FoamX, so I "run" my case with : oddles .../run mycase

I can't find where I am wrong ...I think I still not understand the Foam's philosophy adding some of newly build B/C, ect, ...

Some help is welcome ...thanks

Cedric
cedric_duprat is offline   Reply With Quote

Old   October 16, 2007, 12:12
Default Hi Cedric did you manage to u
  #13
rengu
Guest
 
Posts: n/a
Hi Cedric
did you manage to use rotationBC?
if yes can you tell me the approach to install it and use it?

best regards,
guillaume
  Reply With Quote

Old   February 5, 2008, 07:41
Default I've tried to compile rotation
  #14
Member
 
Paul Mauk
Join Date: Mar 2009
Posts: 39
Rep Power: 8
plmauk is on a distinguished road
I've tried to compile rotationFoam, making by
Normunds Jekabsons, but following error message
appears :

[plmauk@cfd-61 rotationFoam]$ wmake
SOURCE=boundary/derivated/uniformAxialRotation.C ; g++ -m32 -Dlinux -DDP -Wall -Wno-strict-aliasing -Wextra -Wno-unused-parameter -Wold-style-cast -O3 -DNoRepository -ftemplate-depth-40 -I/home/plmauk/OpenFOAM/OpenFOAM-1.4.1/src/finiteVolume/lnInclude -Iinclude -IlnInclude -I. -I/home/plmauk/OpenFOAM/OpenFOAM-1.4.1/src/OpenFOAM/lnInclude -fPIC -pthread -c $SOURCE -o Make/linuxGccDPOpt/uniformAxialRotation.o
/home/plmauk/OpenFOAM/OpenFOAM-1.4.1/src/OpenFOAM/lnInclude/DimensionedField.H: In instantiation of 'Foam::DimensionedField<foam::vector<double>, Foam::volMesh>':
boundary/derivated/uniformAxialRotation.C:14: instantiated from here
/home/plmauk/OpenFOAM/OpenFOAM-1.4.1/src/OpenFOAM/lnInclude/DimensionedField.H:8 3: error: invalid use of incomplete type 'struct Foam::volMesh'
/home/plmauk/OpenFOAM/OpenFOAM-1.4.1/src/finiteVolume/lnInclude/fvPatchField.H:5 8: error: forward declaration of 'struct Foam::volMesh'
/home/plmauk/OpenFOAM/OpenFOAM-1.4.1/src/OpenFOAM/lnInclude/DimensionedField.H:9 2: error: invalid use of incomplete type 'struct Foam::volMesh'
/home/plmauk/OpenFOAM/OpenFOAM-1.4.1/src/finiteVolume/lnInclude/fvPatchField.H:5 8: error: forward declaration of 'struct Foam::volMesh'
/home/plmauk/OpenFOAM/OpenFOAM-1.4.1/src/OpenFOAM/lnInclude/DimensionedField.C:5 8: error: invalid use of incomplete type 'struct Foam::volMesh'
/home/plmauk/OpenFOAM/OpenFOAM-1.4.1/src/finiteVolume/lnInclude/fvPatchField.H:5 8: error: forward declaration of 'struct Foam::volMesh'
/home/plmauk/OpenFOAM/OpenFOAM-1.4.1/src/OpenFOAM/lnInclude/DimensionedField.C:8 6: error: invalid use of incomplete type 'struct Foam::volMesh'
/home/plmauk/OpenFOAM/OpenFOAM-1.4.1/src/finiteVolume/lnInclude/fvPatchField.H:5 8: error: forward declaration of 'struct Foam::volMesh'
/home/plmauk/OpenFOAM/OpenFOAM-1.4.1/src/OpenFOAM/lnInclude/DimensionedField.C:1 01: error: invalid use of incomplete type 'struct Foam::volMesh'
/home/plmauk/OpenFOAM/OpenFOAM-1.4.1/src/finiteVolume/lnInclude/fvPatchField.H:5 8: error: forward declaration of 'struct Foam::volMesh'
/home/plmauk/OpenFOAM/OpenFOAM-1.4.1/src/OpenFOAM/lnInclude/DimensionedFieldIO.C :59: error: invalid use of incomplete type 'struct Foam::volMesh'
/home/plmauk/OpenFOAM/OpenFOAM-1.4.1/src/finiteVolume/lnInclude/fvPatchField.H:5 8: error: forward declaration of 'struct Foam::volMesh'
/home/plmauk/OpenFOAM/OpenFOAM-1.4.1/src/OpenFOAM/lnInclude/DimensionedFieldI.H: 36: error: invalid use of incomplete type 'struct Foam::volMesh'
/home/plmauk/OpenFOAM/OpenFOAM-1.4.1/src/finiteVolume/lnInclude/fvPatchField.H:5 8: error: forward declaration of 'struct Foam::volMesh'
boundary/derivated/uniformAxialRotation.C: In constructor 'Foam::uniformAxialRotationFvPatch::uniformAxialRo tationFvPatch(const Foam::fvPatch&, const Foam::vectorField&)':
boundary/derivated/uniformAxialRotation.C:14: error: no matching function for call to 'Foam::fixedValueFvPatchField<foam::vector<double> >::fixedValueFvPatchField(const Foam::fvPatch&, const Foam::Field<foam::vector<double> >&)'
/home/plmauk/OpenFOAM/OpenFOAM-1.4.1/src/finiteVolume/lnInclude/fixedValueFvPatc hField.C:87: note: candidates are: Foam::fixedValueFvPatchField<type>::fixedValueFvPa tchField(const Foam::fixedValueFvPatchField<type>&, const Foam::DimensionedField<type,>&) [with Type = Foam::Vector<double>]
/home/plmauk/OpenFOAM/OpenFOAM-1.4.1/src/finiteVolume/lnInclude/fixedValueFvPatc hField.C:76: note: Foam::fixedValueFvPatchField<type>::fixedValueFvPa tchField(const Foam::fixedValueFvPatchField<type>&) [with Type = Foam::Vector<double>]
/home/plmauk/OpenFOAM/OpenFOAM-1.4.1/src/finiteVolume/lnInclude/fixedValueFvPatc hField.C:66: note: Foam::fixedValueFvPatchField<type>::fixedValueFvPa tchField(const Foam::fixedValueFvPatchField<type>&, const Foam::fvPatch&, const Foam::DimensionedField<type,>&, const Foam::fvPatchFieldMapper&) [with Type = Foam::Vector<double>]
/home/plmauk/OpenFOAM/OpenFOAM-1.4.1/src/finiteVolume/lnInclude/fixedValueFvPatc hField.C:53: note: Foam::fixedValueFvPatchField<type>::fixedValueFvPa tchField(const Foam::fvPatch&, const Foam::DimensionedField<type,>&, const Foam::dictionary&) [with Type = Foam::Vector<double>]
/home/plmauk/OpenFOAM/OpenFOAM-1.4.1/src/finiteVolume/lnInclude/fixedValueFvPatc hField.C:41: note: Foam::fixedValueFvPatchField<type>::fixedValueFvPa tchField(const Foam::fvPatch&, const Foam::DimensionedField<type,>&) [with Type = Foam::Vector<double>]
boundary/derivated/uniformAxialRotation.C:17: error: 'class Foam::uniformAxialRotationFvPatch' has no member named 'checkVolField'
boundary/derivated/uniformAxialRotation.C: In constructor 'Foam::uniformAxialRotationFvPatch::uniformAxialRo tationFvPatch(const Foam::fvPatch&, const Foam::Field<foam::vector<double> >&, const Foam::dictionary&)':
boundary/derivated/uniformAxialRotation.C:32: error: no matching function for call to 'Foam::fixedValueFvPatchField<foam::vector<double> >::fixedValueFvPatchField(const Foam::fvPatch&, const Foam::Field<foam::vector<double> >&, const Foam::dictionary&)'
/home/plmauk/OpenFOAM/OpenFOAM-1.4.1/src/finiteVolume/lnInclude/fixedValueFvPatc hField.C:87: note: candidates are: Foam::fixedValueFvPatchField<type>::fixedValueFvPa tchField(const Foam::fixedValueFvPatchField<type>&, const Foam::DimensionedField<type,>&) [with Type = Foam::Vector<double>]
/home/plmauk/OpenFOAM/OpenFOAM-1.4.1/src/finiteVolume/lnInclude/fixedValueFvPatc hField.C:76: note: Foam::fixedValueFvPatchField<type>::fixedValueFvPa tchField(const Foam::fixedValueFvPatchField<type>&) [with Type = Foam::Vector<double>]
/home/plmauk/OpenFOAM/OpenFOAM-1.4.1/src/finiteVolume/lnInclude/fixedValueFvPatc hField.C:66: note: Foam::fixedValueFvPatchField<type>::fixedValueFvPa tchField(const Foam::fixedValueFvPatchField<type>&, const Foam::fvPatch&, const Foam::DimensionedField<type,>&, const Foam::fvPatchFieldMapper&) [with Type = Foam::Vector<double>]
/home/plmauk/OpenFOAM/OpenFOAM-1.4.1/src/finiteVolume/lnInclude/fixedValueFvPatc hField.C:53: note: Foam::fixedValueFvPatchField<type>::fixedValueFvPa tchField(const Foam::fvPatch&, const Foam::DimensionedField<type,>&, const Foam::dictionary&) [with Type = Foam::Vector<double>]
/home/plmauk/OpenFOAM/OpenFOAM-1.4.1/src/finiteVolume/lnInclude/fixedValueFvPatc hField.C:41: note: Foam::fixedValueFvPatchField<type>::fixedValueFvPa tchField(const Foam::fvPatch&, const Foam::DimensionedField<type,>&) [with Type = Foam::Vector<double>]
boundary/derivated/uniformAxialRotation.C: In constructor 'Foam::uniformAxialRotationFvPatch::uniformAxialRo tationFvPatch(const Foam::uniformAxialRotationFvPatch&, const Foam::fvPatch&, const Foam::Field<foam::vector<double> >&, const Foam::fvPatchFieldMapper&)':
boundary/derivated/uniformAxialRotation.C:54: error: no matching function for call to 'Foam::fixedValueFvPatchField<foam::vector<double> >::fixedValueFvPatchField(const Foam::uniformAxialRotationFvPatch&, const Foam::fvPatch&, const Foam::Field<foam::vector<double> >&, const Foam::fvPatchFieldMapper&)'
/home/plmauk/OpenFOAM/OpenFOAM-1.4.1/src/finiteVolume/lnInclude/fixedValueFvPatc hField.C:87: note: candidates are: Foam::fixedValueFvPatchField<type>::fixedValueFvPa tchField(const Foam::fixedValueFvPatchField<type>&, const Foam::DimensionedField<type,>&) [with Type = Foam::Vector<double>]
/home/plmauk/OpenFOAM/OpenFOAM-1.4.1/src/finiteVolume/lnInclude/fixedValueFvPatc hField.C:76: note: Foam::fixedValueFvPatchField<type>::fixedValueFvPa tchField(const Foam::fixedValueFvPatchField<type>&) [with Type = Foam::Vector<double>]
/home/plmauk/OpenFOAM/OpenFOAM-1.4.1/src/finiteVolume/lnInclude/fixedValueFvPatc hField.C:66: note: Foam::fixedValueFvPatchField<type>::fixedValueFvPa tchField(const Foam::fixedValueFvPatchField<type>&, const Foam::fvPatch&, const Foam::DimensionedField<type,>&, const Foam::fvPatchFieldMapper&) [with Type = Foam::Vector<double>]
/home/plmauk/OpenFOAM/OpenFOAM-1.4.1/src/finiteVolume/lnInclude/fixedValueFvPatc hField.C:53: note: Foam::fixedValueFvPatchField<type>::fixedValueFvPa tchField(const Foam::fvPatch&, const Foam::DimensionedField<type,>&, const Foam::dictionary&) [with Type = Foam::Vector<double>]
/home/plmauk/OpenFOAM/OpenFOAM-1.4.1/src/finiteVolume/lnInclude/fixedValueFvPatc hField.C:41: note: Foam::fixedValueFvPatchField<type>::fixedValueFvPa tchField(const Foam::fvPatch&, const Foam::DimensionedField<type,>&) [with Type = Foam::Vector<double>]
boundary/derivated/uniformAxialRotation.C: In constructor 'Foam::uniformAxialRotationFvPatch::uniformAxialRo tationFvPatch(const Foam::uniformAxialRotationFvPatch&, const Foam::Field<foam::vector<double> >&)':
boundary/derivated/uniformAxialRotation.C:66: error: no matching function for call to 'Foam::fixedValueFvPatchField<foam::vector<double> >::fixedValueFvPatchField(const Foam::uniformAxialRotationFvPatch&, const Foam::Field<foam::vector<double> >&)'
/home/plmauk/OpenFOAM/OpenFOAM-1.4.1/src/finiteVolume/lnInclude/fixedValueFvPatc hField.C:87: note: candidates are: Foam::fixedValueFvPatchField<type>::fixedValueFvPa tchField(const Foam::fixedValueFvPatchField<type>&, const Foam::DimensionedField<type,>&) [with Type = Foam::Vector<double>]
/home/plmauk/OpenFOAM/OpenFOAM-1.4.1/src/finiteVolume/lnInclude/fixedValueFvPatc hField.C:76: note: Foam::fixedValueFvPatchField<type>::fixedValueFvPa tchField(const Foam::fixedValueFvPatchField<type>&) [with Type = Foam::Vector<double>]
/home/plmauk/OpenFOAM/OpenFOAM-1.4.1/src/finiteVolume/lnInclude/fixedValueFvPatc hField.C:66: note: Foam::fixedValueFvPatchField<type>::fixedValueFvPa tchField(const Foam::fixedValueFvPatchField<type>&, const Foam::fvPatch&, const Foam::DimensionedField<type,>&, const Foam::fvPatchFieldMapper&) [with Type = Foam::Vector<double>]
/home/plmauk/OpenFOAM/OpenFOAM-1.4.1/src/finiteVolume/lnInclude/fixedValueFvPatc hField.C:53: note: Foam::fixedValueFvPatchField<type>::fixedValueFvPa tchField(const Foam::fvPatch&, const Foam::DimensionedField<type,>&, const Foam::dictionary&) [with Type = Foam::Vector<double>]
/home/plmauk/OpenFOAM/OpenFOAM-1.4.1/src/finiteVolume/lnInclude/fixedValueFvPatc hField.C:41: note: Foam::fixedValueFvPatchField<type>::fixedValueFvPa tchField(const Foam::fvPatch&, const Foam::DimensionedField<type,>&) [with Type = Foam::Vector<double>]
make: *** [Make/linuxGccDPOpt/uniformAxialRotation.o] Fehler 1
plmauk is offline   Reply With Quote

Old   February 5, 2008, 09:58
Default Hello Paul! This is an old
  #15
New Member
 
Normunds Jekabsons
Join Date: Mar 2009
Location: Riga, Latvia
Posts: 10
Rep Power: 8
normunds is on a distinguished road
Hello Paul!

This is an old one, some kind of early development version. It works with OF 1.3 only. I have version for 1.4.1, just I can post it only tomorrow morning.

best regards

/normunds
normunds is offline   Reply With Quote

Old   February 6, 2008, 04:27
Default This, perhaps, is slightly bet
  #16
New Member
 
Normunds Jekabsons
Join Date: Mar 2009
Location: Riga, Latvia
Posts: 10
Rep Power: 8
normunds is on a distinguished road
This, perhaps, is slightly better. I am using myself it for time dependent rotation, with a different
updateRot() function.

/Normunds

testRotationFoam.tar
testRoatationCase.tar.bz2
normunds is offline   Reply With Quote

Old   February 6, 2008, 05:24
Default Hi Paul, I just would like
  #17
Senior Member
 
Cedric DUPRAT
Join Date: Mar 2009
Location: Belgium
Posts: 179
Rep Power: 8
cedric_duprat is on a distinguished road
Hi Paul,

I just would like to add that there is also one code avaiable on the wiki from Sig turbomachinery.
You will find all the details here: http://openfoamwiki.net/index.php/Si...e_next_meeting
in addSwirlAndRotation.

Cedric
cedric_duprat is offline   Reply With Quote

Old   February 6, 2008, 06:30
Default Thanks a lot for support, Norm
  #18
Member
 
Paul Mauk
Join Date: Mar 2009
Posts: 39
Rep Power: 8
plmauk is on a distinguished road
Thanks a lot for support, Normunds und Cedric!
I will try it.

Best regards
Paul.
plmauk 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
Boundary condition of the third kind or Danckwertz boundary condition plage OpenFOAM Running, Solving & CFD 4 October 3, 2006 12:21
fan boundary condition? kiran kumar CD-adapco 1 August 4, 2006 14:07
Boundary Condition TengKuei FLUENT 2 May 15, 2006 10:06
What boundary condition? Shanti FLUENT 2 May 4, 2006 13:01
Slip Boundary Condition for Moving Boundary Shukla Main CFD Forum 3 November 11, 2005 16:02


All times are GMT -4. The time now is 02:12.