|
[Sponsors] |
March 25, 2005, 12:05 |
Hi,
I have a 2D domain consis
|
#1 |
Guest
Posts: n/a
|
Hi,
I have a 2D domain consisting of four blocks. I want to specify the initial condition for a field variable as T=1 in block 0 and as T=0 in the other three blocks. Is there a way to specify the initial condition block-by-block? i.e., in file T in folder 0 use the keyword non-uniform and specify a list of blocks and the corresponding T values. I am a novice user and was not able find an example for this in the user's or programmer's guide or in tutorial cases (e.g., damBreak example is similar but seems to use an initialization program). Thanks. Syam |
|
March 25, 2005, 12:34 |
The concept of blocks only exi
|
#2 |
Senior Member
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,419
Rep Power: 26 |
The concept of blocks only exists in blockMesh. (assuming that you are using blockMesh) After mesh generation (with whichever mesh generator you use) OpenFOAM has no concept of blocks. The whole mesh is one unstructured set of cells of arbitrary shape.
Since there is no information kept on what cells originate from what block you'll have to select them yourself. The damBreak application comes closest to your needs I think. Mattijs |
|
March 25, 2005, 13:04 |
What if you build another case
|
#3 |
Member
diablo80@web.de
Join Date: Mar 2009
Posts: 93
Rep Power: 17 |
What if you build another case, with only one block, coinciding with the one you want T=1. Than, if you use mapFields from there to your actual case....
Would that work for you? I know, it is a little dirty solution... Luiz |
|
March 25, 2005, 16:16 |
Luiz,
Thanks for that clever
|
#4 |
Guest
Posts: n/a
|
Luiz,
Thanks for that clever solution! Although an additional case was needed, your solution reduced the complexity of the original case (fewer blocks) and eliminated the need for an initialization program. Syam |
|
November 15, 2005, 15:06 |
I'm trying to set a turbulent
|
#5 |
Senior Member
Maka Mohu
Join Date: Mar 2009
Posts: 305
Rep Power: 18 |
I'm trying to set a turbulent nonuniform initial condition for a channel flow case. The field is available in a file with the format (column-wise):
x y z u v w p 1) I found that SetField utility that is used in the dam break case (1.2) is designed to do similar job but it uses dictionary as its input. Can any body explain how to use or modify the utility to use a data file as input. 2) I also thought of using mapField utility after trying to make a new case and cast my data into the OpenFOAM format but I faced the following problem: the file constant/polyMesh/"points" describes vertices while what is available at my case is the node values that correspond to the values of 0/U and 0/p. I would be grateful if some body can give some help about how to solve this problem. 3) one final question about constant/polyMesh/cells: does the file format of openFOAM enforces any rules regarding the order of cells in the file or it is fully unstructured and I can order the cells as I like as long as it is consistent with 0/U, and 0/p format. Thanks. best regards, Maka |
|
November 15, 2005, 15:40 |
I noticed a talk about cellSet
|
#6 |
Senior Member
Maka Mohu
Join Date: Mar 2009
Posts: 305
Rep Power: 18 |
I noticed a talk about cellSet in:
http://www.cfd-online.com/OpenFOAM_D...tml?1131637441 http://www.cfd-online.com/OpenFOAM_D...es/1/1240.html Can any one explain or give example of how to use cellSet to solve this problem or even what is cellSet? sorry I'm a beginner. Thanks. Regards, Maka |
|
November 16, 2005, 05:28 |
Look at e.g. interFoam/system/
|
#7 |
Senior Member
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,419
Rep Power: 26 |
Look at e.g. interFoam/system/setFieldsDict.
It uses the 'boxToCell' source. Instead you can use say the 'cellToCell' source which allows you to use a cellSet. (b.t.w. these sources are exactly the same one cellSet uses) Mistype it and run setFields to see all the possible sources. |
|
November 16, 2005, 11:36 |
in boxToCell, we have
ďťżdef
|
#8 |
Member
VVqf
Join Date: Mar 2009
Location: Braunschweig
Posts: 66
Rep Power: 17 |
in boxToCell, we have
ďťżdefaultFieldValues ( volScalarFieldValue alpha 1 ); regions ( boxToCell { box (0.4 0 0) (1 1 0.1); fieldValues ( volScalarFieldValue alpha 0.1 ); } What about cellToCell, how to write this? I looked into the source codes cellToCell.H/C, but didn't find answer. |
|
November 17, 2005, 06:05 |
to e.g. read cellSet c0 replac
|
#9 |
Senior Member
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,419
Rep Power: 26 |
to e.g. read cellSet c0 replace the
boxToCell { box (..)(..) fieldValues ... } with: cellToCell { set "c0"; fieldValues ... } (or maybe lose the quotes around c0) Also look at the sample cellSetDict in the cellSet utility. |
|
January 4, 2006, 07:39 |
Hi Mattijis
How to read in
|
#10 |
Member
Nico Petry
Join Date: Mar 2009
Posts: 36
Rep Power: 17 |
Hi Mattijis
How to read in a file containig a list of cells, for example /constant/polyMesh/sets/fluid.1 ? The file looks like: /*---------------------------------------------------------------------------* FoamFile { version 2.0; format ascii; root "OpenFOAM/nico-1.2/run/tutorials/simpleFoam"; case "test01"; instance ""constant""; local "polyMesh/sets"; class cellSet; object fluid.4; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // 240 ( 50 51 52 53 . . 279 280 ) /*************************************************/ Thanks and a happy new year |
|
January 13, 2006, 05:04 |
As an example for reading a ce
|
#11 |
Assistant Moderator
Bernhard Gschaider
Join Date: Mar 2009
Posts: 4,225
Rep Power: 51 |
As an example for reading a cellSet and manipulating data in these cells you can use this:
http://openfoamwiki.net/index.php/Contrib_setfiel dbycellset
__________________
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 |
|
March 20, 2006, 12:29 |
Hello,
I would like to spec
|
#12 |
Member
Mélanie Piellard
Join Date: Mar 2009
Posts: 86
Rep Power: 17 |
Hello,
I would like to specify non uniform initial conditions for my case, with respect to the coordinates of the nodes. Exemple: the velocity field is defined such as r = x^2 + y^2 U[x] = y * a/ r^2 U[y] = -x * b/ r^2 How would you write it ? Firstly, I don't know how to access to the nodes coordinates which is blocking me... Thanks. |
|
March 21, 2006, 05:09 |
Look at the setGammaDambreak a
|
#13 |
Senior Member
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,419
Rep Power: 26 |
Look at the setGammaDambreak app from OpenFOAM1.1. Or look on this site for setGammaField. It should contain how to access coordinates.
|
|
March 21, 2006, 05:54 |
Mattijs,
I looked at the DamB
|
#14 |
Member
Mélanie Piellard
Join Date: Mar 2009
Posts: 86
Rep Power: 17 |
Mattijs,
I looked at the DamBreak case, but the velocity field is set thanks to a bounding box, so this is a different case. Here I report what I have already written, with the error message at compilation: #include "fvCFD.H" #include "physicalConstants.H" // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // int main(int argc, char *argv[]) { # include "setRootCase.H" # include "createTime.H" # include "createMesh.H" # include "createFields.H" // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // scalar pi = physicalConstant::pi; scalar r_0 = 0.0036; scalar r_c = r_0*2.0/9.0; scalar gamma = 4.0 * pi * r_c * 340.0 / 2.0; forAll(mesh.C(), celli) { scalar x = mesh.C()[celli].x; scalar y = mesh.C()[celli].y; scalar r_1 = ::pow((x+r_0)*(x+r_0) + y*y ,0.5); scalar r_2 = ::pow((x-r_0)*(x-r_0) + y*y ,0.5); scalar V_theta1 = - gamma * r_1/(2.*pi*(r_c*r_c + r_1*r_1)); scalar V_theta2 = - gamma * r_2/(2.*pi*(r_c*r_c + r_2*r_2)); scalar Ux = -y * (V_theta1/r_1 + V_theta2/r_2); scalar Uy = (x-r_0) * V_theta1/r_1 + (x+r_0) * V_theta2/r_2; scalar Uz = 0.0; U[celli] = (Ux Uy Uz); } U.write(); Info << "\n end\n"; return(0); } -------------------------------------------------- -------------------------------------------------- tzntgq@cfdlem04:~/OpenFOAM/OpenFOAM-1.2.1/applications/utilities/preProcessing/corotVortex> wmake Making dependency list for source file corotVortex.C SOURCE_DIR=. SOURCE=corotVortex.C ; g++ -m64 -DlinuxAMD64 -Wall -W -Wno-unused-parameter -Wold-style-cast -march=opteron -O3 -ffast-math -DNoRepository -ftemplate-depth-30 -Wno-deprecated -I/home/tzntgq/OpenFOAM/OpenFOAM-1.2.1/src/cfdTools/compressible -I/home/tzntgq/OpenFOAM/OpenFOAM-1.2.1/src/cfdTools/general/lnInclude -I/home/tzntgq/OpenFOAM/OpenFOAM-1.2.1/src/OpenFOAM/lnInclude -IlnInclude -I. -fPIC -c $SOURCE -o Make/linuxAMD64Gcc4Opt/corotVortex.o corotVortex.C: In function 'int main(int, char**)': corotVortex.C:57: error: cannot resolve overloaded function 'x' based on conversion to type 'Foam::scalar' corotVortex.C:58: error: cannot resolve overloaded function 'y' based on conversion to type 'Foam::scalar' corotVortex.C:70: error: expected `)' before 'Uy' corotVortex.C:70: error: no match for 'operator=' in 'U.Foam::GeometricField<foam::vector,>::<anonymous >.Foam::Field<foam::vector>::< anonymous>.Foam::List<foam::vector<foam::scalar> >::<anonymous>.Foam::UList<t>::operator[] [with T = Foam::vector](celli) = Ux' /home/tzntgq/OpenFOAM/OpenFOAM-1.2.1/src/OpenFOAM/lnInclude/Vector.H:62: note: candidates are: Foam::Vector<foam::scalar>& Foam::Vector<foam::scalar>::operator=(const Foam::Vector<foam::scalar>&) corotVortex.C:67: warning: unused variable 'Uy' corotVortex.C:68: warning: unused variable 'Uz' make: *** [Make/linuxAMD64Gcc4Opt/corotVortex.o] Error 1 At compilation, x and y are not recognized and the vector field U is not understood... Could anyone give me a hint please ? |
|
March 21, 2006, 08:35 |
maybe try
forAll(mesh.cells(
|
#15 |
Member
Pierre Le Fur
Join Date: Mar 2009
Location: UK
Posts: 60
Rep Power: 17 |
maybe try
forAll(mesh.cells(), cellsI) scalar x = mesh.C()[cellI].component(0) rather than forAll(mesh.C(), celli)... Pierre |
|
March 21, 2006, 09:26 |
Thank you Pierre, it worked fo
|
#16 |
Member
Mélanie Piellard
Join Date: Mar 2009
Posts: 86
Rep Power: 17 |
Thank you Pierre, it worked for x and y with actually
forAll(mesh.cells(),cellI) scalar x = mesh.C()[cellI].component(0). Now I still have a problem with the velocity; I have defined Ux, Uy and Uz, and the line U[cellI] = (Ux, Uy, Uz); gives me the error message corotVortex.C:71: warning: left-hand operand of comma has no effect corotVortex.C:71: warning: right-hand operand of comma has no effect corotVortex.C:71: error: no match for 'operator=' in 'U.Foam::GeometricField<foam::vector,>::<anonymous >.Foam::Field<foam::vector>::< anonymous>.Foam::List<foam::vector<foam::scalar> >::<anonymous>.Foam::UList<t>::operator[] [with T = Foam::vector](cellI) = (((void)Ux, (void)Uy), Uz)' /home/tzntgq/OpenFOAM/OpenFOAM-1.2.1/src/OpenFOAM/lnInclude/Vector.H:62: note: candidates are: Foam::Vector<foam::scalar>& Foam::Vector<foam::scalar>::operator=(const Foam::Vector<foam::scalar>&) |
|
March 21, 2006, 09:55 |
try
U = vector(Ux, Uy, Uz);
|
#17 |
Member
Pierre Le Fur
Join Date: Mar 2009
Location: UK
Posts: 60
Rep Power: 17 |
try
U[cellI] = vector(Ux, Uy, Uz); Pierre |
|
March 21, 2006, 10:54 |
thank you Pierre, now everythi
|
#18 |
Member
Mélanie Piellard
Join Date: Mar 2009
Posts: 86
Rep Power: 17 |
thank you Pierre, now everything is working well !
mélanie |
|
March 26, 2006, 18:21 |
Inspired by this thread (and b
|
#19 |
Assistant Moderator
Bernhard Gschaider
Join Date: Mar 2009
Posts: 4,225
Rep Power: 51 |
Inspired by this thread (and because I wanted such a thing for myself for some time) I decided to visit two friends of the time of my diploma thesis (the compiler generators bison and flex) and write a utility that can set fields using complex expressions (from the command line or with a dictionary). A first version is available at
http://openfoamwiki.net/index.php/Contrib_funkySe tFields For instance the velocity field Melanie specified on the 20th: r = x^2 + y^2 U[x] = y * a/ r^2 U[y] = -x * b/ r^2 could be set with the utility with the call (assuming a and b to be 1 and 2): funkySetFields . theCase -field U -expression 'vector(pos().y*1/pow(mag(pos()),4),-pos().x*2/pow(mag(pos()),4),0)' -time 0 Another example would be setting the initial condition for the damBreak-tutorial: funkySetFields . damBreak -time 0 -field gamma -expression " pos().x <= 0.1461 && pos().y <= 0.292 ? 1 : 0" or (if you don't want to overwrite the whole gamma field): funkySetFields . damBreak -time 0 -field gamma -expression 1 -condition "pos().x <= 0.1461 && pos().y <= 0.292"
__________________
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 |
|
March 28, 2006, 06:54 |
Hi,
can someone please expl
|
#20 |
Member
Anja Stretz
Join Date: Mar 2009
Posts: 92
Rep Power: 17 |
Hi,
can someone please explain me, what the following line defines forAll(mesh.cells(),cellI) scalar x = mesh.C()[cellI].component(0) Thanks Anja |
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Specifying nonuniform boundary condition | maka | OpenFOAM Running, Solving & CFD | 59 | October 22, 2014 15:52 |
Nonuniform initial condition using cellSetDict | rinao | OpenFOAM Running, Solving & CFD | 6 | January 9, 2013 01:42 |
Initial Condition | Tang Kuei | FLUENT | 0 | May 17, 2006 20:54 |
Nonuniform gradient boundary condition | ankgupta8um | OpenFOAM Running, Solving & CFD | 1 | March 14, 2006 02:34 |
Nonuniform initial conditions | nico | OpenFOAM Pre-Processing | 2 | January 4, 2006 07:37 |