|
[Sponsors] |
November 28, 2008, 02:59 |
Hi
I've tried to compile icoL
|
#1 |
New Member
Sara Schairer
Join Date: Mar 2009
Posts: 26
Rep Power: 17 |
Hi
I've tried to compile icoLagrangianFoam, but when I do wmake I get the following error message: schairer@schairer-desktop:~/OpenFOAM/schairer-.5/run_execute/IcoLagrangianFoam$ wmake icoLagrangianFoam Making dependency list for source file icoLagrangianFoam.C could not open file particle.H for source file icoLagrangianFoam.C Making dependency list for source file HardBallParticle.C could not open file particle.H for source file HardBallParticle.C Making dependency list for source file IncompressibleCloud.C could not open file particle.H for source file IncompressibleCloud.C SOURCE=icoLagrangianFoam.C ; g++ -m32 -Dlinux -DDP -Wall -Wno-strict-aliasing -Wextra -Wno-unused-parameter -Wold-style-cast -O3 -DNoRepository -ftemplate-depth-40 -I/home/schairer/OpenFOAM/OpenFOAM-1.5/src/cfdTools/incompressible -I/home/schairer/OpenFOAM/OpenFOAM-1.5/src/OpenFOAM/lnInclude -I/home/schairer/OpenFOAM/OpenFOAM-1.5/src/lagrangian/basic/lnInclude -I/home/schairer/OpenFOAM/OpenFOAM-1.5/src/cfdTools/general/lnInclude -I/home/schairer/OpenFOAM/OpenFOAM-1.5/src/finiteVolume/lnInclude -IlnInclude -I. -I/home/schairer/OpenFOAM/OpenFOAM-1.5/src/OpenFOAM/lnInclude -I/home/schairer/OpenFOAM/OpenFOAM-1.5/src/OSspecific/Unix/lnInclude -fPIC -pthread -c $SOURCE -o Make/linuxGccDPOpt/icoLagrangianFoam.o In file included from icoLagrangianFoam.C:43: HardBallParticle.H:40:22: error: particle.H: No such file or directory In file included from icoLagrangianFoam.C:43: HardBallParticle.H:56: error: expected template-name before '<' token HardBallParticle.H:56: error: expected `{' before '<' token HardBallParticle.H:56: error: expected unqualified-id before '<' token icoLagrangianFoam.C:126: error: expected `}' at end of input make: *** [Make/linuxGccDPOpt/icoLagrangianFoam.o] Error 1 The error message starts with complaining that the file particle.H isn't found. I can't find it either, it doesn't seem to be in the icoLagrangianFoam directory. I use OpenFoam 1.5 and downloaded icoLagrangianFoam using the link given in the openfoamWiki. Could someone please help me to solve this problem? Cheers, Sara |
|
November 30, 2008, 11:02 |
Hi Sara!
Please post your fil
|
#2 |
Senior Member
|
Hi Sara!
Please post your files in the make directory, maybe there's the problem... |
|
November 30, 2008, 21:02 |
Hi Ivan
The files in the make
|
#3 |
New Member
Sara Schairer
Join Date: Mar 2009
Posts: 26
Rep Power: 17 |
Hi Ivan
The files in the make directory look like this: Make/files icoLagrangianFoam.C HardBallParticle.C IncompressibleCloud.C EXE = $(FOAM_USER_APPBIN)/icoLagrangianFoam Make/Options EXE_INC = \ -I$(LIB_SRC)/cfdTools/incompressible \ -I$(LIB_SRC)/OpenFOAM/lnInclude \ -I$(LIB_SRC)/lagrangian/basic/lnInclude \ -I$(LIB_SRC)/cfdTools/general/lnInclude \ -I$(LIB_SRC)/finiteVolume/lnInclude EXE_LIBS = -lfiniteVolume \ -llagrangian Make/linucGccDPOpt/dependencies dependencies up to date Make/linucGccDPOpt/dependencyFiles DEPENDENCIES = \ icoLagrangianFoam.dep\ HardBallParticle.dep\ IncompressibleCloud.dep Make/linucGccDPOpt/dontIncludeDeps - empty file - Make/linucGccDPOpt/files # 1 "files" # 1 "<built-in>" # 1 "<command-line>" # 1 "files" icoLagrangianFoam.C HardBallParticle.C IncompressibleCloud.C EXE = $(FOAM_USER_APPBIN)/icoLagrangianFoam Make/linucGccDPOpt/filesMacros EXE = $(FOAM_USER_APPBIN)/icoLagrangianFoam Make/linucGccDPOpt/includeDeps - empty file - Make/linucGccDPOpt/localObjectFiles LOCAL_OBJECTS = \ icoLagrangianFoam.o\ HardBallParticle.o\ IncompressibleCloud.o Make/linucGccDPOpt/objectFiles OBJECTS = \ $(OBJECTS_DIR)/icoLagrangianFoam.o\ $(OBJECTS_DIR)/HardBallParticle.o\ $(OBJECTS_DIR)/IncompressibleCloud.o Make/linucGccDPOpt/options # 1 "options" # 1 "<built-in>" # 1 "<command-line>" # 1 "options" EXE_INC = -I$(LIB_SRC)/cfdTools/incompressible -I$(LIB_SRC)/OpenFOAM/lnInclude -I$(LIB_SRC)/lagrangian/basic/lnInclude -I$(LIB_SRC)/cfdTools/general/lnInclude -I$(LIB_SRC)/finiteVolume/lnInclude EXE_LIBS = -lfiniteVolume -llagrangian Make/linucGccDPOpt/sourceFiles SOURCE = \ icoLagrangianFoam.C\ HardBallParticle.C\ IncompressibleCloud.C Sorry for posting them all separately, I don't know how to do it all together. Thanks for looking at them. Sara |
|
December 4, 2008, 02:21 |
Me again
I just realized that
|
#4 |
New Member
Sara Schairer
Join Date: Mar 2009
Posts: 26
Rep Power: 17 |
Me again
I just realized that icoLagrangianFoam doesn't work with OpenFoam 1.5 which is the one I use. So that's probably the reason why it doesn't work for me. |
|
December 4, 2008, 06:34 |
I have corrected the errors in
|
#5 |
Member
florian
Join Date: Mar 2009
Location: Mannheim - Vincennes - Valenciennes, Deutchland - France
Posts: 34
Rep Power: 17 |
I have corrected the errors in order to use it on 1.5
http://www.file-upload.net/download-...m-1.5.zip.html The website upload does'nt work on my computer. I use this solver to create a rhoPorousSimpleLagrangianFoam which give the position of particule hiting a filter. I am actually trying to make a model allowing only small particles to go by, and increasing the wall porosity bit by bit along with the number of molecules clinging on it. It is very easy to understand what icoLagrangian does, but i have a lot of difficulties to modify it. |
|
December 4, 2008, 07:20 |
@ Florian:
How can I set icoL
|
#6 |
Senior Member
|
@ Florian:
How can I set icoLagrangianFoam to implement a massless particles model? In my application I just need a lagrangian tracking of particles that do not interact with nothing, but only carry with them a random number value... |
|
December 4, 2008, 08:03 |
Hi Ivan
The density parame
|
#7 |
Member
florian
Join Date: Mar 2009
Location: Mannheim - Vincennes - Valenciennes, Deutchland - France
Posts: 34
Rep Power: 17 |
Hi Ivan
The density parameter in the file cloudProperties means kg/m^3. I think you have just to chose "density = 0". |
|
December 4, 2008, 09:21 |
There actually has been a vers
|
#8 |
Assistant Moderator
Bernhard Gschaider
Join Date: Mar 2009
Posts: 4,225
Rep Power: 51 |
There actually has been a version of icoLagrangianFoam that is working with 1.5 in the SVN, I just never announced it and didn't update the Wiki-page (which I now did)
Nevertheless: be aware that the type of particles used in this solver does not reflect the state-of-the-art in 1.5. For that have look at the particle solvers that can be found in $FOAM_TUTORIALS or the demo-solver Hakan published here http://openfoamwiki.net/index.php/Co...idParticleFoam 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 |
|
December 4, 2008, 12:54 |
Florian,
if I put density to
|
#9 |
Senior Member
|
Florian,
if I put density to 0, are there any other interactions between the particles? Because I need just a lagrangian tracking without any interactions, I want that my particles only travel on the streamlines... |
|
December 5, 2008, 02:57 |
Hi Bernhard
Thanks a lot, I m
|
#10 |
New Member
Sara Schairer
Join Date: Mar 2009
Posts: 26
Rep Power: 17 |
Hi Bernhard
Thanks a lot, I managed to compile icoLagrangianFoam now. I've tried to work it out but I'm kind of stuck: could you please explain what the expressions in "injection" are? thres center vel0 vel1 d0 d1 tStart tEnd I guess center is the place where the particles are injected, d is the diameter and tStart to tEnd the period over which particles are injected. vel1 is the velocity. But what is vel0 since it's a scalar? And what are r0 and thres? Would be nice if you could give me a short explanation. Thanks, Sara |
|
December 5, 2008, 05:26 |
In this solver there is no int
|
#11 |
Member
florian
Join Date: Mar 2009
Location: Mannheim - Vincennes - Valenciennes, Deutchland - France
Posts: 34
Rep Power: 17 |
In this solver there is no interaction between the particles
Massless particles will follow exatly the stream's lines. thres (i think particule injection by step) center (center of the sphere of injection) r0 (radius of the sphere of injection) vel0, vel1 (in the solver vel=tmp*vel1+vel0 with tmp a vector) vel0 is vmin d0, d1 (in the solver d=random*d1+d0) d0 is the dmin tStart (start time of injection) tEnd (start end of injection) |
|
December 8, 2008, 03:11 |
Hi Florian
Thanks for your an
|
#12 |
New Member
Sara Schairer
Join Date: Mar 2009
Posts: 26
Rep Power: 17 |
Hi Florian
Thanks for your answer. Your explanations concerning vel0, vel1, d0, d1, tStart and tEnd sound good to me. However I don't think that thres can be the number of particles injected per time step. Thres is set to 0.2 in the cavity example. And however I change it in my file, the number of particles stays the same. What do you mean by "shpere of injection"? That the particles are injected forming a sphere? Anyway, it doesn't work for me. Sometimes when I change r0 from 0 to nonzero there's no particle injected ( but there was when r0 was 0). I'm really confused about this. Has anyone some experience with this solver and can give me a hint what I'm missing here? Cheers, Sara |
|
December 8, 2008, 04:28 |
Hi, Sara
In the code the im
|
#13 |
Member
florian
Join Date: Mar 2009
Location: Mannheim - Vincennes - Valenciennes, Deutchland - France
Posts: 34
Rep Power: 17 |
Hi, Sara
In the code the implementation is : pos = td.consProps().center_+tmp*td.constProps().ro_ tmp = (random().vect01()-vect(0.5,0.5,0.5))*2 In a easier langage the position of the particule is : pos = center + (a random vector) * ro Are you sure that the sphere is completely include in your mesh. thres appears just before scalar prop=random().scalar01(); if(prop<td.constProps().thres_) { (..) addparticule(ptr); } I think thres=1 mean injection each step thres=0.2 means that the probability of injection during a step is 20%. Florian |
|
December 8, 2008, 20:35 |
Hi Sara,
I have modified i
|
#14 |
Member
Andrew King
Join Date: Mar 2009
Location: Perth, Western Australia, Australia
Posts: 82
Rep Power: 17 |
Hi Sara,
I have modified icoLagrangianFoam previously to inject a number of particles in each time step (I think by default it only injects one). I have attached two modified files (hopefully they still are compatible) you will need to add a line "nParts 10;" to the injection section of the cloudProperties dictionary, and a recompile is required of course. IncompressibleCloud.H IncompressibleCloud.C Also, florian is correct with the threshold. If you set thresh to 1, you'll get nParts every step. Otherwise you may not always get a particle injected. I hope this helps. Cheers, Andrew
__________________
Dr Andrew King Fluid Dynamics Research Group Curtin University |
|
December 8, 2008, 21:46 |
Hi Again,
I attached the w
|
#15 |
Member
Andrew King
Join Date: Mar 2009
Location: Perth, Western Australia, Australia
Posts: 82
Rep Power: 17 |
Hi Again,
I attached the wrong files. (They're for 1.4.1). Here are the correct files. HardBallParticle.H HardBallParticle.C IncompressibleCloud.C Cheers, Andrew
__________________
Dr Andrew King Fluid Dynamics Research Group Curtin University |
|
January 6, 2009, 16:37 |
hi,
Andrew King : I tried to
|
#16 |
Member
Sachin Kanetkar
Join Date: Mar 2009
Posts: 57
Rep Power: 17 |
hi,
Andrew King : I tried to put these files for OpenFOAM1.5 in icoLagrangianFoam but there were some failures related to density (which is because in icoLagrangianFoam density was defined in HardBallparticle class whereas in these files it is done in constantProperties class) also there was failure of constProp function (which is not at all defined in icoLagrangianFoam). I tried to modify but my C++ knowledge is very limited as when i solved these problems something else started failing? Please help me out? thanks florian about thres and sphere of injection ,I was searching for it. there is still one question regarding these dimensions... blockMeshdict we provide a multiplying factor on top 'converttoMetres' the dimesions given for injection are the absolute values in metres(dimesion of domain per say)or even these dimension will be multiplied by the factor mentioned in blockmeshdict thanks in advance sachin |
|
January 7, 2009, 05:51 |
blockmesh has an influence onl
|
#17 |
Member
florian
Join Date: Mar 2009
Location: Mannheim - Vincennes - Valenciennes, Deutchland - France
Posts: 34
Rep Power: 17 |
blockmesh has an influence only on mesh files during the mesh generation (file contain in Constant/polymesh).
You must specify initial value (velocity.. ) in the defauts units. |
|
January 12, 2009, 15:47 |
hi all,
Thanks florian,
I ha
|
#18 |
Member
Sachin Kanetkar
Join Date: Mar 2009
Posts: 57
Rep Power: 17 |
hi all,
Thanks florian, I have 2 more questions 1. I wanted to know the actual equation (if anyone can provide me some ref document it would be helpful) we are solving in the term relax, coeff in hardBallParticle from icoLagrangianFoam , so that i can understand whether i need to add few more terms in that calculation. 2. where and how are we calculating smoment_ thanks in advance sachin |
|
January 12, 2009, 17:45 |
Hi Sachin!
@1: that relax-s
|
#19 |
Assistant Moderator
Bernhard Gschaider
Join Date: Mar 2009
Posts: 4,225
Rep Power: 51 |
Hi Sachin!
@1: that relax-stuff is just a reformulation of the naive U_new = U_old+dt * dragForce/m (explicit Euler) in a way that makes sure that U_new will not exceed the gas-velocity for too large deltaT @2: That is just the momentum source for the gas (which is the negative sum of the momentum changes all the particles are seeing) 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 |
|
January 13, 2009, 03:24 |
hi all,
Thanks Bernhard
I w
|
#20 |
Member
Sachin Kanetkar
Join Date: Mar 2009
Posts: 57
Rep Power: 17 |
hi all,
Thanks Bernhard I would like to add thermal effect for drag force calculation and eventually to the momentum change in particle....so would like to know where are the calculation for smoment_ is done so that i can add these term...smoment_ is actually defined just above tsource calculation where it is used then where are the calculations for smoment_ done thanks in advance sachin |
|
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Errors when Compiling UDF: error C2040/error C2099 | Julian K. | FLUENT | 1 | December 21, 2008 01:23 |
Compiling MRFSimple foam error | mrangitschdowcom | OpenFOAM Installation | 0 | September 15, 2008 16:09 |
FOAM FATAL IO ERROR | msrinath80 | OpenFOAM Running, Solving & CFD | 4 | July 30, 2008 11:06 |
Adding collision to icoLagrangian foam | alan_fergus | OpenFOAM Running, Solving & CFD | 0 | December 12, 2006 08:55 |
FOAM FATAL IO ERROR | sita | OpenFOAM Running, Solving & CFD | 2 | August 23, 2005 05:37 |