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

Error while compiling icoLagrangian Foam

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

Reply
 
LinkBack Thread Tools Display Modes
Old   November 28, 2008, 02:59
Default Hi I've tried to compile icoL
  #1
New Member
 
Sara Schairer
Join Date: Mar 2009
Posts: 26
Rep Power: 8
sara is on a distinguished road
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
sara is offline   Reply With Quote

Old   November 30, 2008, 11:02
Default Hi Sara! Please post your fil
  #2
Senior Member
 
Ivan Flaminio Cozza
Join Date: Mar 2009
Location: Torino, Piemonte, Italia
Posts: 207
Rep Power: 9
ivan_cozza is on a distinguished road
Send a message via MSN to ivan_cozza
Hi Sara!
Please post your files in the make directory, maybe there's the problem...
ivan_cozza is offline   Reply With Quote

Old   November 30, 2008, 21:02
Default Hi Ivan The files in the make
  #3
New Member
 
Sara Schairer
Join Date: Mar 2009
Posts: 26
Rep Power: 8
sara is on a distinguished road
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
sara is offline   Reply With Quote

Old   December 4, 2008, 02:21
Default Me again I just realized that
  #4
New Member
 
Sara Schairer
Join Date: Mar 2009
Posts: 26
Rep Power: 8
sara is on a distinguished road
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.
sara is offline   Reply With Quote

Old   December 4, 2008, 06:34
Default I have corrected the errors in
  #5
Member
 
florian
Join Date: Mar 2009
Location: Mannheim - Vincennes - Valenciennes, Deutchland - France
Posts: 34
Rep Power: 8
floooo is on a distinguished road
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.
floooo is offline   Reply With Quote

Old   December 4, 2008, 07:20
Default @ Florian: How can I set icoL
  #6
Senior Member
 
Ivan Flaminio Cozza
Join Date: Mar 2009
Location: Torino, Piemonte, Italia
Posts: 207
Rep Power: 9
ivan_cozza is on a distinguished road
Send a message via MSN to ivan_cozza
@ 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...
ivan_cozza is offline   Reply With Quote

Old   December 4, 2008, 08:03
Default Hi Ivan The density parame
  #7
Member
 
florian
Join Date: Mar 2009
Location: Mannheim - Vincennes - Valenciennes, Deutchland - France
Posts: 34
Rep Power: 8
floooo is on a distinguished road
Hi Ivan

The density parameter in the file cloudProperties means kg/m^3.
I think you have just to chose "density = 0".
floooo is offline   Reply With Quote

Old   December 4, 2008, 09:21
Default There actually has been a vers
  #8
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,912
Rep Power: 40
gschaider will become famous soon enoughgschaider will become famous soon enough
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
gschaider is offline   Reply With Quote

Old   December 4, 2008, 12:54
Default Florian, if I put density to
  #9
Senior Member
 
Ivan Flaminio Cozza
Join Date: Mar 2009
Location: Torino, Piemonte, Italia
Posts: 207
Rep Power: 9
ivan_cozza is on a distinguished road
Send a message via MSN to ivan_cozza
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...
ivan_cozza is offline   Reply With Quote

Old   December 5, 2008, 02:57
Default Hi Bernhard Thanks a lot, I m
  #10
New Member
 
Sara Schairer
Join Date: Mar 2009
Posts: 26
Rep Power: 8
sara is on a distinguished road
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
sara is offline   Reply With Quote

Old   December 5, 2008, 05:26
Default In this solver there is no int
  #11
Member
 
florian
Join Date: Mar 2009
Location: Mannheim - Vincennes - Valenciennes, Deutchland - France
Posts: 34
Rep Power: 8
floooo is on a distinguished road
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)
floooo is offline   Reply With Quote

Old   December 8, 2008, 03:11
Default Hi Florian Thanks for your an
  #12
New Member
 
Sara Schairer
Join Date: Mar 2009
Posts: 26
Rep Power: 8
sara is on a distinguished road
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
sara is offline   Reply With Quote

Old   December 8, 2008, 04:28
Default Hi, Sara In the code the im
  #13
Member
 
florian
Join Date: Mar 2009
Location: Mannheim - Vincennes - Valenciennes, Deutchland - France
Posts: 34
Rep Power: 8
floooo is on a distinguished road
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
floooo is offline   Reply With Quote

Old   December 8, 2008, 20:35
Default Hi Sara, I have modified i
  #14
Member
 
Andrew King
Join Date: Mar 2009
Location: Perth, Western Australia, Australia
Posts: 81
Rep Power: 8
andersking is on a distinguished road
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
andersking is offline   Reply With Quote

Old   December 8, 2008, 21:46
Default Hi Again, I attached the w
  #15
Member
 
Andrew King
Join Date: Mar 2009
Location: Perth, Western Australia, Australia
Posts: 81
Rep Power: 8
andersking is on a distinguished road
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
andersking is offline   Reply With Quote

Old   January 6, 2009, 16:37
Default hi, Andrew King : I tried to
  #16
Member
 
Sachin Kanetkar
Join Date: Mar 2009
Posts: 57
Rep Power: 8
sachin is on a distinguished road
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
sachin is offline   Reply With Quote

Old   January 7, 2009, 05:51
Default blockmesh has an influence onl
  #17
Member
 
florian
Join Date: Mar 2009
Location: Mannheim - Vincennes - Valenciennes, Deutchland - France
Posts: 34
Rep Power: 8
floooo is on a distinguished road
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.
floooo is offline   Reply With Quote

Old   January 12, 2009, 15:47
Default hi all, Thanks florian, I ha
  #18
Member
 
Sachin Kanetkar
Join Date: Mar 2009
Posts: 57
Rep Power: 8
sachin is on a distinguished road
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
sachin is offline   Reply With Quote

Old   January 12, 2009, 17:45
Default Hi Sachin! @1: that relax-s
  #19
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,912
Rep Power: 40
gschaider will become famous soon enoughgschaider will become famous soon enough
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
gschaider is offline   Reply With Quote

Old   January 13, 2009, 03:24
Default hi all, Thanks Bernhard I w
  #20
Member
 
Sachin Kanetkar
Join Date: Mar 2009
Posts: 57
Rep Power: 8
sachin is on a distinguished road
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
sachin 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
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 15:09
FOAM FATAL IO ERROR msrinath80 OpenFOAM Running, Solving & CFD 4 July 30, 2008 10:06
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 04:37


All times are GMT -4. The time now is 19:25.