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

Multiphase Solid Particle Tracking

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

Reply
 
LinkBack Thread Tools Display Modes
Old   May 7, 2013, 10:05
Post Multiphase Solid Particle Tracking
  #1
New Member
 
alexlupo's Avatar
 
Alejandro López
Join Date: Mar 2013
Location: Glasgow
Posts: 11
Rep Power: 3
alexlupo is on a distinguished road
Hi,

After some time trying I finally compiled a new solver for particle tracking in interFoam and set up a case but when I try to run the case it seems that, at some point, it gets stuck in an infinite loop. I tracked in the .C file where the problem is and it shows that it is in the piece of code particles.move(g); and in the second iteration. The first iteration runs ok.
Any suggestions would be appreciated!
Thanks a lot in advance!

Alex
alexlupo is offline   Reply With Quote

Old   May 7, 2013, 11:27
Default Solved
  #2
New Member
 
alexlupo's Avatar
 
Alejandro López
Join Date: Mar 2013
Location: Glasgow
Posts: 11
Rep Power: 3
alexlupo is on a distinguished road
Hi again!
I just solved the issue. It didn't get through the second iteration because tetFaceI and tetPtI were not properly initialised!
Cheers anyway!
P.S.:If someone wants to discuss such a solver in order to improve it, comments are welcome!!
alexlupo is offline   Reply With Quote

Old   September 6, 2013, 14:47
Default
  #3
Member
 
Ovie Doro
Join Date: Jul 2009
Posts: 97
Rep Power: 7
ovie is on a distinguished road
Quote:
Originally Posted by alexlupo View Post
Hi again!
I just solved the issue. It didn't get through the second iteration because tetFaceI and tetPtI were not properly initialised!
Cheers anyway!
P.S.:If someone wants to discuss such a solver in order to improve it, comments are welcome!!
Hi:

I am trying to combine interFoam with lagrangian particle tracking (2 or 4 way coupling). Could you please share some insight into how you developed your solver? Have you been able to validate results from the solver?

Thanks.
ovie is offline   Reply With Quote

Old   September 6, 2013, 16:26
Default
  #4
New Member
 
alexlupo's Avatar
 
Alejandro López
Join Date: Mar 2013
Location: Glasgow
Posts: 11
Rep Power: 3
alexlupo is on a distinguished road
Quote:
Originally Posted by ovie View Post
Hi:

I am trying to combine interFoam with lagrangian particle tracking (2 or 4 way coupling). Could you please share some insight into how you developed your solver? Have you been able to validate results from the solver?

Thanks.
Hi there!
I havent been able to validate because I am working now on the same kind of solver but with pimpleFoam.
Anyway, as a starting point, there is a very good tutorial on how to couple both interFoam and the solidParticle class:
http://www.tfd.chalmers.se/~hani/kur...LPT_120911.pdf
The tutorial is for a previous version of OpenFoam so you will have to upgrade it in case you are using 2.2.x.
Take a look and just let me know if you need some help. I will be glad to help you.
Cheers,
__________________
Alex
alexlupo is offline   Reply With Quote

Old   September 6, 2013, 18:33
Default
  #5
Member
 
Ovie Doro
Join Date: Jul 2009
Posts: 97
Rep Power: 7
ovie is on a distinguished road
Quote:
Originally Posted by alexlupo View Post
Hi there!
I havent been able to validate because I am working now on the same kind of solver but with pimpleFoam.
Anyway, as a starting point, there is a very good tutorial on how to couple both interFoam and the solidParticle class:
http://www.tfd.chalmers.se/~hani/kur...LPT_120911.pdf
The tutorial is for a previous version of OpenFoam so you will have to upgrade it in case you are using 2.2.x.
Take a look and just let me know if you need some help. I will be glad to help you.
Cheers,
Hi:

Thanks for the information. I actually have a copy of the Chalmers slides with me and I have been using it as guide to develop my solver. And yes, the tutorial in the pdf is for an older OF version. But I think the new Lagrangian implementation makes it easier to do particle tracking in an existing fluid solver.

My main worry is how to deal with issues relating to particles migrating from one phase (say liquid) into another. I have not run any such simulations so I dont know if this is something that is likely to occur in the first place. I was just wondering if this is something you have thought of as well and could provide some ideas on how to design the solver to prevent such migration.

Thanks for sharing your thoughts.
ovie is offline   Reply With Quote

Old   September 7, 2013, 15:10
Question
  #6
New Member
 
alexlupo's Avatar
 
Alejandro López
Join Date: Mar 2013
Location: Glasgow
Posts: 11
Rep Power: 3
alexlupo is on a distinguished road
Quote:
Originally Posted by ovie View Post
Hi:

Thanks for the information. I actually have a copy of the Chalmers slides with me and I have been using it as guide to develop my solver. And yes, the tutorial in the pdf is for an older OF version. But I think the new Lagrangian implementation makes it easier to do particle tracking in an existing fluid solver.

My main worry is how to deal with issues relating to particles migrating from one phase (say liquid) into another. I have not run any such simulations so I dont know if this is something that is likely to occur in the first place. I was just wondering if this is something you have thought of as well and could provide some ideas on how to design the solver to prevent such migration.

Thanks for sharing your thoughts.
I am not sure if I understood your question properly, but the solidParticle class should not give any problems relating phase migration. The issues you can experience (and by the way that I am experiencing) are related to the particles going out of the boundaries, thus showing unexpected behavior, or simulations crashing in parallel due to the injection of particles in more than one processor boundary.
If your question is related to particles moving from one phase to another, I guess that could eventually happen, but from my point of view that could also have a physical explanation, taking into account the difference of density between both particles and fluids.
I guess if both phases are clearly separated, you could just create a boundary in between so that you would not allow the particles to move from phase to the other.
Let me know if this was what you intend to do and if not, could you explain it further?
Cheers,
__________________
Alex
alexlupo is offline   Reply With Quote

Old   September 10, 2013, 05:49
Default
  #7
New Member
 
Sebastian W.
Join Date: Nov 2012
Posts: 11
Rep Power: 3
nero235 is on a distinguished road
Send a message via ICQ to nero235
Quote:
Originally Posted by alexlupo View Post
Hi again!
I just solved the issue. It didn't get through the second iteration because tetFaceI and tetPtI were not properly initialised!
Cheers anyway!
P.S.:If someone wants to discuss such a solver in order to improve it, comments are welcome!!
Hello alexlupo,

how did you define these two variables: tetFaceI, tetPtI? I am stuck right here, because the tutorial from Aurelia Vallier doesn't include how to define these two. My inject function looks like this right now:

Code:
void Foam::solidParticleCloud::inject(solidParticle::trackingData &td)
{
    label cellI=mesh_.findCell(td.spc().posP1_);        // primitiveMesh::findCell()
    //label tetFaceI=mesh_.findCellFacePt(td.spc().posP1_, ?);
    //label tetPtI=mesh_.findCellFacePt(td.spc().posP1_, ? );
    label tetPtI=mesh_.findCellFacePt(td.spc().posP1_,cellI,tetFaceI,tetPtI);

    solidParticle* ptr1=new solidParticle(*this,td.spc().posP1_,cellI,tetFaceI,tetPtI,td.spc().dP1_,td.spc().UP1_);
    Cloud<solidParticle>::addParticle(ptr1);

    label cellI=mesh_.findCell(td.spc().posP2_);        // primitiveMesh::findCell()
    //label tetFaceI=mesh_.findCellFacePt(td.spc().posP2_, ? );
    //label tetPtI=mesh_.findCellFacePt(td.spc().posP2_, ? );
    label tetPtI=mesh_.findCellFacePt(td.spc().posP2_,cellI,tetFaceI,tetPtI);

    solidParticle* ptr2=new solidParticle(*this,td.spc().posP2_,cellI,tetFaceI,tetPtI,td.spc().dP2_,td.spc().UP2_);
    Cloud<solidParticle>::addParticle(ptr2);
}
I would be glad for some insight on how to define:
Code:
label tetFaceI
and
Code:
label tetPtI
Thanks for your help!

Greetings, Sebastian.
nero235 is offline   Reply With Quote

Old   September 11, 2013, 13:00
Default
  #8
New Member
 
alexlupo's Avatar
 
Alejandro López
Join Date: Mar 2013
Location: Glasgow
Posts: 11
Rep Power: 3
alexlupo is on a distinguished road
Hello Sebastian,

First of all, what you do with that first part of the code, if I remember well, is to tell OpenFoam to search for the cell, the tetFaceI and the tetPtI in the position of the point you defined you injector is going to be.
If you look in Doxygen for findCellFacePt you will get a definition of what I just said.
So, basically this function
Code:
mesh_.findCellFacePt()
takes a point as an argument and it returns three labels, which will be the cell, the tetFaceI and the tetPtI.
For this to work properly, it is better to initialize first those variables you are going to use and then just write them inside the function so that the values that it returns are stored in those variables you created. For example:
Code:
label cellI=1; 
label tetFaceI=1; 
label tetPtI=1; 
mesh_.findCellFacePt(td.cloud().posP1_, cellI, tetFaceI, tetPtI);
Now the values in those cellI tetFaceI and tetPtI are the ones you need to inject the particles at the point you defined.
Finally, for the code to work properly (if you are using newer versions of OpenFOAM than the one Aurelia used) you should change the
Code:
 td.spc().
for
Code:
td.cloud().
because that spc will not be recognized in the new code.
Hope this helps you!
Cheers,
Alex

Quote:
Originally Posted by nero235 View Post
Hello alexlupo,

how did you define these two variables: tetFaceI, tetPtI? I am stuck right here, because the tutorial from Aurelia Vallier doesn't include how to define these two. My inject function looks like this right now:

Code:
void Foam::solidParticleCloud::inject(solidParticle::trackingData &td)
{
    label cellI=mesh_.findCell(td.spc().posP1_);        // primitiveMesh::findCell()
    //label tetFaceI=mesh_.findCellFacePt(td.spc().posP1_, ?);
    //label tetPtI=mesh_.findCellFacePt(td.spc().posP1_, ? );
    label tetPtI=mesh_.findCellFacePt(td.spc().posP1_,cellI,tetFaceI,tetPtI);

    solidParticle* ptr1=new solidParticle(*this,td.spc().posP1_,cellI,tetFaceI,tetPtI,td.spc().dP1_,td.spc().UP1_);
    Cloud<solidParticle>::addParticle(ptr1);

    label cellI=mesh_.findCell(td.spc().posP2_);        // primitiveMesh::findCell()
    //label tetFaceI=mesh_.findCellFacePt(td.spc().posP2_, ? );
    //label tetPtI=mesh_.findCellFacePt(td.spc().posP2_, ? );
    label tetPtI=mesh_.findCellFacePt(td.spc().posP2_,cellI,tetFaceI,tetPtI);

    solidParticle* ptr2=new solidParticle(*this,td.spc().posP2_,cellI,tetFaceI,tetPtI,td.spc().dP2_,td.spc().UP2_);
    Cloud<solidParticle>::addParticle(ptr2);
}
I would be glad for some insight on how to define:
Code:
label tetFaceI
and
Code:
label tetPtI
Thanks for your help!

Greetings, Sebastian.
__________________
Alex
alexlupo is offline   Reply With Quote

Old   September 16, 2013, 11:16
Default
  #9
New Member
 
Sebastian W.
Join Date: Nov 2012
Posts: 11
Rep Power: 3
nero235 is on a distinguished road
Send a message via ICQ to nero235
Quote:
Originally Posted by alexlupo View Post
Hello Sebastian,

First of all, what you do with that first part of the code, if I remember well, is to tell OpenFoam to search for the cell, the tetFaceI and the tetPtI in the position of the point you defined you injector is going to be.
If you look in Doxygen for findCellFacePt you will get a definition of what I just said.
So, basically this function
Code:
mesh_.findCellFacePt()
takes a point as an argument and it returns three labels, which will be the cell, the tetFaceI and the tetPtI.
For this to work properly, it is better to initialize first those variables you are going to use and then just write them inside the function so that the values that it returns are stored in those variables you created. For example:
Code:
label cellI=1; 
label tetFaceI=1; 
label tetPtI=1; 
mesh_.findCellFacePt(td.cloud().posP1_, cellI, tetFaceI, tetPtI);
Now the values in those cellI tetFaceI and tetPtI are the ones you need to inject the particles at the point you defined.
Finally, for the code to work properly (if you are using newer versions of OpenFOAM than the one Aurelia used) you should change the
Code:
 td.spc().
for
Code:
td.cloud().
because that spc will not be recognized in the new code.
Hope this helps you!
Cheers,
Alex
Hello Alex,

thank you for your help! I will try this as soon I have some time for it . However I found another way to couple interfoam with a lagrangian particle tracking method, which is by including swak4Foam libraries into your controlDict.

Thanks for the help!

Greetings, Sebastian
nero235 is offline   Reply With Quote

Old   March 3, 2014, 10:22
Default
  #10
New Member
 
Stefan Wenzel
Join Date: Mar 2013
Posts: 3
Rep Power: 3
scram is on a distinguished road
Hallo Foamers,

Does anyone know the coupling algorithm of "LPTtoVOF.H" by Vallier form this presentation:

http://www.tfd.chalmers.se/~hani/kurser/OS_CFD_2011/OF_kurs_LPT_120911.pdf

or has an idea where to find it? I can't find any publication on this

thank you
Stefan
scram is offline   Reply With Quote

Old   March 3, 2014, 10:55
Default
  #11
New Member
 
Sebastian W.
Join Date: Nov 2012
Posts: 11
Rep Power: 3
nero235 is on a distinguished road
Send a message via ICQ to nero235
Quote:
Originally Posted by scram View Post
Hallo Foamers,

Does anyone know the coupling algorithm of "LPTtoVOF.H" by Vallier form this presentation:

http://www.tfd.chalmers.se/~hani/kurser/OS_CFD_2011/OF_kurs_LPT_120911.pdf

or has an idea where to find it? I can't find any publication on this

thank you
Stefan

Hello Stefan,

I am not sure if the any code was published but Ms. Vallier, but she describes in the presentation pretty good on how to couple LPT methods with interFoam. I tried it myself until I found a better solution. Also the tutorial uses a very old OpenFOAM version (1.6.x or 1.7.x). Therefor the coupling is different when using 2.3.x for example. A better way to integrate LPT into any OpenFOAM solver is by using swak4Foam.

Hope this helps.

Sebastian
nero235 is offline   Reply With Quote

Old   March 4, 2014, 03:51
Default
  #12
New Member
 
Stefan Wenzel
Join Date: Mar 2013
Posts: 3
Rep Power: 3
scram is on a distinguished road
Quote:
Originally Posted by nero235 View Post
Hello Stefan,

I am not sure if the any code was published but Ms. Vallier, but she describes in the presentation pretty good on how to couple LPT methods with interFoam. I tried it myself until I found a better solution. Also the tutorial uses a very old OpenFOAM version (1.6.x or 1.7.x). Therefor the coupling is different when using 2.3.x for example. A better way to integrate LPT into any OpenFOAM solver is by using swak4Foam.

Hope this helps.

Sebastian

Hello Sebastian,

thanks for the reply. i absolutly agree with you. She discribed the including of the "solidParticle" lib very good, and the solver is runnig (by the way, your upper hints where very helpful, thank you for that!). But i guess the key algorithm, which switches from LPT to VOF is implemented in this "LPTtoVOF.H" and not discribed in the presentation. Is swak4Foam able to remove lagrangian particles and add there mass/momentum/volume to the alpha fraction of the VOF methode?
scram is offline   Reply With Quote

Old   March 4, 2014, 09:07
Default
  #13
New Member
 
Sebastian W.
Join Date: Nov 2012
Posts: 11
Rep Power: 3
nero235 is on a distinguished road
Send a message via ICQ to nero235
Quote:
Originally Posted by scram View Post
Hello Sebastian,

thanks for the reply. i absolutly agree with you. She discribed the including of the "solidParticle" lib very good, and the solver is runnig (by the way, your upper hints where very helpful, thank you for that!). But i guess the key algorithm, which switches from LPT to VOF is implemented in this "LPTtoVOF.H" and not discribed in the presentation. Is swak4Foam able to remove lagrangian particles and add there mass/momentum/volume to the alpha fraction of the VOF methode?
Ok, what she does in "LPT to VOF" is that she injects a solid particle into the multiphase flow. To do that she couples the solver interFoam (VOF) with the solidParticle (Lagrange) library. This method is really handy and it has also a physical background. However this coupling can be done with swak4Foam also, without creating a new solver. Then she describes the different interaction types (1-way, 2-way, 4-way) and how to implement them into the LPTinterFoam.

However in this "LPTtoVOF" method she describes the modeling of a solid particle (Lagrange) which as soon it hits the phase interface becomes another fluid phase (VOF). This is physical non-sense however. Do you really need this feature? Normally a solid particle falling into a fluid interacts with the interface (creating waves resulting from the kinetic energy of the impact), it stays however solid.

What is your physical setup you want to simulate?
nero235 is offline   Reply With Quote

Old   March 5, 2014, 03:36
Default
  #14
New Member
 
Stefan Wenzel
Join Date: Mar 2013
Posts: 3
Rep Power: 3
scram is on a distinguished road
I'm trying to simulate breakup (atomization) and coalescence in small scales by using such a coupling of VOF and LPT in OF. Tomar et al. had already done implementaions like this in other codes:

3. Video (Lagrangian Particle Atomization Simulation - 5 Mbytes, click on image to view movie)

http://www.lmm.jussieu.fr/~zaleski/zaleski.html

> Link to "Animations"

correlated paper:

http://www.lmm.jussieu.fr/~zaleski/Papers/tomar-CAF.pdf

as a first step for this, i thought i just try Ms Valliers way to switch from LPT to VOF near the surface. That's why i'm searching for her algorithm in LTPtoVOF.H
scram is offline   Reply With Quote

Old   March 22, 2014, 06:22
Default
  #15
New Member
 
Will Chen
Join Date: Mar 2013
Posts: 1
Rep Power: 0
willchennewcastle is on a distinguished road
Quote:
Originally Posted by nero235 View Post
Ok, what she does in "LPT to VOF" is that she injects a solid particle into the multiphase flow. To do that she couples the solver interFoam (VOF) with the solidParticle (Lagrange) library. This method is really handy and it has also a physical background. However this coupling can be done with swak4Foam also, without creating a new solver. Then she describes the different interaction types (1-way, 2-way, 4-way) and how to implement them into the LPTinterFoam.

However in this "LPTtoVOF" method she describes the modeling of a solid particle (Lagrange) which as soon it hits the phase interface becomes another fluid phase (VOF). This is physical non-sense however. Do you really need this feature? Normally a solid particle falling into a fluid interacts with the interface (creating waves resulting from the kinetic energy of the impact), it stays however solid.

What is your physical setup you want to simulate?
It's certainly interesting about how to implement the Parcels in interFoam through SWAK. Could you please just share some thoughts on the procedure? My assumption is to use interFoam with swak4foam to set lagrangian particle field.
willchennewcastle is offline   Reply With Quote

Old   March 26, 2014, 04:44
Default
  #16
New Member
 
Mahdi S
Join Date: Jul 2012
Posts: 12
Rep Power: 4
Mahdi2010 is on a distinguished road
Actually you are right, as the solid particle impinges the fluid interface it
will cause splash and the physical change makes no sense. But, just imagine the
solid particles as representative particles. They are used only as some imaginary
data holder. you can add them and remove them whenever you need a continuous phase.
Also I agree with Stefan that the LPTtoVOF.H is not presented in her document and it is a key
part.
Mahdi2010 is offline   Reply With Quote

Old   April 23, 2014, 08:07
Default
  #17
New Member
 
houwy
Join Date: Nov 2013
Posts: 19
Rep Power: 2
houwy is on a distinguished road
Quote:
Originally Posted by alexlupo View Post
Hi there!
I havent been able to validate because I am working now on the same kind of solver but with pimpleFoam.
Anyway, as a starting point, there is a very good tutorial on how to couple both interFoam and the solidParticle class:
http://www.tfd.chalmers.se/~hani/kur...LPT_120911.pdf
The tutorial is for a previous version of OpenFoam so you will have to upgrade it in case you are using 2.2.x.
Take a look and just let me know if you need some help. I will be glad to help you.
Cheers,
I'm sorry to trouble you. I have coupled the inerFoam and solidParticleFoam in of2.2.0. But there are some problems when I add a particle injector. Can you tell me how to upgrade it.
houwy is offline   Reply With Quote

Old   April 23, 2014, 08:11
Default
  #18
New Member
 
houwy
Join Date: Nov 2013
Posts: 19
Rep Power: 2
houwy is on a distinguished road
Quote:
Originally Posted by scram View Post
I'm trying to simulate breakup (atomization) and coalescence in small scales by using such a coupling of VOF and LPT in OF. Tomar et al. had already done implementaions like this in other codes:

3. Video (Lagrangian Particle Atomization Simulation - 5 Mbytes, click on image to view movie)

http://www.lmm.jussieu.fr/~zaleski/zaleski.html

> Link to "Animations"

correlated paper:

http://www.lmm.jussieu.fr/~zaleski/Papers/tomar-CAF.pdf

as a first step for this, i thought i just try Ms Valliers way to switch from LPT to VOF near the surface. That's why i'm searching for her algorithm in LTPtoVOF.H
Hi! Have you success to couple interfoam with solidParticle using Aurelia Vallier's method? I have some problem to do it on OF2.2.0. Can you give me some help?
houwy is offline   Reply With Quote

Old   April 24, 2014, 01:19
Default
  #19
New Member
 
Mahdi S
Join Date: Jul 2012
Posts: 12
Rep Power: 4
Mahdi2010 is on a distinguished road
Quote:
Originally Posted by houwy View Post
Hi! Have you success to couple interfoam with solidParticle using Aurelia Vallier's method? I have some problem to do it on OF2.2.0. Can you give me some help?
Please tell us more about your problem.
Mahdi2010 is offline   Reply With Quote

Old   April 24, 2014, 02:41
Default
  #20
New Member
 
houwy
Join Date: Nov 2013
Posts: 19
Rep Power: 2
houwy is on a distinguished road
Quote:
Originally Posted by alexlupo View Post
Hello Sebastian,

First of all, what you do with that first part of the code, if I remember well, is to tell OpenFoam to search for the cell, the tetFaceI and the tetPtI in the position of the point you defined you injector is going to be.
If you look in Doxygen for findCellFacePt you will get a definition of what I just said.
So, basically this function
Code:
mesh_.findCellFacePt()
takes a point as an argument and it returns three labels, which will be the cell, the tetFaceI and the tetPtI.
For this to work properly, it is better to initialize first those variables you are going to use and then just write them inside the function so that the values that it returns are stored in those variables you created. For example:
Code:
label cellI=1; 
label tetFaceI=1; 
label tetPtI=1; 
mesh_.findCellFacePt(td.cloud().posP1_, cellI, tetFaceI, tetPtI);
Now the values in those cellI tetFaceI and tetPtI are the ones you need to inject the particles at the point you defined.
Finally, for the code to work properly (if you are using newer versions of OpenFOAM than the one Aurelia used) you should change the
Code:
 td.spc().
for
Code:
td.cloud().
because that spc will not be recognized in the new code.
Hope this helps you!
Cheers,
Alex
Hi! I still have some problem with it.
code:

Code:
void Foam::solidParticleCloud::inject(solidParticle::trackingData &td)
{
  label cellI = 1;
  label tetFaceI = 1;
  label tetPtI = 1;
  mesh_.findCellFacePt(td.cloud().posP1_, cellI, tetFaceI, tetPtI);
  solidParticle* ptr1=new solidParticle(*this,td.cloud().posP1_,cellI,tetFaceI, tetPtI,
  td.cloud().dP1_,td.cloud().UP1_);
  Cloud<solidParticle>::addParticle(ptr1);
  mesh_.findCellFacePt(td.cloud().posP1_, cellI, tetFaceI, tetPtI);
  solidParticle* ptr2=new solidParticle(*this,td.cloud().posP2_,cellI,tetFaceI, tetPtI,
  td.cloud().dP2_,td.cloud().UP2_);
  Cloud<solidParticle>::addParticle(ptr2);
}


when I compile it , There are still some errors.


Code:
solidParticleCloud.C: In member function ‘void Foam::solidParticleCloud::inject(Foam::solidParticle::trackingData&)’:
solidParticleCloud.C:81:34: error: no matching function for call to ‘Foam::solidParticle::solidParticle(Foam::solidParticleCloud&, Foam::vector&, Foam::label&, Foam::label&, Foam::label&, Foam::scalar&, Foam::vector&)’
solidParticleCloud.C:81:34: note: candidates are:
solidParticle.H:135:9: note: Foam::solidParticle::solidParticle(const Foam::polyMesh&, Foam::Istream&, bool)
solidParticle.H:135:9: note:   candidate expects 3 arguments, 7 provided
solidParticleI.H:47:8: note: Foam::solidParticle::solidParticle(const Foam::polyMesh&, const vector&, Foam::label, Foam::label, Foam::label, Foam::scalar, const vector&)
solidParticleI.H:47:8: note:   no known conversion for argument 1 from ‘Foam::solidParticleCloud’ to ‘const Foam::polyMesh&’
solidParticle.H:58:7: note: Foam::solidParticle::solidParticle(const Foam::solidParticle&)
solidParticle.H:58:7: note:   candidate expects 1 argument, 7 provided
solidParticleCloud.C:85:34: error: no matching function for call to ‘Foam::solidParticle::solidParticle(Foam::solidParticleCloud&, Foam::vector&, Foam::label&, Foam::label&, Foam::label&, Foam::scalar&, Foam::vector&)’
solidParticleCloud.C:85:34: note: candidates are:
solidParticle.H:135:9: note: Foam::solidParticle::solidParticle(const Foam::polyMesh&, Foam::Istream&, bool)
solidParticle.H:135:9: note:   candidate expects 3 arguments, 7 provided
solidParticleI.H:47:8: note: Foam::solidParticle::solidParticle(const Foam::polyMesh&, const vector&, Foam::label, Foam::label, Foam::label, Foam::scalar, const vector&)
solidParticleI.H:47:8: note:   no known conversion for argument 1 from ‘Foam::solidParticleCloud’ to ‘const Foam::polyMesh&’
solidParticle.H:58:7: note: Foam::solidParticle::solidParticle(const Foam::solidParticle&)
solidParticle.H:58:7: note:   candidate expects 1 argument, 7 provided 

Last edited by wyldckat; April 24, 2014 at 15:41. Reason: Added [CODE][/CODE]
houwy is offline   Reply With Quote

Reply

Tags
interfoam, lagrangian, move, solidparticle

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
lagrangian solid particle tracking - OFv2.1 PelusDadidus OpenFOAM Programming & Development 0 April 3, 2012 07:08
Questions regarding Particle Tracking and Rotating Frame of reference Maxime Gauthier CFX 1 May 9, 2011 15:07
DPM UDF particle position using the macro P_POS(p)[i] dm2747 FLUENT 0 April 17, 2009 01:29
Particle tracking - Domain interface / FrozenRotor mohanrao CFX 4 January 23, 2008 03:39
restarting lagrange (particle tracking) simulation dbdias CFX 0 September 22, 2007 19:26


All times are GMT -4. The time now is 00:02.