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

InterTrackFoam any information

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

Reply
 
LinkBack Thread Tools Display Modes
Old   August 24, 2006, 02:03
Default Hello everybody ( specially to
  #1
New Member
 
rajon
Join Date: Mar 2009
Posts: 6
Rep Power: 8
rajon is on a distinguished road
Hello everybody ( specially to the developers),

From the wiki page of the OpenFoam, i came up with a solver in OpenFoam solving free surface simulation with surface tracking method. The link is:

http://www.mfix.org/mwiki/index.php/...e_Surface_Flow

I am using OpenFoam 1.3 version; unfortunately, this solver is not there :-( . I was wondering whether "interTrackFoam" is available for the users ?

If not, is there any example in OpenFoam 1.3 where surface tracking method has been implemented ?

Best regards,

Rajon
rajon is offline   Reply With Quote

Old   August 24, 2006, 04:23
Default Yup, this is in my development
  #2
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,761
Rep Power: 21
hjasak will become famous soon enough
Yup, this is in my development version togeter with a tutorial, courtesy of dr Zeljko Tukovic. You will need to compile OpenFOAM yourself. You can download the snapshot (they appear and disappear) from:

http://powerlab.fsb.hr/ped/kturbo/OpenFOAM/.

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   August 24, 2006, 05:13
Default Hi Hrv, Thanks for the info
  #3
New Member
 
rajon
Join Date: Mar 2009
Posts: 6
Rep Power: 8
rajon is on a distinguished road
Hi Hrv,

Thanks for the information & also for the link.

Best regards,

Rajon
rajon is offline   Reply With Quote

Old   August 24, 2006, 09:28
Default Hi Hrv, I have found the fo
  #4
New Member
 
rajon
Join Date: Mar 2009
Posts: 6
Rep Power: 8
rajon is on a distinguished road
Hi Hrv,

I have found the following version of OpenFoam from the link you provided me with :

OpenFOAM-1.3_15_08_06.tgz

I have already a standard OpenFoam-1.3 installed in my computer. Do i need to install your version of OpenFoam seprately ? Or can i use the interTrackFoam from the standard OpenFoam-1.3 ?


Thanks for yr time

regards,

Rajon
rajon is offline   Reply With Quote

Old   August 24, 2006, 10:03
Default I don't give you good odds on
  #5
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,761
Rep Power: 21
hjasak will become famous soon enough
I don't give you good odds on this - it is likely that you will hit trouble because of various updates and bug fixes I've mande in the meantime. You're welcome to try but I personally wouldn't waste my time.

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   August 31, 2006, 04:12
Default Hi Hrv, I am contacting you
  #6
New Member
 
rajon
Join Date: Mar 2009
Posts: 6
Rep Power: 8
rajon is on a distinguished road
Hi Hrv,

I am contacting you again for your version of OpenFoam so that i can use the case inteTrackFoam.

I must confess that I am new with linux systems & i am using bash. Your implementation is built on "tcsh" & i didnot find any "Binary pack, double precision (required for Linux platform)" that is needed to install standard OpenFoam. In order to use your version, am i in need of any Binary pack as the standard release ?

If it is ok with you, then can you explain me, how can i use your version which uses "tcsh", in "bash" that i have.

Best regards,

Rajon
rajon is offline   Reply With Quote

Old   August 31, 2006, 05:29
Default Yes, sorry about that: people
  #7
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,761
Rep Power: 21
hjasak will become famous soon enough
Yes, sorry about that: people in Zagreb are reconfiguring the ftp server and it is likely to be down for a few days.

I have temporarily put a copy of the source pack into my Mac repository (it will be removed when the "normal" site comes back)

http://homepage.mac.com/h.jasak/

As for the "bash and tcsh" question, both work in the same way as with the release. You should have no problems. Please note that I always use the latest version of the compiler and supporting tools - the forum will tell you how to deal with this.

Enjoy,

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   August 31, 2006, 05:32
Default Sorry, forgot: this is a sourc
  #8
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,761
Rep Power: 21
hjasak will become famous soon enough
Sorry, forgot: this is a source pack: you will need to compile it yourself.

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   August 31, 2006, 06:06
Default Thanks a lot, Hrv. I will try
  #9
New Member
 
rajon
Join Date: Mar 2009
Posts: 6
Rep Power: 8
rajon is on a distinguished road
Thanks a lot, Hrv. I will try to compile your sources. And, please be prepared for some more questions :-) ..

Best regards,

Rajon
rajon is offline   Reply With Quote

Old   January 17, 2007, 10:43
Default Hi Dr Zeljko Tukovic and Dr Hr
  #10
Senior Member
 
Jens Klostermann
Join Date: Mar 2009
Posts: 117
Rep Power: 8
jens_klostermann is on a distinguished road
Hi Dr Zeljko Tukovic and Dr Hrvoje Jasak,

Thank you for interTrackFoam. I try to set up a case with it, but got some problems with faMesh directory. Is there a tool which creates the files?
What I did so far:

-created file faceLabels with faceSets
-left file boundary empty, just set (), which is possible wrong. I guess this is the boundary (edges) of the free surface. How to create this file? How to get the edge labels?

-in file faMeshDefinition I just put

-----------------------------------------------
polyMeshPatches 1( freeSurface );

boundary
{
wall_1
{
type wall;
ownerPolyPatch freeSurface;
neighbourPolyPatch wall_1;
}

wall_2
{
type wall;
ownerPolyPatch freeSurface;
neighbourPolyPatch wall_2;
}

-------------------------------------------------

So when I run the case I get a very high curvature of the surface, output of the first timeStep:

Create mesh, no clear-out for time = 0

Reading field p

Reading field U

Reading/calculating face flux field phi

Selecting motion solver: laplaceTetDecomposition
Selecting motion diffusion: patchEnhanced
Found free surface patch. ID: 4

Starting time loop

Time = 0.002
Courant Number mean: 0 max: 0.633947
Free surface curvature: min = 0, max = 346.383, average = 34.3053
BICCG: Solving for Ux, Initial residual = 1, Final residual = 3.85494e-17, No Iterations 1
BICCG: Solving for Uy, Initial residual = 0, Final residual = 0, No Iterations 0
BICCG: Solving for Uz, Initial residual = 1, Final residual = 2.15042e-16, No Iterations 1
ICCG: Solving for p, Initial residual = 1, Final residual = 9.33451e-09, No Iterations 397
ICCG: Solving for p, Initial residual = 0.035736, Final residual = 8.79983e-09, No Iterations 349
time step continuity errors : sum local = 3.64974e-11, global = -7.30283e-14, cumulative = -7.30283e-14
Free surface flux: sum local = 0, global = 0
Free surface continuity error : sum local = nan, global = nan


Why is there such a hight free Surface curvature?
(All faces of the path survace are coplanar.)

Is it because of the faMesh/boundary file?

Best regards

Jens
jens_klostermann is offline   Reply With Quote

Old   January 17, 2007, 12:21
Default Hi Jens, You can use makeFa
  #11
New Member
 
Zeljko Tukovic
Join Date: Mar 2009
Posts: 22
Rep Power: 8
ztukovic is on a distinguished road
Hi Jens,

You can use makeFaMesh application to create faMesh data. But before that you have to set the faMeshDefinition properly.

Regards,
Zeljko
ztukovic is offline   Reply With Quote

Old   January 18, 2007, 09:04
Default Hi Zeljko, What do I have t
  #12
Senior Member
 
Jens Klostermann
Join Date: Mar 2009
Posts: 117
Rep Power: 8
jens_klostermann is on a distinguished road
Hi Zeljko,

What do I have to do to make a parallel interTrackingFoam run?

With the following I had no success

-decompose the mesh
-creation of faMeshDefinition in the processor*/constant directory (with and without explicit declaration of the processor boundary in faMeshDefinition, but not the globalprocessor)
-makeFaMesh root case -parallel

This all led to no sucess.

Thanks,

Jens
jens_klostermann is offline   Reply With Quote

Old   January 19, 2007, 04:36
Default Hi Jens, In order to make p
  #13
New Member
 
Zeljko Tukovic
Join Date: Mar 2009
Posts: 22
Rep Power: 8
ztukovic is on a distinguished road
Hi Jens,

In order to make parallel run you have to be sure that freeSurface (and freeSurfaceShadow) patch exists only on master processor. After that you have to make faMesh data on each processor using makeFaMesh . processor*. Size of faMesh on the slave processors must be zero.

Regards,
Zeljko
ztukovic is offline   Reply With Quote

Old   January 23, 2007, 13:50
Default Hi Hi Zeljko, I have anothe
  #14
Senior Member
 
Jens Klostermann
Join Date: Mar 2009
Posts: 117
Rep Power: 8
jens_klostermann is on a distinguished road
Hi Hi Zeljko,

I have another question:
In my case the free Surface is "connected" to a wall. How does the mesh move on the edge (wall-freeSurface) in this case? What are the right boundary conditions for these walls in motionU (slip or fixed value)?

Best regards
Jens
jens_klostermann is offline   Reply With Quote

Old   January 23, 2007, 15:44
Default Hi Jens, You can use slip b
  #15
New Member
 
Zeljko Tukovic
Join Date: Mar 2009
Posts: 22
Rep Power: 8
ztukovic is on a distinguished road
Hi Jens,

You can use slip boundary condition if your wall is flat.

Regards,
Zeljko
ztukovic is offline   Reply With Quote

Old   January 24, 2007, 08:47
Default Hi Zeljko, that is what I t
  #16
Senior Member
 
Jens Klostermann
Join Date: Mar 2009
Posts: 117
Rep Power: 8
jens_klostermann is on a distinguished road
Hi Zeljko,

that is what I thought. Can you give me a hint how the Free surface curvature is determined. I found in src/finiteArea/meshes/faMesh/faMeshDemandDrivenData.C

areaVectorField kN =
fac::edgeIntegrate(Le()*edgeLengthCorrection());

faceCurvatures = sign(kN&faceAreaNormals())*mag(kN);


What means Le and sign?

I have the problem that I get localy a very high surface curfatures:
Free surface curvature: min = -269.011, max = 246.218, average = -1.08988
BICCG: Solving for Ux: solution singularity
BICCG: Solving for Uy: solution singularity
BICCG: Solving for Uz: solution singularity
AMG: Solving for p, Initial residual = nan, Final residual = nan, No Iterations 501
AMG: Solving for p, Initial residual = nan, Final residual = nan, No Iterations 501
time step continuity errors : sum local = nan, global = nan, cumulative = nan
Free surface flux: sum local = nan, global = nan
Free surface continuity error : sum local = nan, global = nan

... and than I get bad nans, which I think, come from the mesh distortion. Any idea how I can get rid off them?

Best regards

Jens
jens_klostermann is offline   Reply With Quote

Old   January 24, 2007, 18:20
Default Hello Jens, Unfortunately,
  #17
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,761
Rep Power: 21
hjasak will become famous soon enough
Hello Jens,

Unfortunately, Zeljko was very unlucky and had to write his Thesis in Croatian to satisfy the requirements of the PhD Exam Board in Zagreb. He's been working on the translation for a while but due to other work he is doing as well, the english version is not ready yet. Unless you've got a Croatian colleague at the office (or one of our neighbours), I cannot provide a good reference for your question.

The surface curvature calculation is something that Zeljko has done very carefully and is based only on point positions (rather than faces). Whe is being done in the lines of code above is the calculation of the divergence of the surface normal vector using FInite Area discretisation.

My guess is that your surface is indeed folded over at this stage and that curvature number are real. It might be worth while visualising the surface to see wnat happened - no errors in the code.

Please keep me posted,

Hrv

P.S. Of course, once the translation is complete, Zeljko's Thesis in Englis will become available on http://www.foamcfd.org together with all the other material I can lay my hands on. If anyone in the Forum has publications or slides to add, please let me know.
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   January 25, 2007, 04:57
Default Hi Jens, If you give me you
  #18
New Member
 
Zeljko Tukovic
Join Date: Mar 2009
Posts: 22
Rep Power: 8
ztukovic is on a distinguished road
Hi Jens,

If you give me your case I could try to find out what is wrong.

Regards,
Zeljko
ztukovic is offline   Reply With Quote

Old   February 20, 2009, 06:49
Default Hello, I have a question a
  #19
Member
 
Virginie Ehrlacher
Join Date: Mar 2009
Posts: 52
Rep Power: 8
virginie_e is on a distinguished road
Hello,

I have a question about interTrackFoam. I am trying to simulate the flow of a liquid over a slope with it and I realized that the more vsicous the liquid is, the smaller the time step should be so that the simulation runs. I am quiet astonished because usually in CFD it is the opposite. Can soemone explain me why it is so with interTrackFoam?
Thank you a lot.

Virginie
virginie_e is offline   Reply With Quote

Old   March 6, 2009, 04:48
Default Hello, I have a question a
  #20
Member
 
Virginie Ehrlacher
Join Date: Mar 2009
Posts: 52
Rep Power: 8
virginie_e is on a distinguished road
Hello,

I have a question about faMeshDefinition in interTrackFoam.
I know you have already talked about it above in the thread but I still can't get what makeFaMesh does exactly. Does it simply set the boundary of the free surface or does it do something a little more complex?


I have another question, in faMeshDefintion, Jens Klosterman used a faPatch of type wall:

boundary
{
wall_1
{
type wall;
ownerPolyPatch freeSurface;
neighbourPolyPatch wall_1;
}

wall_2
{
type wall;
ownerPolyPatch freeSurface;
neighbourPolyPatch wall_2;
}

I would have liked to make the same, however I am using OpenFOAM-1.5-dev and I get the following error message:
Unknown faPatch type wall

Valid faPatch types are :

4
(
empty
processor
wedge
patch
)

Has the faPatch wall been deleted from the 1.5 version? If yes why and what should I set as a faPatch instead? If no, have you got an idea why I do not have it in the sources?

Thank you in advance.

Virginie
virginie_e 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
Wall contact in interTrackFoam virginie_e OpenFOAM Running, Solving & CFD 2 November 8, 2011 12:52
SIMPLE loop in interTrackFoam virginie_e OpenFOAM Running, Solving & CFD 3 March 17, 2009 06:40
Pressure divergence with interTrackFoam virginie_e OpenFOAM Running, Solving & CFD 8 March 4, 2009 06:07
OF15dev Hydrofoil tutorial for interTrackFoam philippose OpenFOAM Bugs 7 February 22, 2009 16:22
InterTrackFoam error kester OpenFOAM Running, Solving & CFD 10 November 8, 2007 03:55


All times are GMT -4. The time now is 22:42.