CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   InterTrackFoam any information (http://www.cfd-online.com/Forums/openfoam-solving/57837-intertrackfoam-any-information.html)

rajon August 24, 2006 02:03

Hello everybody ( specially to
 
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

hjasak August 24, 2006 04:23

Yup, this is in my development
 
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

rajon August 24, 2006 05:13

Hi Hrv, Thanks for the info
 
Hi Hrv,

Thanks for the information & also for the link.

Best regards,

Rajon

rajon August 24, 2006 09:28

Hi Hrv, I have found the fo
 
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

hjasak August 24, 2006 10:03

I don't give you good odds on
 
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

rajon August 31, 2006 04:12

Hi Hrv, I am contacting you
 
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

hjasak August 31, 2006 05:29

Yes, sorry about that: people
 
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

hjasak August 31, 2006 05:32

Sorry, forgot: this is a sourc
 
Sorry, forgot: this is a source pack: you will need to compile it yourself.

Hrv

rajon August 31, 2006 06:06

Thanks a lot, Hrv. I will try
 
Thanks a lot, Hrv. I will try to compile your sources. And, please be prepared for some more questions :-) ..

Best regards,

Rajon

jens_klostermann January 17, 2007 10:43

Hi Dr Zeljko Tukovic and Dr Hr
 
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

ztukovic January 17, 2007 12:21

Hi Jens, You can use makeFa
 
Hi Jens,

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

Regards,
Zeljko

jens_klostermann January 18, 2007 09:04

Hi Zeljko, What do I have t
 
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

ztukovic January 19, 2007 04:36

Hi Jens, In order to make p
 
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

jens_klostermann January 23, 2007 13:50

Hi Hi Zeljko, I have anothe
 
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

ztukovic January 23, 2007 15:44

Hi Jens, You can use slip b
 
Hi Jens,

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

Regards,
Zeljko

jens_klostermann January 24, 2007 08:47

Hi Zeljko, that is what I t
 
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

hjasak January 24, 2007 18:20

Hello Jens, Unfortunately,
 
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.

ztukovic January 25, 2007 04:57

Hi Jens, If you give me you
 
Hi Jens,

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

Regards,
Zeljko

virginie_e February 20, 2009 06:49

Hello, I have a question a
 
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 March 6, 2009 04:48

Hello, I have a question a
 
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


All times are GMT -4. The time now is 17:12.