[anon_c]

hello jovai

me agian

could you plz tel me if there is some papers from you about the solver and how it works!??

i only take your master theses and your presentation it owuld be nice form you if you have any papers about it

[jovani]

Hello Tajoooko,

The papers about the solver was submitted but they are with the reviewers!
There is a small paper was presented in a congress and now published:

http://www.sciencedirect.com/science...84a12a8d75a411

but in this there is no relevant aspects about implementations only mathematical formulation and results.

Jovani

[anon_c]

hello

yeh is ok i only need the mathematical aspekts bcz i am doning a bechmark between your solver and a comerzial one like fluent (i just do the visous formulations in the fluent solver and going to do the DEVSS method in fluent)

so i need to see what about the diffrene to your solver in openfoam, i just recognized that yours is really stable in higher De numbers very nice work really

plz could you mail me the paper ?! i cant get incide

[mohsenkh599]

hi jovani
I have downloaded your new solver (viscoelasticFluidFoam). but how it works? would I just copy it and paste in application folder? please tell me what should I do?
the Best

[anon_c]

hi mohsenkh599

you have to recombile it

but the solver in an viscoelastic order, then go in application order and edit the Allmake file and then reombile it...

you have to look in the openfoam1.5-dev version how the file herarchiy should be (and do it like them) then reombile and you get the solver

[jovani]

Hi Mohsen,

You need specifies what OpenFOAM version are you using.
IF you are using OpenFOAM-1.5-dev the solver is already after you compiles the OF sources.
IF you have other OF them take a look in this same thread for one of my old post, once I answered how compile the solver in OF-1.6 times ago.

After the right compilation the solver will be ready to use, similar you uses icoFoam, for example. The tutorial of the solver (tutorials/viscoelasticFluidFoam) will guide you.

Best,

Jovani

[mohsenkh599]

hi Foamers
I am trying to simulate viscoelastic fluids flow through a contraction using models which were developed by jovani e.g. PTT, Leonov, ....
I am using version 1.6 on ubuntu 9.1 and a PC with 2.35 GHz of cpu. but it takes a very long time to solve.
I just alter the fvSolutions as follows because the solver "PBiCGstab" is not included in version 1.6:
solvers
{

p
{
solver PCG;
preconditioner DIC;
tolerance 1e-06;
relTol 0;
}

U
{
solver PBiCG;
preconditioner DILU;
tolerance 1e-05;
relTol 0;
}

taufirst
{
solver PBiCG;
preconditioner DILU;
tolerance 1e-05;
relTol 0;
}


}

PISO
{
momentumPredictor yes;
nCorrectors 2;
nNonOrthogonalCorrectors 1;
pRefCell 0;
pRefValue 0;
}

relaxationFactors
{
p 0.01;
U 0.01;
taufirst 0.01;
}

[jovani]

Hello Mohsen,

This simulations really takes some time. I see you changes in relaxation factors, but this is very very small now, this parameters is to make the problem more stable smoothing the solution and for your case this can`t help you to get the steady-state first, i.e, with this relaxation you need increase the final time too, I can`t see great enhancements with this changes. One think really can help you on your question is use multigrid techniques to solve pressure (is the pressure takes a lot of time). I used this on tutorials examples, but you need see how use multigrid tecnhiques in your OF version. I have feedback of some people have adjusted multigrid (in OF) for 3d geometries with good enhancements in computational cost.

Best,
Jovani

[jovani]

Hello Foamers,

Sometimes we want take the value of some property in any point of the domain for each time step. We do not need save data for each time step, once we can do more easy in OpenFOAM.

All is necessary is put some new lines in the controlDict file, i. e., the lines bellow:

functions
(
centerline // the name for the probe
{
// Type of functionObject
type probes;

// Where to load it from (if not already in solver)
functionObjectLibs ("libsampling.so");

// Locations to be probed. runTime modifiable!
probeLocations
(
(1 0 0) // first point to probe inside the geometry
(1.5 0 0) // second point to probe inside the geometry
);

// Fields to be probed. runTime modifiable!
fields
(
taufirst // create probe data to taufirst field (symmTensor)
U // create probe data to U field (vector)
p // create probe data to p field (scalar)
// .... another field we want
);
}
);

Soon we start the solver a directory named centerline is created into the case directory. Into this there is the time directory and into the time directory the files containing the data for the probe.

The files generated by probe are not ready to use in grace or gnuplot, once the data are in tensor OpenFOAM form. See bellow for the field U, for example:

# Time
1.19998e-05 (1.44637e-05 -1.50596e-11 0) (1.44637e-05 -1.91593e-11 0)
2.63988e-05 (3.17809e-05 -1.25082e-11 0) (3.17809e-05 -1.14036e-12 0)
4.36766e-05 (5.2514e-05 9.46453e-12 0) (5.2514e-05 5.30116e-12 0)

To process tensorial OF probes files and get another files ready to use in graph programs I use the shell script attached. The script automatically make xmgrace graphs too.

Once the script is on the system the usage is easy:

$foamProbe [<probes files directory> <numbers of monitoring points> <field name> <optional value: 0 - open in xmgrace, 1 - save to eps file>]

For the example above we can do:
$foamProbe centerline/0/ 2 U --> to create data for the 2 monitoring points and for field U.
or
$foamProbe centerline/0/ 2 U 0 --> to open in xmgrace. Obs.: this need xmgrace.
or
$foamProbe centerline/0/ 2 U 1 --> to create automatically eps figures for the data. Obs.: this need xmgrace too.

A new file is generated for each monitoring point.

Enjoy,

Jovani

[ata]

Hi Jovani
I hope you are well.
I have one question about your solver. When I copied viscoelastic models from OpenFOAM-dev to different version of OpenFOAM (I think it's name is standard version) and I used wmake for viscoelastic library it didn't compile correctly but when I used Allwmake for complete transport models library it worked correctly. Why?
Could you or any one else help me?
Thanks very much
Best regards

[ternik]

Originally Posted by jovani

Hello Foamers,

Sometimes we want take the value of some property in any point of the domain for each time step. We do not need save data for each time step, once we can do more easy in OpenFOAM.

All is necessary is put some new lines in the controlDict file, i. e., the lines bellow:

functions
(
centerline // the name for the probe
{
// Type of functionObject
type probes;

// Where to load it from (if not already in solver)
functionObjectLibs ("libsampling.so");

// Locations to be probed. runTime modifiable!
probeLocations
(
(1 0 0) // first point to probe inside the geometry
(1.5 0 0) // second point to probe inside the geometry
);

// Fields to be probed. runTime modifiable!
fields
(
taufirst // create probe data to taufirst field (symmTensor)
U // create probe data to U field (vector)
p // create probe data to p field (scalar)
// .... another field we want
);
}
);

Soon we start the solver a directory named centerline is created into the case directory. Into this there is the time directory and into the time directory the files containing the data for the probe.

The files generated by probe are not ready to use in grace or gnuplot, once the data are in tensor OpenFOAM form. See bellow for the field U, for example:

# Time
1.19998e-05 (1.44637e-05 -1.50596e-11 0) (1.44637e-05 -1.91593e-11 0)
2.63988e-05 (3.17809e-05 -1.25082e-11 0) (3.17809e-05 -1.14036e-12 0)
4.36766e-05 (5.2514e-05 9.46453e-12 0) (5.2514e-05 5.30116e-12 0)

To process tensorial OF probes files and get another files ready to use in graph programs I use the shell script attached. The script automatically make xmgrace graphs too.

Once the script is on the system the usage is easy:

$foamProbe [<probes files directory> <numbers of monitoring points> <field name> <optional value: 0 - open in xmgrace, 1 - save to eps file>]

For the example above we can do:
$foamProbe centerline/0/ 2 U --> to create data for the 2 monitoring points and for field U.
or
$foamProbe centerline/0/ 2 U 0 --> to open in xmgrace. Obs.: this need xmgrace.
or
$foamProbe centerline/0/ 2 U 1 --> to create automatically eps figures for the data. Obs.: this need xmgrace too.

A new file is generated for each monitoring point.

Enjoy,

Jovani

Hey Jovani,

thanks again for your contribution - I have tried your "Probes" recipe and (of course) it works well ! And your script for extracting the "Probed" results - I think it will make our "post-processing live" much easier!

One question - do you think it is possible (if yes, how) to use the "Probes" for the components of the symmetrical rate of deformation tensor and the average velocity of a fluid (the latter might be found useful for pressure-driven oscillating flows, i.e. flows where the average velocity and therefore fluid mass flow changes with time)?

Thank you again!

Enjoy,
Primoz

[jovani]

Hello,

Ata,
you need more then only "wmake" to compile this, once you are trying compile a LIBRARY (the viscoelastic models library). You must compile without problems using "wmake libso", this is what Allwmake script do!!

Primoz,

yes, is possible, there is more than 1 possibility to do it, but one fast and simple is:
Create an object to store symmetrical rate of deformation tensor and calculate this in each time step. Later this field can be used without problems with probe library. This can be done to others fields you want too. To flow and U average the simple way is see for patchAverage and patchIntegrate tools, or you can take the velocity on a boundary field U.boundaryField() and the area mesh.magSf().boundaryField() to do these calculations.


Enjoy,

Jovani

[ata]

Hi Jovani
Thank you very much for your reply.
Best regards

Ata

[anon_c]

hello viscoelastic foamers

i just implemnted a new model to use with viscoelasticfluidfoam this is very easy on an ubuntu 8.10 system the same way and prcedure in opensuse 10.3 didnt accept that

when i put in newmodell > (newmodell.C and newmodell.H) in viscoelasticlows

then go to the place of transprot modells where the ./Allmake is there then (before i need to wirte in make that is should also be done) i do this on ubuntu very succsicfull but in opensuse it complie it
and then by using viscoelasticfluidfoam allways it come that the model is not availebe

what is wrong?

[ata]

Hi Tajoooko
Did you add your model to Allwmake file itself?

[anon_c]

hi ata

i adad that in the directory

viscoelastic/Make

and then there in the

file data

i write the newModell like the otheres

then go out to directory

src/transportModells and there

just typ

./Allmake

and it seems that every thing is ok and it is compiled

(the same way i do in ubuntu 8.10) really the same way the only difference is that on this system i have opensuse 10.3??!! no idea now the secound third day with the same problem

this kind of adding a modell i do in the past very often on my ubuntu system

[ata]

Hi tajoooko
I hope you are well. Jovani got a thread for me on this topic. As he said you must open Allwmake in gedit and add a line at the end of it. See that post. I think it probably help you.
Best regards

Ata

[anon_c]

ah no the why that jovai discriped is complety the same i used under ubuntu and opensuse

i really dont under stnad what is the problem

i even also looked in side the directory the new model is in i can find all kind of need such like newmodell.o and so on even in the data file where all models are listed

but only when runing vsicoelasticfluidfoam then i see that there isn't this newmodell

[anon_c]

ok it is solved the problem was that i have in opensuse done the bachrc other then in ubuntu bcz i am using it from another source

thank you ata

[ata]

Hi tajoooko
How are you? I hope you are well. I am very glad for solving your problem.
I have a problem. When I compile a new model I got an error like this:
No rule to make target.
Do you or any one else help me?
Any help will be appreciated.
Best regards