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

InterFoam: add a source term in alpha eq.

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

Reply
 
LinkBack Thread Tools Display Modes
Old   November 28, 2011, 06:26
Default InterFoam: add a source term in alpha eq.
  #1
Member
 
valerio
Join Date: Jun 2009
Location: Nancy
Posts: 30
Rep Power: 8
Alucard is on a distinguished road
Goodmorning,

I'm try to simulate the growth of a cristal using,as a basis, interfoam.
As i'm at the beginning, i consider as a first case, a simple 2D circle that grows at a constant velocity "Uoo". Alpha=1 in the circle and 0 outside.

So what i want to "see" it's just a simple circle that grows in time in my square domain.
If the basic alpha transport equation is something like that:

d(alpha)/dt+U*grad(alpha)=0

in my case I add a "second" velocity that is the envelope growth:

d(alpha)/dt+U*grad(alpha)+Ug*grad(alpha)=0

So if I initialise my U=0 (I 've not motion of my circle) and I impose a constant Ug, how it's possible to integrate correctly this term "Ug*grad(alpha)" in the equation?

I tried to replace directly U=Ug BUT the calculation of the phi fluxes is quite complicated and realted to Ueqn so I cannot do that easily.
I know perhaps is a dummy question but it's 10 days I'm trying to figure out how to solve it and I don't see a clever solution to that.


Thank you in advance.

Last edited by Alucard; November 28, 2011 at 06:42.
Alucard is offline   Reply With Quote

Old   November 28, 2011, 08:37
Default
  #2
Member
 
Sabin Ceuca
Join Date: Mar 2010
Location: Munich
Posts: 42
Rep Power: 7
sabin.ceuca is on a distinguished road
Hi,
if i were you i would take a look at the alphaEqn.H of interPhaseChangeFoam and just tailor it to suite your needs.
Although i don't understand your reasons behind it, because the alpha transport equation reads somehow different from what you have posted here.
sabin.ceuca is offline   Reply With Quote

Old   November 28, 2011, 09:24
Default
  #3
Member
 
valerio
Join Date: Jun 2009
Location: Nancy
Posts: 30
Rep Power: 8
Alucard is on a distinguished road
Quote:
Originally Posted by sabin.ceuca View Post
Hi,
if i were you i would take a look at the alphaEqn.H of interPhaseChangeFoam and just tailor it to suite your needs.
Although i don't understand your reasons behind it, because the alpha transport equation reads somehow different from what you have posted here.
Hi,
thank you I'm looking at it right now I guess I've to work on the "Su" term (I don't know exactly how yet!
Why I'm using the interfoam approach?
Cause I have two phases in my study (liquid and solid) and So I need a "marker" for the phase.
So as I need a method that allows me to transport phases without numerical diffusion I thought to interFoam where all the "tricks" in order to have a sharp interface during time are already developped.
So i tried rigid translations and roatation of a circle with success and now I was trying to add the term related to surface growth.
In the complete problem it will be function of Temperature and other thermodynamical parameters but for the moment I impose it.
Why so do you think my approach is not the good one?
Thanks
Alucard is offline   Reply With Quote

Old   November 28, 2011, 09:39
Default
  #4
Member
 
valerio
Join Date: Jun 2009
Location: Nancy
Posts: 30
Rep Power: 8
Alucard is on a distinguished road
So a good way to do that could be to write the "Su" term like that?

volScalarField Su
(
IOobject
(
"Su",
runTime.timeName(),
mesh
),
// Divergence term is handled explicitly to be
// consistent with the explicit transport solution
fvc::grad(alpha1) & Ug

);


where Ug is the "growth velocity" vector field (I already initalised in my code)?

Thank you again.
Alucard is offline   Reply With Quote

Old   November 28, 2011, 09:41
Default
  #5
Senior Member
 
Olivier
Join Date: Jun 2009
Location: France, grenoble
Posts: 238
Rep Power: 9
olivierG is on a distinguished road
Hello,

I think interFoam is not the best method in cristal grow, because usually the interface transition is very sharp, and with VOF method, you will get a "sharp but not enough" interface, + difficulties to set thermal source / density.

The best method may be Level set, but i don"t know how to deal with in OpenFoam (though i've seen a VOF/ level set coupling related to openFoam somewhere in a workshop pdf.)

Anyway, i would try to setup an hybrid buoyant+InterFoam, i.e thermal with variable properties and VOF, so if you go that way, we can share some part of the solver.

regards,

olivier
olivierG is offline   Reply With Quote

Old   November 28, 2011, 10:20
Default
  #6
Member
 
Sabin Ceuca
Join Date: Mar 2010
Location: Munich
Posts: 42
Rep Power: 7
sabin.ceuca is on a distinguished road
Hi Alucard,
yes your Su looks fine, give it a try. From the point of view of OF it looks good , if it makes sense from a point of view of the physics you'll see.
Greets
sabin.ceuca is offline   Reply With Quote

Old   November 28, 2011, 13:02
Default
  #7
Member
 
valerio
Join Date: Jun 2009
Location: Nancy
Posts: 30
Rep Power: 8
Alucard is on a distinguished road
Quote:
Originally Posted by sabin.ceuca View Post
Hi Alucard,
yes your Su looks fine, give it a try. From the point of view of OF it looks good , if it makes sense from a point of view of the physics you'll see.
Greets
Thank you ,
it worked in OF (compilation+running) but not under a phisical point of view...I don't know why, i also tried to solve explicitly the equation:

" alpha1=alpha1-runTime.deltaT()*(Ug_mod*mag(fvc::grad(alpha1))); "
with Ug_mod, module of the velocity vector
but I'm having strong oscillations close to the circle-interface and alpha that becomes higher than 1.
Do you think something is wrong?

(before I tried to put Su as supposed and i got the same kinda of results)
Alucard is offline   Reply With Quote

Old   November 29, 2011, 05:10
Default
  #8
Member
 
Sabin Ceuca
Join Date: Mar 2010
Location: Munich
Posts: 42
Rep Power: 7
sabin.ceuca is on a distinguished road
Hmm,
don't worry it never works at the first try Did you also implement source and sink terms to the pEqn and UEqn? Because it might be that you create some 1st phase but do not transport it away.
Bon courage!
Sabin
sabin.ceuca is offline   Reply With Quote

Old   November 29, 2011, 09:50
Default
  #9
Senior Member
 
akidess's Avatar
 
Anton Kidess
Join Date: May 2009
Location: Delft, Netherlands
Posts: 919
Rep Power: 17
akidess will become famous soon enough
olivierG, the solid-liquid interface is sharp for pure materials, and diffuse for melting of alloys.

Nonetheless I agree interFoam is not the best choice for this problem. Instead, if not too late, I recommend having a look at phase-change solvers which other users have posted:
melting problem
akidess is offline   Reply With Quote

Old   January 13, 2012, 11:16
Smile melting solver
  #10
Senior Member
 
fabian_roesler's Avatar
 
Fabian Roesler
Join Date: Mar 2009
Location: Bad Friedrichshall, Germany
Posts: 164
Rep Power: 8
fabian_roesler is on a distinguished road
Hi all

nice that my melting solver

melting problem

made it into another thread of this forum.
I although tried using interFoam for melting and solidification problems. But as you have a solid phase, alpha cannot be transported as done in VOF. My solver uses the enthalpy-porosity-method proposed by Voller. The solver will be improved in the next months.

Regards

Fabian
fabian_roesler 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
Solve poisson equation just add a source term nandiganavishal OpenFOAM Running, Solving & CFD 16 August 28, 2014 13:02
GPU Linear Solvers for OpenFOAM gocarts OpenFOAM Announcements from Other Sources 35 March 1, 2012 21:41
DxFoam reader update hjasak OpenFOAM Post-Processing 69 April 24, 2008 01:24
How can I add a source term danielle OpenFOAM Running, Solving & CFD 1 February 29, 2008 12:52
UDFs for Scalar Eqn - Fluid/Solid HT Greg Perkins FLUENT 0 October 11, 2000 03:43


All times are GMT -4. The time now is 17:51.