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

Solidification in OpenFoam

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

Reply
 
LinkBack Thread Tools Display Modes
Old   April 28, 2009, 04:49
Default Solidification in OpenFoam
  #1
New Member
 
Luke Christ
Join Date: Apr 2009
Posts: 7
Rep Power: 8
luke.christ is on a distinguished road
Dear all,

I'm going to use OpenFoam for simulating a continuous casting problem. I'm completely new to OpenFoam, and it seems to me that there is not any solidification model in OpenFoam. Should I create solidification model myself?

As my case is continuous casting, I should consider a pull velocity for solid phase, too. Is it possible without great difficulties in OpenFoam?

I will be thankful for you reply.
luke.christ is offline   Reply With Quote

Old   January 30, 2013, 02:38
Default Updates
  #2
Member
 
,...
Join Date: Apr 2011
Posts: 92
Rep Power: 5
hawkeye321 is an unknown quantity at this point
Are you still interested in solidification in OpenFOAM?
hawkeye321 is offline   Reply With Quote

Old   May 3, 2013, 10:25
Default
  #3
New Member
 
Mac
Join Date: May 2013
Posts: 2
Rep Power: 0
Mac007 is on a distinguished road
Hello

I'm newbie with OpenFOAM, but I'm interested to model solidification of steel. If i have well understood, there is no built-in solver? Do you know where I can find one?

Regards
Mac007 is offline   Reply With Quote

Old   May 3, 2013, 11:00
Default solidification problem
  #4
Senior Member
 
fabian_roesler's Avatar
 
Fabian Roesler
Join Date: Mar 2009
Location: Bad Friedrichshall, Germany
Posts: 156
Rep Power: 8
fabian_roesler is on a distinguished road
Hi

In the thread melting problem you can find several solvers for melting and solidification using the enthalpy method and the enthalpy porosity method.

Regards

Fabian
fabian_roesler is offline   Reply With Quote

Old   May 6, 2013, 01:45
Default
  #5
New Member
 
Mac
Join Date: May 2013
Posts: 2
Rep Power: 0
Mac007 is on a distinguished road
Thanks a lot
Mac007 is offline   Reply With Quote

Old   June 9, 2013, 16:02
Default Explanation for terms in TEqn.H?
  #6
Member
 
einat
Join Date: Jul 2012
Posts: 31
Rep Power: 5
einatlev is on a distinguished road
Hello all!
I am trying to use meltFOAM for my project on solidification of lavas. I am trying to understand the terms appearing in TEqn.H. I identified the dT/dt, advection and diffusion terms, and then see terms that involve latent heat, and what I figure is some sort of a melt fraction term, but I don't understand the details -- what is the exponent, where did all the "4" factors come from, etc.?
Here's the code:

fvScalarMatrix TEqn
(
fvm::ddt(cp, T)
+ fvm::div(phi*fvc::interpolate(cp), T)
+ hs*4.0*exp(-pow(4.0*(T-Tmelt)/(Tl-Ts),2))/Foam::sqrt(pi)/(Tl-Ts)*fvm::ddt(T)
+ hs*4.0*exp(-pow(4.0*(T-Tmelt)/(Tl-Ts),2))/Foam::sqrt(pi)/(Tl-Ts)*(U & fvc::grad(T))
- fvm::laplacian(lambda/rho, T)
);

Thanks!!!
einatlev is offline   Reply With Quote

Old   June 11, 2013, 08:58
Default
  #7
Senior Member
 
fabian_roesler's Avatar
 
Fabian Roesler
Join Date: Mar 2009
Location: Bad Friedrichshall, Germany
Posts: 156
Rep Power: 8
fabian_roesler is on a distinguished road
Have a look into my paper on the solver:

F. Rösler, D. Brüggemann (2011): Shell-and-tube type latent heat thermal energy storage: numerical analysis and comparison with experiments. Heat and Mass Transfer, Vol. 47 Issue 8 , 1027-1033, DOI: 10.1007/s00231-011-0866-9
http://www.springerlink.com/content/b1tp01k2u7q8j432/

Keep in mind that the solver does not account for non-linearity like the linear source method by Voller. The erfMeltSolver just reduces the non-linearity effects in the energy conservation equation. For simple problems, the results converge with a very small error for the energy conservation. With increasing convective transport, the error increases and some iteration to account for the non-linearity have to be performed.
In my previous work, I use a linear liquid fraction function and the linear source method proposed by Voller.

Regards

Fabian
fabian_roesler is offline   Reply With Quote

Old   June 11, 2013, 11:15
Default
  #8
Member
 
einat
Join Date: Jul 2012
Posts: 31
Rep Power: 5
einatlev is on a distinguished road
Excellent paper Fabian! Thanks for pointing it. Just what I needed.
einatlev is offline   Reply With Quote

Old   July 6, 2013, 02:24
Default Stefan problem
  #9
Member
 
Vjoess
Join Date: Oct 2012
Posts: 52
Rep Power: 4
dinesh is on a distinguished road
Sir
i am also trying to analysize the phase change problem.I want to know is it possible to do it on Fluent and if yes which solver /model i should go for.
thanks

Quote:
Originally Posted by fabian_roesler View Post
Have a look into my paper on the solver:

F. Rösler, D. Brüggemann (2011): Shell-and-tube type latent heat thermal energy storage: numerical analysis and comparison with experiments. Heat and Mass Transfer, Vol. 47 Issue 8 , 1027-1033, DOI: 10.1007/s00231-011-0866-9
http://www.springerlink.com/content/b1tp01k2u7q8j432/

Keep in mind that the solver does not account for non-linearity like the linear source method by Voller. The erfMeltSolver just reduces the non-linearity effects in the energy conservation equation. For simple problems, the results converge with a very small error for the energy conservation. With increasing convective transport, the error increases and some iteration to account for the non-linearity have to be performed.
In my previous work, I use a linear liquid fraction function and the linear source method proposed by Voller.

Regards

Fabian
dinesh is offline   Reply With Quote

Old   July 10, 2013, 04:38
Default
  #10
Senior Member
 
fabian_roesler's Avatar
 
Fabian Roesler
Join Date: Mar 2009
Location: Bad Friedrichshall, Germany
Posts: 156
Rep Power: 8
fabian_roesler is on a distinguished road
Hi dinesh

Yes, Fluent offers an Enthalpy-Porosity-Method for simulation of solid/liquid phase change. Unfortunately I never used Fluent for such simulations so go on and find out yourself. Good luck.

Regards

Fabian
fabian_roesler is offline   Reply With Quote

Old   July 20, 2013, 11:59
Default
  #11
New Member
 
Mojtaba
Join Date: Nov 2012
Location: Tehran
Posts: 20
Rep Power: 4
r.mojtaba is on a distinguished road
Quote:
Originally Posted by dinesh View Post
Sir
i am also trying to analysize the phase change problem.I want to know is it possible to do it on Fluent and if yes which solver /model i should go for.
thanks
Hello danish.

As Fabian said, FLUENT can solve Solidification/Melting problems. I myself tested and validated the solver for my thesis. There are excellent tutorial and theory materials from Ansys Fluent. Using Google, you may find them with no problem.

Have fun!
r.mojtaba is offline   Reply With Quote

Old   August 30, 2013, 05:18
Default
  #12
Member
 
Vjoess
Join Date: Oct 2012
Posts: 52
Rep Power: 4
dinesh is on a distinguished road
Quote:
Originally Posted by r.mojtaba View Post
Hello danish.

As Fabian said, FLUENT can solve Solidification/Melting problems. I myself tested and validated the solver for my thesis. There are excellent tutorial and theory materials from Ansys Fluent. Using Google, you may find them with no problem.

Have fun!
I found from literature but there is contradiction.
Ref "H. Shmueli et al. / International Journal of Heat and Mass Transfer 53 (2010) 4082–4091" this paper says "page number 4086 says: As for the pressure discretization, only PRESTO!and Body-Force-Weighted schemes are available for the VOF and mixture multiphase models." Does this means that multiphase has to be used for my case. Enabling this i find that courant number can be inserted which the paper says to be kept around 0.5. what about the phase 1 and phase 2. see this post by me which flotus replied on 11july
Ref "http://www.cfd-online.com/Forums/system-analysis/120322-stefan-problem.html#post439934"
eagerly waiting for the reply
dinesh is offline   Reply With Quote

Old   August 30, 2013, 21:59
Default
  #13
New Member
 
Mojtaba
Join Date: Nov 2012
Location: Tehran
Posts: 20
Rep Power: 4
r.mojtaba is on a distinguished road
Quote:
Originally Posted by dinesh View Post
see this post by me which flotus replied on 11july
Ref "http://www.cfd-online.com/Forums/system-analysis/120322-stefan-problem.html#post439934"
So you have two zones, one is a closed container with PCM solidification and the other with a fluid flow around container, Right? If so, you don't need multiphase model at all. Using Fluent, during the solidification there is only one phase (fluid). To model solid zone (which is not really a solid phase in this model), Fluent adds a huge artificial viscosity to the solid zone to prevent flow on it. In this way, there is no need to define two phase flow.

I think this open access paper can help you:
A Numerical Study on Time-Dependent Melting and Deformation Processes of Phase Change Material (PCM) Induced by Localized Thermal Input
r.mojtaba is offline   Reply With Quote

Old   September 1, 2013, 08:34
Default
  #14
Member
 
Vjoess
Join Date: Oct 2012
Posts: 52
Rep Power: 4
dinesh is on a distinguished road
Quote:
Originally Posted by r.mojtaba View Post
So you have two zones, one is a closed container with PCM solidification and the other with a fluid flow around container, Right? If so, you don't need multiphase model at all. Using Fluent, during the solidification there is only one phase (fluid). To model solid zone (which is not really a solid phase in this model), Fluent adds a huge artificial viscosity to the solid zone to prevent flow on it. In this way, there is no need to define two phase flow.

I think this open access paper can help you:
A Numerical Study on Time-Dependent Melting and Deformation Processes of Phase Change Material (PCM) Induced by Localized Thermal Input
I went through this paper it refers on page no 529 TO REPRESENT THE FREE SURFACE OF THE MELTING REGION ADJACENT TO THE GAS PHASE, VOF METHOD IS USED. Now in fluent this VOF is under the menu of multiphase model. so plz clarify me? how can i find the melted region profile?
dinesh is offline   Reply With Quote

Old   September 3, 2013, 01:30
Default
  #15
New Member
 
Mojtaba
Join Date: Nov 2012
Location: Tehran
Posts: 20
Rep Power: 4
r.mojtaba is on a distinguished road
You didn't answer my question about whether the solidification zone is a fully filled container or not? If there is no gas in contact, using VOF is not necessary at all.
When you plot the contour of liquid fraction (F) the melt-solid (or melt-gas) interface can obviously be seen and extract. Refer to Kim's paper, Fig. 9 to 11.
r.mojtaba is offline   Reply With Quote

Old   September 3, 2013, 02:53
Default
  #16
Member
 
Vjoess
Join Date: Oct 2012
Posts: 52
Rep Power: 4
dinesh is on a distinguished road
Quote:
Originally Posted by r.mojtaba View Post
You didn't answer my question about whether the solidification zone is a fully filled container or not? If there is no gas in contact, using VOF is not necessary at all.
When you plot the contour of liquid fraction (F) the melt-solid (or melt-gas) interface can obviously be seen and extract. Refer to Kim's paper, Fig. 9 to 11.
I am handling without air case.
Plz see the plot i got
https://www.dropbox.com/s/gg3mqyum1u3mx5z/frac4000s.png
How can i extract the data regarding the anount or percent of solid melted/or mushy zone volume.
thanks
dinesh is offline   Reply With Quote

Old   September 3, 2013, 11:15
Default
  #17
New Member
 
Mojtaba
Join Date: Nov 2012
Location: Tehran
Posts: 20
Rep Power: 4
r.mojtaba is on a distinguished road
Quote:
Originally Posted by dinesh View Post
How can i extract the data regarding the amount or percent of solid melted/or mushy zone volume.
You need to calculate volume integral of liquid fraction. Fluent can do this by some simple Clicks. Do as below:
-From Menu Bar, go to Report and choose Volume Integrals... to open Volume Integral Window.
-In Volume Integrals Window:
--Choose Fluid (or whatever the solidification zone's name is) from right menu (Cell Zones),
--Choose Volume Integral from left menu (Report Type),
--Under Field Variable, select Solidification/Melting... and then Liquid Fraction,
--Click Compute button... and it's done!
Good Luck
r.mojtaba is offline   Reply With Quote

Old   September 4, 2013, 08:56
Default
  #18
Member
 
Vjoess
Join Date: Oct 2012
Posts: 52
Rep Power: 4
dinesh is on a distinguished road
Quote:
Originally Posted by r.mojtaba View Post
You need to calculate volume integral of liquid fraction. Fluent can do this by some simple Clicks. Do as below:
-From Menu Bar, go to Report and choose Volume Integrals... to open Volume Integral Window.
-In Volume Integrals Window:
--Choose Fluid (or whatever the solidification zone's name is) from right menu (Cell Zones),
--Choose Volume Integral from left menu (Report Type),
--Under Field Variable, select Solidification/Melting... and then Liquid Fraction,
--Click Compute button... and it's done!
Good Luck
thankyou very much for the support you provided.
Can you plz tell me about the discretization method. I used SIMPLE method with PRESTO scheme (without gravity being aplied) i got some result. Now i am using PISO with Body Force weighted with gravity added slowly from 1m/s2 to 9.81 m/s2 (as recommended by some user). I run the simulation for some time and then i get divergence either in epsilon or( x y z componenet of velocity) can you suggest some way to overcome this.
dinesh is offline   Reply With Quote

Old   September 4, 2013, 10:01
Default
  #19
New Member
 
Mojtaba
Join Date: Nov 2012
Location: Tehran
Posts: 20
Rep Power: 4
r.mojtaba is on a distinguished road
What are Ra and Pr numbers related to your simulation?

I've done an unsteady simulation of melting Gallium in a 2D cavity with Ra=2.2x10^5. I used SIMPLE for pressure-velocity coupling, PRESTO! for pressure discretization and SST k-w for turbulence modeling. You can obtain a good convergence with a small enough time step and fine enough grid.

If the convergence problem is still bothering, bring up more info about your simulation.
r.mojtaba is offline   Reply With Quote

Old   September 4, 2013, 14:03
Default
  #20
Member
 
Vjoess
Join Date: Oct 2012
Posts: 52
Rep Power: 4
dinesh is on a distinguished road
Quote:
Originally Posted by r.mojtaba View Post
What are Ra and Pr numbers related to your simulation?

I've done an unsteady simulation of melting Gallium in a 2D cavity with Ra=2.2x10^5. I used SIMPLE for pressure-velocity coupling, PRESTO! for pressure discretization and SST k-w for turbulence modeling. You can obtain a good convergence with a small enough time step and fine enough grid.

If the convergence problem is still bothering, bring up more info about your simulation.
With SIMPLE and PRESTO i also got the convergence. But with PISO and Body Force weighted i am not getting the convergence, I am refering" H Shmueli et al /IJHMT 53(2010) 4082-4091 where he is comparing the different schemes(page no 4085).
Regarding Pr and Ra i have not calculated. My hot water flow velocity is 0.1m/s at 350 K which is used to melt parafin wax which initially is at 293K and melting temperature is 313-316K. Hot fluid flows inside while the outer cylinder(0.6m dia 1m length) is enclosing the wax.
dinesh is offline   Reply With Quote

Reply

Tags
continuous casting

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
Superlinear speedup in OpenFOAM 13 msrinath80 OpenFOAM Running, Solving & CFD 18 March 3, 2015 06:36
Solidification simulation with OpenFOAM James OpenFOAM 5 June 26, 2012 02:33
64bitrhel5 OF installation instructions mirko OpenFOAM Installation 2 August 12, 2008 18:07
Adventure of fisrst openfoam installation on Ubuntu 710 jussi OpenFOAM Installation 0 April 24, 2008 14:25
OpenFOAM Debian packaging current status problems and TODOs oseen OpenFOAM Installation 9 August 26, 2007 13:50


All times are GMT -4. The time now is 06:27.