If you want to model a PCM with an air phase on top, you've correctly chosen solidification and melting model and VOF model. For simplicity, the air phase is often neglected and only PCM without volume expansion is simulated. If you use VOF, you have to initialize a solution with the two different materials, e.g. "pcm" and "air", which you have to specify in the VOF settings. The interface is then tracked by the VOF model. The initialization needs 3 steps: 1.) Initialize the first phase, e.g. "pcm" with "pcm volume fraction"  0, i.e. you have only "air" in your domain. 2.) Mark a region, where you want to have pcm: Chose adapt/region from the file menu, input coordinates and then click "mark". 3.) In solution initialization click on "patch", chose phase "pcm", variable "volume fraction", value 1, the marked region in "registers to patch" and then click "patch". Now, check your vof phase contours. If everything is fine, you're ready to start your simulation. Beware that you will need a pressure inlet/outlet or compressible air phase to allow volume expansion. Another to take special care of is material properties of the PCM over phase change, especially density.

If you want to model a PCM with an air phase on top, you've correctly chosen solidification and melting model and VOF model. For simplicity, the air phase is often neglected and only PCM without volume expansion is simulated. If you use VOF, you have to initialize a solution with the two different materials, e.g. "pcm" and "air", which you have to specify in the VOF settings. The interface is then tracked by the VOF model. The initialization needs 3 steps: 1.) Initialize the first phase, e.g. "pcm" with "pcm volume fraction"  0, i.e. you have only "air" in your domain. 2.) Mark a region, where you want to have pcm: Chose adapt/region from the file menu, input coordinates and then click "mark". 3.) In solution initialization click on "patch", chose phase "pcm", variable "volume fraction", value 1, the marked region in "registers to patch" and then click "patch". Now, check your vof phase contours. If everything is fine, you're ready to start your simulation. Beware that you will need a pressure inlet/outlet or compressible air phase to allow volume expansion. Another to take special care of is material properties of the PCM over phase change, especially density.

 Thanks very much Julian. This was really helpful. Is there a way to Patch an annular 3d configuration. I know in fluent one can mark a cylindrical region, but in my problem the region containing the pcm is annular with heat transfer fluid flowing through the center. Can I also use VOF for this? And if so, do I also specify the HTF as a phase? Without specifying 3 phases in the VOF model I'm not able to define a material for the HTF. Does this mean I now have 3 phases i.e HTF,  air and Pcm? 

I am happy to help. Do you have direct contact between PCM and HTF? And where is the air phase? Direct contact of PCM, HTF and air could be quite tricky. An annular region should be possible by initializing the whole cylindrical region with one phase (PCM) and then patching a smaller cylindrical region with the other phase (HTF).

Thanks for the help. There is no direct contact between the HTF and air/ Pcm. The Pcm and air are enclosed in the annular container made of copper. The air space above is to allow for the expansion of the Pcm. 

Okay, that's reasonable! Then you only need two VOF phases for PCM/air in the container and one single phase without VOF for the HTF. I am not sure, however, how to configure two different fluid regions in one domain. I think it's possible, but I never tried it. Is it possible to represent the HTF with a convective boundary condition instead of simulating the flow? You could specify a temperature profile over the height and use a heat transfer coefficient. You could even calculate all that in C in a UDF (if you're familiar with it) or just assume constant values that are only calculated once. That would make things easier.

I think using a convective boundary condition should work. I initially made a rough calculation of the convective heat transfer coefficient, and I can use that to simplify the calculation. I'm not looking for really high accuracy,  just basically trying to do a transient simulation to estimate the melting time of the Pcm. Thanks again sir! 

Hi Julian. One question please? How can i simulate the effect of sinking solid phase (unconstrained melting) for the pcm? In all simulations i've run so far i notice, the solid phase remains constrained even though the gravity effect is on.

Hi Obiajulu,You're very welcome. Sinking of the solid phase will only happen with a small "mushy zone constant". However, this will adversely affect phase change modelling. To my knowledge, there is no possibility to model correct sinking of the solid with the solidification and melting model in Fluent. You would have to integrate your own custom model as UDF or build a custom CFD code from scratch. But both options imply a great effort. To start with, I would simplify the problem to constrained melting without volume expansion. Later, you can enhance the model at will. Good luck with your simulation!

Thanks. I saw a journal where the effect of sinking was simulated and tried as much to replicate it to no avail. Though they didn't explain their procedure, i thought it might have to do with UDF, but not sure how to go about it. Just wanted to be sure, i'll probably look into writing a code when i have more time. For now, i'll simplify the problem as you said.

Do you mind my asking if you have solved the problem of defining the HTF after turning on the VOF? I encountered the same problem. I am so confused.

I recommend you to read this paper:

http://ijens.org/Vol_18_I_05/180505-3737-IJMME-IJENS.pdf

Best regards

Julian Vogel i am trying to simulate phase change of paraffin wax in a metal mesh. I am not sure if using the Solidification/melting model alone shall suffice or i have to use VOF as well as solidification/melting model together. Can you guide me about it?

Dear Zahid Ahmed Qureshi ,

from my experience, you can neglect volume expansion and therefore you don't need the VOF model. I compared a model with volume expansion to a model without it and did find only small differences. In the end, I used the solidification/melting model without VOF and validated it using my experimental setup. If you're interested, you can find the comparison and validation in this paper:

Article Validation of a numerical model with a benchmark Experiment ...

Best regards,

Julian

Dear Julian Vogel , thanks for your response. I performed a simulation of metal matrix-PCM composite being heated above the PCM's melting point. I was able to see the evolution of melting front. I am also interested in buoyancy velocities of the PCM but for some reason, I am not able to get non-zero velocities. The activated models are energy, viscuous laminar and solidification/melting (as you suggested i am not using VOF since the volume expansion is negligible).

Could you suggest any thing?

Dear Zahid Ahmed Qureshi ,

I am glad to hear that you could set up your test case.

To obtain buoyancy with constant density, you have to use the Boussinesq approximation. To do this in Fluent, you have to set Boussinesq under Density in the material properties. I would choose the liquid or mean solid/liquid density very close to the melting temperature. You also have to set a reference temperature under operating conditions. You can use the melting temperature, if you chose your density close to the melting point. You also have to set the thermal expansion coefficient, which is another material property.

For more detailed information on how to set up Fluent, I can recommend the tutorial "Modeling Radiation and Natural Convection" in the official ANSYS Fluent Tutorial Guide.

Please let me know if this was of any help or if you have any questions.

Best regards,

Julian

Dear julian, i am already using boussinesq approx under density. Since the PCM i m using has almost no volumetric expansion (2%) the densities in the solid and liquid states are almost identical. One thing that i genuinely messed up is taking a zero value for thermal expansion coefficient. I dont know how serious the repurcussions of this goofy are. Id it because of this that i m getting a zero value for buoyancy velocities.

Regards,

Zahid

Dear Zahid Ahmed Qureshi ,

That explains it. With a zero thermal expansion coefficient, there will be no buoyancy. With the Boussinesq approximation, the buoyancy term is linearized around a reference density rho0:

(rho-rho0)*g = rho0*beta*(T-T0)*g

with rho0 and T0 being the reference values specified in Fluent as Boussinesq density and reference temperature, and beta being the thermal expansion coefficient.

You might have to reduce the time step to obtain convergence with non-zero velocities.

Good luck,

Julian

Dear Julian, i will re visit, make these changes and give it a shot. I m sure it would prove fruitful. Thanks mate, stay blessed

Dear Pouyan,

As far as I know, the reference values in the reference values section do not change the results and they do not have to be adjusted. However, they might influence derived values such as total energy. I personally never had to change these reference values.

Best regards,

Julian

Dear Dr. Julian Vogel ,

I am doing a simulation about laser melting pool, but I would like to start with a simple case: ice melting & flowing.

I used Melting&Solidification, Energy, and VOF models. The BC & IC were like this: 300K for air domain, 270 K for the ice cubic domain, heat flux at the bottom of the ice, the others were just 300 K wall.

I had two animations: (1) Liquid fraction of ice (2) Volume Fraction of air.

None of them made sense if I kept the 3 models on, but if I turn off the melting model, I could see the water drop and spread out.

Could I have some suggestions from you, please?

Thanks,

Xiangtao

Dear Xiangtao Gong ,

I am not really familiar with this test case. Where does the water drop and spread out? Could you please provide an illustration of the test case?

I only know that it is not easy to combine all the models. So, testing the models separately is a good idea. Did you also test only melting without air phase and VOF?

Best regards,

Julian

Dear Dr. Julian Vogel ,

Thanks for your reply. I have attached the sketch of the test case. The blue is the air domain and the black is the ice domain. The ice will gradually melt into water and spread out the substrate, right?

I have tested only VOF model and set the initial condition of the black cube as water, the water will spread out because of the vertical gravity, the simulation looked ok.

I have tested the melting model as well, the solid phase shrink and turn into liquid phase.

I combined the two models, it did not work.

Thank you,

Xiangtao

Dear Xiangtao,

okay, good. And this domain is closed, so that there will be a pool of water at the bottom? And the solid will sink as a result of melting?

From my experience, using S&M model and VOF model together is possible, but you have to use small time steps, a reasonably fine mesh and tinker a lot with the VOF settings. And some other additional models could not work well, such as the surface tension model.

Sinking of the solid (so-called close contact melting) is not possible out of the box (AFAIK from the 2017 version), but it could be implemented using a UDF.

Best regards,

Julian

Dear Dr. Julian Vogel ,

Thanks a lot for your advice. I will try to fix my VOF settings.

Best regards,

Xiangtao

Dear Dr. Julian Vogel,

I am working on simulating the descending of solid PCM (n-octadecane) during unconstrained melting when the rectangular container is heated from all sides except the top (close contact melting) in FLUENT. I am currently using solidification and melting model along with VOF to model volume expansion, however I am not able to see the solid sinking.

I had initially used the Boussinesq approximation, however since it does not take into account the difference in densities between the solid and liquid phases, I changed to a piece-wise linear variation of density with temperature. But it still gave the same result.

And I did try out numerous VOF settings, none of which have proved fruitful.

I kindly request your help regarding this issue sir.

Dear @Shrikiran Srinivasan,

The problem with sinking of the solid lies in the solidification and melting model. This model forces the velocities in the solid very close to zero. When you decrease the mushy parameter, there will be more velocities in the solid and some sinking. But your solid will loose shape and also the sinking velocity might not be correct. To correctly attack this problem, you will have to write a UDF and include this functionality yourself. There are some research works out there with implementations in other software. But I don't know of any in fluent. Still I would assume it is possible.

Best regards,

Julian

Thank you for your valuable input sir. I will try writing a UDF to solve this issue.

Hi, a very basic question here. hope someone can help esp. Julian Vogel

I have a PCM which has a very small change in density during phase change i.e. it has a density of 0.90 kg/liter in solid phase (measure at 25 deg C) and a density of 0.89 kg/liter in liquid phase (measured at 80 deg C). The PCM has a melting range of 50-51 deg C. I want to impregnate this PCM in two different metal matrices and capture the differences in convective heat transfer indicated by buoyancy velocities.

What i fear is that this small difference in density over a huge temperature range (i.e. from 25 to 80 deg C) would not create any buoyancy (basic principle of buoyancy is differences in densities as a function of temperature). Therefore, the heat transfer in liquid phase would also be largely conduction dominated. Hence, i wont be able to capture the effect of metal matrix morphology in convective heat transfer.

Did i say it right?

Regards,

Zahid

Julian Vogel Attached below is the model 2-D Model that I created to simulate the phase change material. The center circle (The smallest circle) is the fluid domain. The bigger circle (Brown Colour) is the PCM and the top part which is the green coloured is cut off from the bigger circle and that is the air. I am not able to make the air and the PCM interact with one another by using the VOF. Can you advice me on how to resolve this problem?

Dear Zahid Ahmed Qureshi ,

I did not see such a small density difference between solid and liquid, yet. Do you have other data to confirm these values?

Moreover, buoyancy is generated by the density variation in the liquid (for natural convection in the liquid). So, you would need the density gradient in the liquid in the temperature range you're interested in. Also I am not aware of a material that has nearly no density variation in the liquid with temperature. However, I am not a material expert.

What kind of material is this?

Best regards,

Julian

Dear Muhamad Rosland,

that's an interesting test case. I have a couple of questions:

1.) Can the fluid and the PCM mix? How is the fluid modeled? Is it a solid acting as heat source or is flow being modeled?

2.) Do you want to model melting or solidification of the PCM?

3.) How is the volume expansion of the PCM compensated by the air layer? Can the air flow in or out somewhere?

My first advice:

1.) You do NOT need a seperate region for the air layer. With the VOF model, the PCM and air share the same region. Which part is air and which part is PCM, is determined when initializing the simulation with the "patch" functionality.

2.) You could use a structured mesh in the outer PCM+air ring and an O-Grid in the central fluid grid to improve solution convergence and accuracy.

Best regards,

Julian

Greetings Julian Vogel ,

To answer your question,

1. No, both the fluid and PCM will not mix due to the way I created the geometry. Each surface is generated from 3 different sketches. I am trying to make the fluid domain as the heat source but I am not able to do such a thing,

2. Melting processes.

3. I read this on a paper where the decreasing density of the pcm during melting caused volumetric expansion. Hence the air region was added to provide space for such expansion.

Greetings Julian Vogel

I am trying to simulate the melting processes of PCM just by having hot HTF flowing in the inner circle of the tube. Geometry shown as before with the air is neglected in this case. I patched the temperature of the HTF to the Inner circle to be higher than the liquidus temperature of the pcm itself but somehow the pcm is not interacting with hot HTF. Can you give insight on this?

Hi again Muhamad Rosland ,

if you just want to model PCM melting, the simplest and most robust way is to model only a PCM ring without the fluid region. So, you have only one material in your domain.

If you don't model fluid flow in axial direction, you don't need to create a region for the fluid. Instead, you can apply a convective boundary condition at the inner edge of the ring. This way, heat transfer from the fluid is approximated using a heat transfer coefficient and a fluid temperature.

You can model the PCM with the Boussinesq approximation of buoyancy and constant density. Then you won't have volume expansion and you also don't need an air phase.

Good luck with your test case!

Julian

It seems that if you have a UDF function to initialize the model, you could see the melting process. Write a code to define a zone of pcm with temp

you do inter name selection for interface wall in meshing and selected name is interface, far example: interface inner wall 1 or interface outer wall 1

Greetings, Julian Vogel

I am trying a melting problem, in which Initially the ice is in the inner ring and the water in the outer box initially at 21 deg Celcius as shown in the figure. I am unable to provide the initial condition. I am using, Solidification and melting model, VOF for multiphase modelling and k-epsilon for turbulence. Please guide me through

I'm modelling 2D melting and solidification of a phase change material in a container using Ansys fluent with VOF like the picture below but I don't know how to modeling this with VOF that initially complete solid PCM on the bottom that is 85% of container and above is Air. please help me.

Dear Parth and Mehran,

I would recommend to start by using only the solidification and melting model without the VOF model. If you obtain meaningful results, you can still extend your model setup. For such a simplified setup you would exclude the air region on top and assume a constant density for the pcm. The buoyancy is then created by the boussinesq approximation, which is set in the material properties for density.

Regarding turbulence, you should check the Rayleigh number and compare to a correlation for similar problems.

Regards, Julian

Dear Julian

I have another question. I want to create a region in Ansys 19 R3 but I can't find the icon to create. In last versions we can create in adapt but 19 R3 doesn't have.

Dear juloan

I was able to simulate the project, only the pcm melts faster than the actual laboratory conditions. Especially from the side of the chamber tube. What should I do to reduce the melting rate?

Dear Mehran,

I haven't used Ansys in a while, so I can't help you with the use of the newer versions.

Also, there could be many reasons for faster melting as in the laboratory, e.g. material properties, boundary conditions, melting range or solver settings.

Bests

Julian