CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   solidification (freezing) (http://www.cfd-online.com/Forums/fluent/99415-solidification-freezing.html)

eneja April 3, 2012 05:33

solidification (freezing)
 
Does anybody have an idea how could I model freezing of water in sand? Let's say we have box filled with sand and water, initially above 0 degrees and than temperature falls bellow 0. I am not sure how to model zone which contains sand and water.
Any suggestions?

Thanks in advance

LuckyTran April 3, 2012 10:37

Quote:

Originally Posted by eneja (Post 352863)
Does anybody have an idea how could I model freezing of water in sand? Let's say we have box filled with sand and water, initially above 0 degrees and than temperature falls bellow 0. I am not sure how to model zone which contains sand and water.
Any suggestions?

Thanks in advance

Is the sand stationary or is it a particle laden flow?

If the sand is stationary, you can define the sand as a porous media and that should allow you to model the flow of water through sand.

The porous model in Fluent uses the Darcy-Weisbach (and related) correlations. These models are based on empirical observations of packed beds (gravel and dirt). I imagine they can be used for sand as well without any loss of accuracy.

eneja April 3, 2012 10:45

There is no flow of water. I only have to take into account heat transfer and solidification.
I am not sure if Fluent calculates effective conductivity or also effective heat capacity and density. I used porous model and run calculation and when investigating properties of zone, results were strange. Conductivity was OK, but contours of liquid fraction, density and specific heat didn't show anything.
Besides, which thermal model should I use (equilibrium or non-equi.)?

Thanks!

LuckyTran April 3, 2012 11:36

Quote:

Originally Posted by eneja (Post 352936)
There is no flow of water. I only have to take into account heat transfer and solidification.
I am not sure if Fluent calculates effective conductivity or also effective heat capacity and density. I used porous model and run calculation and when investigating properties of zone, results were strange. Conductivity was OK, but contours of liquid fraction, density and specific heat didn't show anything.
Besides, which thermal model should I use (equilibrium or non-equi.)?

Thanks!

The porous model also is compatible with multiphase model so there also should not be any problems there.

Are you performing a transient simulation of the melting process or just calculating the steady state distribution? Equilibrium thermal model can be used for when the porous media (sand) is in thermal equilibrium with the fluid (water). I don't see any reason why the equilibrium model wouldn't be valid. The equilibrium model is valid for steady state and transient flows. Thermal equilibrium refers to the contact patch between the solid and fluid zones, where they interact they must have the same temperature (for exotic situations, even when in contact the two materials can hold different temperatures and the equilibrium model will not be valid).

Recall that the energy transport is the first calculated quantity before the temperature is solved.

For the equilibrium model, Fluent uses the effective thermal conductivity to calculate what the heat flux should look like (which will eventually yield temperature). The effective thermal conductivity is the volume average of the conductivities of solid and fluid (for steady state, density and specific heat do not have any influence).

For transient, a similar weighted thermal inertial is used for both zones to calculate the heat flux. After the energy transport is known, the specific heat is taken care of in the final calculation to calculate temperature. No effective density / specific heat is used. Only an effective conductivity. All other mixed zone properties are computed directly.

eneja April 4, 2012 05:22

I am performing transient simulation.
I did the following: I turned on energy eq. and solidification/melting, I set viscous model to laminar (not sure if this is necessary).
Results for temperature are OK, but liquid fraction remains all the time 1. I would expect that it changes as the water solidifies.
Any ideas what to do?

LuckyTran April 4, 2012 08:57

Quote:

Originally Posted by eneja (Post 353066)
I am performing transient simulation.
I did the following: I turned on energy eq. and solidification/melting, I set viscous model to laminar (not sure if this is necessary).
Results for temperature are OK, but liquid fraction remains all the time 1. I would expect that it changes as the water solidifies.
Any ideas what to do?

If temperature is OK, then there should be some locations where the temperature is less than the solidus point correct? Your liquid fraction can only be 0 or 1 since water does not have a mixed phase (solidus and liquidus temperature are equal).

Did your remember to specify the material properties? The default for solidus and liquidus temperature is 0K (absolute zero) and should be changed to 273.15 or similar.

Also by default, the properties of the solid and liquid phases are the same (density, specific heat, conductivity). Just something to keep in mind. Getting the simulation to work in this stage is an important first step. For improved accuracy later, and when there is time, you should make the properties piece-wise polynomials (with 1 constant coefficient per temperature range) as a function of temperature.

ravipvb October 3, 2012 23:26

solidification of water-copper mixture
 
Dear All,
I am simulation the solidification of water Cu nanoparticles mixtures. I want to vary the Grashof number with density of various volume fraction of nano particles. can anyone suggest me how to do that in ANSYS Fluent ?

jobito_2012 October 14, 2012 15:29

CAN you send me the details of the answer of the problem? geometry,mesh,setup,solutio
 
Quote:

Originally Posted by eneja (Post 352863)
Does anybody have an idea how could I model freezing of water in sand? Let's say we have box filled with sand and water, initially above 0 degrees and than temperature falls bellow 0. I am not sure how to model zone which contains sand and water.
Any suggestions?

Thanks in advance


Hi, i need to do the same, can you send me the details of the answer of the problem please??...thanks a lot!!

my mails is: aguilera1623@gmail.com

(Im sorry for my English, im learning) :)


All times are GMT -4. The time now is 06:13.