Cooling behavior of liquid aluminum
Hallo @ all,
I am new here and I am new to star ccm+ too.
Also english is not my first language, so sorry for all the faults.
I need help with a strange problem, i want to simulate the cooling down of an tank filled with a liquid set to a specific temperature, for this purpose i have generated a simple geometry a outer cylinder for the solid (concrete)
and a inner cylinder filled with the liquid (water etc.), they are both connected with a interface
the outer boundaries of the outer cylinder are set to enviromental
when i start the simulation the outer solid clyinder behaves like expected but the liquid in the inner cylinder is not cooling down,
i have an heat transfer over the interface between the solid and the liquid regions i checked this and the temperatur of the liquid adjadcent to the solid wall changes,
but the liquid as a whole does not cool down i have waited of hours insimulation and outsimulation but it never changes please help me
i think there has to be somthing wrong with my choosen physics, it is almost like there is an hiden heat source in the liquid
Have you selected Gravity model in Physics?
Check also to ensure that you have not selected constant density for your liquid.
Thank you rwryne and siara817 for your answers, the physics for the solid region of the outer cylinder are: three dimensional/ gradients/ solid: concrete/ implicit unsteady/ constant density/ coupled solid energy the physics for the fluid region of the inner cylinder are: implicit unsteady/ three dimensional/ liquid: Al/ laminar/ polynomial density/ coupled energy/ coupled flow/ gravity so yes gravity is activated (in the right direction i checked) and i have not selected constant density for the liquid natural convection is happening in the simulation it almost looks like as if the whole liquid region is set to isenthalpic but how could that be? i would be very grateful for any suggestion thank you
Dont keep the liquid density as constant. There are options of power law, polynomial in T, Sutherland law etc... ( i m not sure if all these options are present for density...pls check). When temperature effects are present in the simulation..usually it is not recommended to keep the density as constant. With change in temperature, density changes...
see if it works :p
Indeed - if you neglect convection (set Constant Density and/or no Gravity) - your liquid will be cooled down only due to heat conductivity; this will take really much time - taking into consideration its Specific Heat and Heat Conductivity.
please any other ideas?
Does the solid part cover all the liquid? I mean if the liquid will have connection with air, then you need to add a phase for air. Other than this, your solid phase is located in an environment, like air then you need to have some air environment around the solid part. Then the solid part will give off the heat to the air and whole system will cool down.
I guess natural outer convection can be modeled by setting arbitrary outer temperture and heat-exchange coefficient - this could prove the corectness of the model; also - take a closer look at Fluid-Solid Interface surface (In-Place this time i guess) it might be incorrect.
@ siara817 thank you for your answer, yes the inside of the solid part ( a container) is full of the liquid, i have set the outer boundaries of the cylinder to enviromental (293K and 10 W/(m2K)) i thought this would be enough to simulate the air surrounding the container, and the solid of the outer cylinder is reacting like i expected it (could this be my problem and a freefield of air surrounding the container the solution, what do you think?)
@ cwl thanks for helping me, i am not sure what you mean by"I guess natural outer convection can be modeled by setting arbitrary outer temperture and heat-exchange coefficient - this could prove the corectness of the model" but the outer boundary of the solid cylinder is set to enviromental (293k and , W/(m2K) the outer solid regions is reacting like i expected i think the inner liquid cylinder is the problem
the interface is a solid/liquid contact interface (in place) based on my knowledge this should be correct, or am i wrong?
i have tried something: i set the inner cylinder to a gas/solid region in both cases i observed an believable behavior, nothing strange, the whole thing is slowly cooling down (in a believable time), with a cute natural convection in the gas case
because of this i assume the geometry/ mesh etc is not my problem
i am pretty sure the liquid physics is my troublemaker, is there an option i am missing
the physics for the fluid region of the inner cylinder are: implicit unsteady/ three dimensional/ liquid: Al/ laminar/ polynomial density/ coupled energy/ coupled flow/ gravity
any ideas what the fuck (sorry for that) i am doing wrong?
can the preselected. properties of the material ( density etc) be trusted or do i have to make something custom?
>> " i am not sure what you mean by"
i meant exactly what you've done - "i have set the outer boundaries of the cylinder to enviromental (293K and 10 W/(m2K)) "
maybe it would be easier if you upload your model - so we'll be able to look at it closer?
thanks for alle the help
here are the links to
1) my model right @ the beginning of the simulation
2) the simulation after servel hours of simulation, the water is not cooling down and i am really frustrated becaus i am pretty sure its somekind of idiotic fault i should be ashamed of
From what i can see:
0) Inner cylinder of R=0.75m, H=1.6
1) Concrete shell (R_in=0.75, R_out=0.9m)
2) Environment with Heat Transfer Coefficient = 10 W/K*m^-2 and T_env = 293.7 K
3) Initial T0 = 373.7 K
Initial energy of Water (Inner cylinder):
E0 = SpecificHeat * Density * Volume * T0,
where Volume = Pi*R*R*H
Let's evaluate approximate time required for water to be cooled downto T_env (without taking into consideration the concrete shell):
Heat loss to the environment would be:
CylinderSurfaceArea * HeatTransferCoefficient * (T_surface - T_env) * Time;
assuming T_surface to be constant over time (i.e. T_surface = T_0; that is inexact of cource - but we want rough estimation), heat ballance would be:
SpecificHeat * Density * Volume * (T0 - T_env) = CylinderSurfaceArea * HeatTransferCoefficient * (T_0 - T_env) * Time;
which gives us approximate time water requires to cool downto T_env:
Time = SpecificHeat * Density * Volume / CylinderSurfaceArea * HeatTransferCoefficient;
Time = SpecificHeat * Density * R / (2 * HeatTransferCoefficient);
so, Time = 4200 * 1000 * 0.75 / (2 * 10) = 157500 seconds = 43.75 hrs ~ 1.8 days
As far as we have assumed
A) temperature difference between environment and cylinder surface to be constant (while it decreases - and this slows down the cooling process);
B) cylinder to have infinite heat conductivity - i mean its temperature is all the same in space in our evaluation, while in CFD there will be convection - that slows down the cooling process;
both theese lead to the fact that above Time estimation is lower-bound.
Also there is a layer of concrete with Heat Conductivity Coef = 0.53 W/m*K - which (as soon as we take it into consideration) will .. slow down the cooling process again;
So. My idea is that .. man, you've got 2.8 tons of heat insulated water to cool down, imagine the required time; and, yes in your calculation its Temperature is constant, because your Time Step is 1.0E-4 s.
I believe this task should be better solved with (more precise then mentioned above) analytical estimation - with heat conductivity equation for cylindrical/plane wall analytical solution used for concrete and Gr/Pr/Nu numbers used for convection;
@ cwl thanks for your help,
i know that this amount of water will take quite some time to cool down, especially if you consider the shell of concrete,
if you looked @ the simulation "the finished one" of the second link you will see that the time step of 1.0E-4 s was only my initial time step, i gradually rised it to 60 s, and the end time of the simulation was almost 160000 s, after this enormous amount of time the temperature of the inner cylinder has changed next to nothing and this certainly is wrong
this is only a first try and analytical precision is not (yet) needed, i only want to get familiar with star ccm+, precision is my next step
there is something fundamental wrong with my simulation and i cant figure out what it is, could you please give it another look, and tell me what it is?
Well .. your polynomial density looks strange
Plot Density instead of Temperature - your liquid will turn out to have Density ~ 40000 kg/m^3; is that correct? - note that it increases estimation above by 10 times.
If liquid is water - i'd prefer something like this:
Setting such Density leads to an easy-to-see convective motion.
If you set liquid Specific Heat to 100 J/kg-K - you shall see it stratified in 5000 seconds with Temperature difference (between top and bottom) ~ 0.2 K.
Also - it seems more meaningful to use minimum Temperature of liquid monitor - it drops faster than average one, i believe it being more representative.
My conclusion is that your model (especially with fixed Density) works fine, except for the large physical time required for cooling down.
thanks a lot, it was the polynomial density
i thought star ccm+ would automatically set it right if i choose H20, so i ignored it, in hindsight this was not the smartest move
thanks for your help
|All times are GMT -4. The time now is 08:11.|