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

Cooling behavior of liquid aluminum in a closed container

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

Reply
 
LinkBack Thread Tools Display Modes
Old   May 6, 2013, 13:06
Unhappy Cooling behavior of liquid aluminum
  #1
New Member
 
Join Date: May 2013
Posts: 12
Rep Power: 4
§$§eth is on a distinguished road
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
Attached Images
File Type: jpg Unbenannt3.jpg (44.5 KB, 26 views)
File Type: jpg Unbenannt4.jpg (39.3 KB, 20 views)

Last edited by §$§eth; May 7, 2013 at 09:28. Reason: Old problem solved new problem found
§$§eth is offline   Reply With Quote

Old   May 8, 2013, 09:28
Default
  #2
Senior Member
 
siara817's Avatar
 
siamak rahimi ardkapan
Join Date: Jul 2010
Location: Copenhagen, Denmark
Posts: 218
Rep Power: 9
siara817 is on a distinguished road
Have you selected Gravity model in Physics?
Check also to ensure that you have not selected constant density for your liquid.
__________________
Good luck
Siamak
siara817 is offline   Reply With Quote

Old   May 8, 2013, 10:58
Default
  #3
Super Moderator
 
Ryne Whitehill
Join Date: Aug 2009
Posts: 313
Rep Power: 9
rwryne is on a distinguished road
Quote:
Originally Posted by siara817 View Post
Have you selected Gravity model in Physics?
Check also to ensure that you have not selected constant density for your liquid.
And when you do turn on gravity, make sure its pointing the right direction. I think it defaults to -Z but not sure.
rwryne is offline   Reply With Quote

Old   May 9, 2013, 16:14
Default
  #4
New Member
 
Join Date: May 2013
Posts: 12
Rep Power: 4
§$§eth is on a distinguished road
Thank you rwryne and siara817 for your answers, the physics for the solid region of the outer cylinder are: three dimensional/ gradients/ solid: concrete/ implicit unsteady/ constant density/ coupled solid energy the physics for the fluid region of the inner cylinder are: implicit unsteady/ three dimensional/ liquid: Al/ laminar/ polynomial density/ coupled energy/ coupled flow/ gravity so yes gravity is activated (in the right direction i checked) and i have not selected constant density for the liquid natural convection is happening in the simulation it almost looks like as if the whole liquid region is set to isenthalpic but how could that be? i would be very grateful for any suggestion thank you
§$§eth is offline   Reply With Quote

Old   May 10, 2013, 02:26
Default
  #5
New Member
 
Join Date: Feb 2013
Posts: 7
Rep Power: 4
rajeev50588 is on a distinguished road
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
rajeev50588 is offline   Reply With Quote

Old   May 11, 2013, 06:44
Default
  #6
cwl
Member
 
Chaotic Water
Join Date: Jul 2012
Posts: 51
Rep Power: 4
cwl is on a distinguished road
Send a message via Skype™ to cwl
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.
cwl is offline   Reply With Quote

Old   May 11, 2013, 15:05
Default
  #7
New Member
 
Join Date: May 2013
Posts: 12
Rep Power: 4
§$§eth is on a distinguished road
Quote:
Originally Posted by §$§eth View Post
....the physics for the fluid region of the inner cylinder are: .... polynomial density/....
thank you for all your help but the liquid is not set to constant density (as i already wrote)

please any other ideas?
§$§eth is offline   Reply With Quote

Old   May 12, 2013, 04:48
Default
  #8
Senior Member
 
siara817's Avatar
 
siamak rahimi ardkapan
Join Date: Jul 2010
Location: Copenhagen, Denmark
Posts: 218
Rep Power: 9
siara817 is on a distinguished road
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.
__________________
Good luck
Siamak
siara817 is offline   Reply With Quote

Old   May 12, 2013, 10:56
Default
  #9
cwl
Member
 
Chaotic Water
Join Date: Jul 2012
Posts: 51
Rep Power: 4
cwl is on a distinguished road
Send a message via Skype™ to cwl
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.
cwl is offline   Reply With Quote

Old   May 15, 2013, 15:44
Default
  #10
New Member
 
Join Date: May 2013
Posts: 12
Rep Power: 4
§$§eth is on a distinguished road
@ 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?
§$§eth is offline   Reply With Quote

Old   May 15, 2013, 16:23
Default
  #11
cwl
Member
 
Chaotic Water
Join Date: Jul 2012
Posts: 51
Rep Power: 4
cwl is on a distinguished road
Send a message via Skype™ to cwl
2§$§eth
>> " 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?
cwl is offline   Reply With Quote

Old   May 16, 2013, 09:37
Default
  #12
New Member
 
Join Date: May 2013
Posts: 12
Rep Power: 4
§$§eth is on a distinguished road
thanks for alle the help

here are the links to

1) my model right @ the beginning of the simulation
http://www.mediafire.com/?k20huezr8bx2432

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
http://www.mediafire.com/?ogb4v87sfw37390
§$§eth is offline   Reply With Quote

Old   May 16, 2013, 15:45
Default
  #13
cwl
Member
 
Chaotic Water
Join Date: Jul 2012
Posts: 51
Rep Power: 4
cwl is on a distinguished road
Send a message via Skype™ to cwl
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 is offline   Reply With Quote

Old   May 17, 2013, 04:40
Default
  #14
New Member
 
Join Date: May 2013
Posts: 12
Rep Power: 4
§$§eth is on a distinguished road
@ 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?

thanks
§$§eth is offline   Reply With Quote

Old   May 17, 2013, 09:53
Default
  #15
cwl
Member
 
Chaotic Water
Join Date: Jul 2012
Posts: 51
Rep Power: 4
cwl is on a distinguished road
Send a message via Skype™ to cwl
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.

Quote:
if you looked @ the simulation "the finished one" of the second link
I'm sorry - i have missed it :<

Quote:
i only want to get familiar with star ccm+
I'd say that such task is not good for your purpose; as far as i understand - unless you keep residuals low (1e-4..1e-3) - heat transfer due to convection might be easily "eaten" by numerical errors (they are of the same order in your task i guess), which leads to much more than 5 inner iterations per time step.

My conclusion is that your model (especially with fixed Density) works fine, except for the large physical time required for cooling down.
cwl is offline   Reply With Quote

Old   May 21, 2013, 05:29
Default
  #16
New Member
 
Join Date: May 2013
Posts: 12
Rep Power: 4
§$§eth is on a distinguished road
@cwl

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
§$§eth 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
How to create liquid gaseous interaction in the same container? haristrawberry CFX 4 June 14, 2015 06:54
inflow into closed container ehooi Main CFD Forum 9 June 13, 2011 05:03
radiation of molton liquid metal in enclosure richard CFX 0 April 8, 2008 15:43
Need some help for total liquid fraction linus FLUENT 0 December 19, 2006 04:29
pressure distribution in a closed container prasanth FLUENT 3 December 21, 2003 08:21


All times are GMT -4. The time now is 19:21.