CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > FLUENT > Fluent Multiphase

Wall heat transfer

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   March 23, 2016, 06:42
Default
  #41
Senior Member
 
Jordi Pina
Join Date: Mar 2015
Posts: 157
Rep Power: 7
jpina is on a distinguished road
Btw, when you mean "Heat transfer coefficient for laminar flows is simply given by conservation of thermal energy, conduction on one side and convection on other".

In a fixed temperature approach:

q=h_fluid*(T_wall-T_fluid)

In the solid we have:

q=k_solid/\Delta{n}*(Twall-T_s)

http://www.afs.enea.it/project/neptu...l-calc-temp-fl

So that:

h_fluid*(T_wall-T_fluid)=k_solid/n*(T_wall-T_s)

h_fluid=k_solid/n*(T_wall-T_s)/(T_wall-T_fluid)

So that, how you said yesterday, I have to modify k_solid for artificially touching the h value.

Last edited by jpina; March 23, 2016 at 07:43.
jpina is offline   Reply With Quote

Old   March 23, 2016, 06:47
Default
  #42
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,948
Blog Entries: 1
Rep Power: 31
vinerm will become famous soon enough
I said No CFD Tool
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Old   March 23, 2016, 07:14
Default
  #43
Senior Member
 
Jordi Pina
Join Date: Mar 2015
Posts: 157
Rep Power: 7
jpina is on a distinguished road
Thanks vinerm, the point confused me.

Can you take a look at my previous post, where I state that:

h_fluid=k_s/n*(T_w-T_s)/(T_w-T_f)

My doubts are:

- Why doesn't k_fluid appear in my equation? k_fluid should has some effect in the h_fluid!

- And second thing, wonder that T_wall is 523K. T_s is the reference temperature of the solid, which would be also 523K.

We would have: h_fluid=k_solid/n*0

Not logical!

Well, I think that my solution is to name as Wall an edge of the fluid. Set fixed temperature and, for artificially increasing the h_fluid, increase k_s.

However, when I look at the ANSYS help I found that the heat transfer coefficient is calculated with:



Where is this equation used? As far as I understand, in the fluid there's convection and this is the Fourier equation for conduction!

I would like, however, to control all the theory. If somebody could give light to me I would appreciate it.
jpina is offline   Reply With Quote

Old   March 23, 2016, 09:25
Default
  #44
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,948
Blog Entries: 1
Rep Power: 31
vinerm will become famous soon enough
I ain't sure what literature you referred. Let me clarify it including my statement about thermal conservation. Thermal energy can be transferred within a single medium by diffusion, you may call it conduction as well, and by thermal radiation. Let's forget about radiation for time being. So, within a medium, it is conduction that transfers thermal energy until and unless medium is in motion. Most of the time when we consider solid, it is stationary. And fluid is in motion. Now, conduction requires different temperatures at two spatially different locations within any medium, be it fluid or solid. That's how we calculate gradient, dT/dx or (T_wall -
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Old   March 23, 2016, 09:28
Default
  #45
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,948
Blog Entries: 1
Rep Power: 31
vinerm will become famous soon enough
(T_wall - T_solid)/(x_wall - x_solid). x for wall is certainly position coordinate of wall. x for solid can be any location as long as this position lies on vector normal to wall. T_solid is temperature of solid at that location. If T_wall and T_solid are same, there will not be any thermal energy or heat transfer at all. This is call thermal equilibrium.
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Old   March 23, 2016, 09:33
Default
  #46
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,948
Blog Entries: 1
Rep Power: 31
vinerm will become famous soon enough
In other words, temperature of solid mold had to be higher near wall and lower away from it so that heat could transfer from inside to outside. But this heat has to come from somewhere. So, it has to be equal to hear transferred from liquid to solid. Though this transfer mechanism is also conduction, we cannot use conduction equation to determine this because fluid is in motion. If fluid is static, like water in a bottle, then there is only conduction. However, here fluid is in motion, so, heat transfer is given by product of h with difference in temperatures of fluid and wall. So, thermal energy lost by fluid has to be equal to that gained by solid. That's what conservation implies. Furthermore, solid will lose it to environment
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Old   March 23, 2016, 09:35
Default
  #47
Senior Member
 
Jordi Pina
Join Date: Mar 2015
Posts: 157
Rep Power: 7
jpina is on a distinguished road
But I don't have any "solid" zone in my model. I have just called "wall" to the edge where the wall lies and assigned a fixed temperature. How can Fluent then transfer the heat in the solid, if there is no solid?
jpina is offline   Reply With Quote

Old   March 23, 2016, 09:38
Default
  #48
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,948
Blog Entries: 1
Rep Power: 31
vinerm will become famous soon enough
Thermal conductivity of fluid does into picture via h. h is a function of fluid and flow properties, i.e., velocity, density, viscosity, conductivity, and specific heat. You change any one of these, h changes. However, since they don't affect individually, you may change these in a manner so that h remains as it is. These regulations are called non-dimensional groups, Re and Pr for forced convection.
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Old   March 23, 2016, 09:57
Default
  #49
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,948
Blog Entries: 1
Rep Power: 31
vinerm will become famous soon enough
If you do not have solid, then you do not have to worry about T_solid. T_wall is common and Fluent will calculate h. It is on you to decide whether you wish to apply q on wall or T. You can't control both.
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Old   March 24, 2016, 05:46
Default
  #50
Senior Member
 
Jordi Pina
Join Date: Mar 2015
Posts: 157
Rep Power: 7
jpina is on a distinguished road
Dear vinerm,

yesterday I tried to increase the velocity at which the polymer freezes.

Using a fixed temperature value of the wall, I can only increase the freezing speed by changing the material properties, am I right?

I tried increasing a lot the thermal conductivity of the polymer but I didn't succeed, it needs very big k values, etc.. I will try to increase the thermal conductivity of the solid, but I don't think it will have a big effect.

How could I increase the heat transfer speed? I cannot increase neither the velocity of the polymer or the wall temperature, since these ara values that I want to control.

If I want to do a UDF setting a q value, how could I make the following:

if VOF=1
q=h*(Twall-Tfluid)
if VOF=0
q=0
end if

Thanks!

Is there something more than the thermal conductivity?
jpina is offline   Reply With Quote

Old   March 24, 2016, 06:20
Default
  #51
Senior Member
 
Jordi Pina
Join Date: Mar 2015
Posts: 157
Rep Power: 7
jpina is on a distinguished road
Dear Vinerm,

I have found this tutorial:

https://www.ndsu.edu/me/images/Kallm...%20Example.pdf

And I am VERY confused, here it says:

"The Film Coefficient on the inside of the pipe is 1200 (fluid temperature is 450), and the Film Coefficient on the outside of the pipe is 200 (air temperature is 300). "

And:

"ANSYS Main Menu - Solution - Define Loads - Apply - Thermal - Convection - On Areas - Select (with the mouse) the Areas defining the inside of the pipe (A5 and A6 in this case) - OK - Enter 1200 for ‘Film coefficient’ and 450 for ‘Bulk temperature’ - OK "

It looks like that they can fix a convection heat transfer coefficient, which is something that I understood that you said it was not possible:

"No CFD tool will allow fixing h on fluid-solid interface where fluid flow is being simulated. That renders the whole idea of simulation useless." Vinerm.

What is happening? I'm totally confused now...

Thanks!

Last edited by jpina; March 24, 2016 at 07:38.
jpina is offline   Reply With Quote

Old   March 24, 2016, 07:31
Default
  #52
Senior Member
 
Jordi Pina
Join Date: Mar 2015
Posts: 157
Rep Power: 7
jpina is on a distinguished road
Maybe I should solve my problem using ANSYS Thermal Transient analysis instead of ANSYS Fluent??
jpina is offline   Reply With Quote

Old   March 28, 2016, 06:14
Default
  #53
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,948
Blog Entries: 1
Rep Power: 31
vinerm will become famous soon enough
What you're referring to as Ansys here is essentially a structural solver and does not solve any fluid flow. This can only predict temperature inside solid objects and not fluid. Hence, this requires specification of conditions on both sides of solid. You can use any type on any side. Choice of tool is driven by objective. If your objective is clearly defined, choice is rather easy.
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Old   March 30, 2016, 05:15
Default
  #54
Senior Member
 
Jordi Pina
Join Date: Mar 2015
Posts: 157
Rep Power: 7
jpina is on a distinguished road
Dear vinerm,

I have spoken with the author of the paper and his answer has surprised me a lot:

------------------------
The heat transfer coefficient was kept constant in each simulation. A parametric study was carried out to see which value best fitted with the experiemental results. How you do this in Ansys you must figure out yourself. That being said.
1. The simulation results are highly sensitive to the choice of h
2. We do not really know what h should be at those temperature gradients (in time and space) and shear rates since there was no good way of measuring them as I wrote this paper. Also, I would question the concept of a constant heat transfer coefficient at those conditions, but it was the best I had.
------------------------
How could I do this in Fluent? :S
jpina is offline   Reply With Quote

Old   March 30, 2016, 16:48
Default
  #55
Senior Member
 
Jordi Pina
Join Date: Mar 2015
Posts: 157
Rep Power: 7
jpina is on a distinguished road
After a lot of research, I've finally found how to set a constant heat transfer coefficient. I copy what I've found and used:

5. Wall Heat Flux

The wall heat flux function ( DEFINE_HEAT_FLUX) can be used to modify
the way that the solver computes the heat flux between
a wall and the neighboring fluid cells. For example, you can customize
the heat transfer coefficient or the law-of-the-wall for
temperature. The UDF presented below uses an internal heat transfer
coefficient to specify the wall heat flux. It is another example
of a UDF that utilizes the ADJUST function to adjust a computed value,
and it is executed as a compiled UDF.

The diffusive heat flux coefficients ( cid) are specified in this UDF.
The diffusive heat flux ( qid) will then be computed by
FLUENT using the following equation:

qid = cid[0] + cid[1]*C_T(c0,t0) - cid[2]*F_T(f,t) -
cid[3]*pow(F_T(f,t),4)

/************************************************** *********************/
/* UDF for specifying the diffusive heat flux between a wall and
*/
/* neighboring cells
*/
/************************************************** *********************/

#include "udf.h"

static real h = 0.; /* heat transfer coefficient (W/m^2 C)
*/

DEFINE_ADJUST(htc_adjust, domain)
{
/* Define the heat transfer coefficient. */

h = 120;
}

DEFINE_HEAT_FLUX(heat_flux, f, t, c0, t0, cid, cir)
{
cid[0] = 0.;
cid[1] = h;
cid[2] = h;
cid[3] = 0.;
}
jpina is offline   Reply With Quote

Old   March 31, 2016, 13:03
Default
  #56
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,948
Blog Entries: 1
Rep Power: 31
vinerm will become famous soon enough
DEFINE_HEAT_FLUX is not meant for defining heat flux or heat transfer coefficient, rather how temperature and heat flux are related. Yes, you may use it to force Fluent to have a specific value of h, however, that would be a manufactured solution and won't represent a real scenario. That implies a solution, which might have some academic interest but no use or application. If a coefficient of 5000 cannot be achieved either in lab or industry, then it is of no use. And if it can be, then Fluent will also be able to predict it.
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Old   April 1, 2016, 08:00
Default
  #57
Senior Member
 
Jordi Pina
Join Date: Mar 2015
Posts: 157
Rep Power: 7
jpina is on a distinguished road
Hello Vinerm,

I know that with DEFINE_HEAT_FLUX macro I override the rigorous calculation of the HTC.

The fact is that in the nano-world, the physics behind the heat transfer is different from the macro-world one. Heat transfer in the nano-world is according to the literature bigger than in the macro-world, hence, itís useful to override the calculation of the heat transfer with a HTC that correlates the simulations with the experimental work. Maybe in the future, the physics of the nano-world will be understood and will be possible to calculate the HTC, since then our trick is to set an HTC that fits in with the experimental results.

Thanks!
jpina is offline   Reply With Quote

Old   April 1, 2016, 23:55
Default
  #58
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,948
Blog Entries: 1
Rep Power: 31
vinerm will become famous soon enough
That's correct. However, nano and macro world are not disconnected. Nano regime will disperse only that energy which it will receive and what it receives is given by htc. Nano scale will not generate is own heat. As I mentioned earlier, htc is not something real, rather an averaged effect that is used to represent thermal energy carryover by moving bodies. Anyway, give it a try by specifying high value and if some issue is faced, then it can be resolved.
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
How to set heat transfer coefficient and wall temperature jpina FLUENT 1 March 21, 2016 09:47
Use of Wall Function Heat Transfer co-efficient mohibanwar FLUENT 1 September 8, 2015 02:02
Flow around pipes - heat transfer coefficient on the wall of pipe doodek Main CFD Forum 2 November 23, 2009 09:48
Convective / Conductive Heat Transfer in Hypersonic flows enigma Main CFD Forum 2 November 1, 2009 23:53
How can I increase Heat Transfer at Domain Interf? B.Simon CFX 3 October 28, 2008 19:53


All times are GMT -4. The time now is 15:25.