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

Heat transfer

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

Like Tree4Likes
  • 1 Post By BlackHeartInertia
  • 1 Post By LuckyTran
  • 1 Post By LuckyTran
  • 1 Post By BlackHeartInertia

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   May 24, 2017, 00:56
Default Heat transfer
  #1
New Member
 
BlackHeartInertia
Join Date: May 2017
Posts: 29
Rep Power: 7
BlackHeartInertia is on a distinguished road
HI. How do you simulate heat transfer in fluent?
In my case Im using a wall made of 100 mm of steel and 200 mm of firebrick but In my 3d model I just made the fluid domain because Im using the option shell conduction.
I thought about
1. Define a new material with an equivalent k
2. Modify the 3d model and made a wall for steel and a wall for firebrick

Sent from my SM-G570M using CFD Online Forum mobile app
Светлана likes this.
BlackHeartInertia is offline   Reply With Quote

Old   May 25, 2017, 21:40
Default
  #2
Senior Member
 
Svetlana Tkachenko
Join Date: Oct 2013
Location: Australia, Sydney
Posts: 405
Rep Power: 13
Светлана is on a distinguished road
You can do a hand calculation to merge these two walls into one, and supply that to Fluent.

Particularly for one wall the fourier law says

q = k * dT / L <-- Fourier law

For two walls you have

q1 = k1 * dT1 / L1 <-- Fourier law wall 1
q2 = k2 * dT2 / L2 <-- Fourier law wall 2

But in equilibrium these two amounts are the same so

k1 * dT1 / L1 = k2 * dT2 / L2 <-- energy equilibrium at wall interface

And we also know what dT2 + dT1 is, let's call it dTtotal (we know it because the solver will rely on 'T internal - T ambient' and this is the total T difference)

Two equations now:

1) k1 * dT1 / L1 = k2 * dT2 / L2

2) dT1 + dT2 = dTtotal

We have 2 equations and 2 unknowns here. These unknowns are dT1 and dT2. We need to find value of either of them and plug it back into the "Fourier law wall 1" equation.

Therefore (from equation 2)

dT2 = dTtotal - dT1

Therefore (plug this back into equation 1)

k1 * dT1 / L1 = k2 * (dTtotal - dT1) / L2

Therefore (open the brackets)

k1 * dT1 / L1 = k2 * dTtotal / L2 - k2 * dT1 / L2

Therefore (move one term to the LHS)

k1 * dT1 / L1 + k2 * dT1 / L2 = k2 * dTtotal / L2

Therefore (group)

dT1 * (k1 / L1 + k2 / L2) = k2 * dTtotal / L2

Therefore now we know dT1

dT1 = k2 * dTtotal / (L2 * (k1 / L1 + k2 / L2))

Therefore we can now put this back into the heat flux formula as told before

q = k1 * dT1 / L1 = k1 * k2 * dTtotal / (L2 * L1 * (k1 / L1 + k2 / L2)) = k1 * k2 * dTtotal / (k1 * L2 + k2 * L1)

Now what is the meaning of this? We can write it in a more meaningful form:

q = k1 * k2 * dTtotal / (k1 * L2 + k2 * L1) = dTtotal / (L2/k2 + L1/k1)

It means that L/k is the material resistance to conduction and it is allowed to add them for multi layer walls.

You can see the same thing explained (but not derived) at this page:

http://scientificsentence.net/Thermo...Thermal_Energy

Then you can tell Fluent any wall conduction and any wall thickness you like, for one walls only, as long as L/k for the new wall (its thickness divided by its material conductivity) equals to (L2/q2 + L1/q1).

Please correct me if I am wrong here. I am not familiar with your problem so I may have missed something essential.
Светлана is offline   Reply With Quote

Old   May 26, 2017, 00:53
Default
  #3
Senior Member
 
Lucky
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 5,112
Rep Power: 60
LuckyTran has a spectacular aura aboutLuckyTran has a spectacular aura aboutLuckyTran has a spectacular aura about
Quote:
Originally Posted by BlackHeartInertia View Post
2. Modify the 3d model and made a wall for steel and a wall for firebrick
I would recommend to always start with 2 until you run into some serious technical issues like running out of RAM or something. Fluent is a 3D tool and you need to be using it as a 3D tool, otherwise you shouldn't be using Fluent.
Светлана likes this.
LuckyTran is offline   Reply With Quote

Old   May 28, 2017, 20:02
Default mesh wall?
  #4
Senior Member
 
Svetlana Tkachenko
Join Date: Oct 2013
Location: Australia, Sydney
Posts: 405
Rep Power: 13
Светлана is on a distinguished road
Do you mean that it would be better to include the wall into the computational domain, mesh it, and include it in the calculations?

If so, it could be perhaps interesting to check how much the results differ from those obtained with a 1d Fourier law assumption. In some cases this is very important but not in others.
Светлана is offline   Reply With Quote

Old   May 28, 2017, 20:29
Default
  #5
Senior Member
 
Lucky
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 5,112
Rep Power: 60
LuckyTran has a spectacular aura aboutLuckyTran has a spectacular aura aboutLuckyTran has a spectacular aura about
Quote:
Originally Posted by Светлана View Post
Do you mean that it would be better to include the wall into the computational domain, mesh it, and include it in the calculations?
Yes. Mesh it and run it.

Quote:
Originally Posted by Светлана View Post
If so, it could be perhaps interesting to check how much the results differ from those obtained with a 1d Fourier law assumption. In some cases this is very important but not in others.
Again Fluent is a 3D tool (or 2D, but definitely more than 1D). 1D calculations can be done on pen and paper (or excel/mathcad/matlab). You don't walk into a casino, sit at a poker table, and try to play blackjack.
Светлана likes this.
LuckyTran is offline   Reply With Quote

Old   May 28, 2017, 21:07
Default it's a bc
  #6
Senior Member
 
Svetlana Tkachenko
Join Date: Oct 2013
Location: Australia, Sydney
Posts: 405
Rep Power: 13
Светлана is on a distinguished road
I think this is a boundary condition. They have a multi dimensional computational domain and 1d heat transfer on one of its boundaries.
Светлана is offline   Reply With Quote

Old   May 29, 2017, 20:00
Default
  #7
New Member
 
BlackHeartInertia
Join Date: May 2017
Posts: 29
Rep Power: 7
BlackHeartInertia is on a distinguished road
Ok, I have included the walls as a solid with design geometry but Im not sure if I just have to specify the material in the cell zone conditions.. or i need to specify wall boundary conditions too at thermal like shell conduction? Because my results are different now


Sent from my SM-G570M using CFD Online Forum mobile app
Светлана likes this.
BlackHeartInertia is offline   Reply With Quote

Old   May 29, 2017, 23:52
Default convection
  #8
Senior Member
 
Svetlana Tkachenko
Join Date: Oct 2013
Location: Australia, Sydney
Posts: 405
Rep Power: 13
Светлана is on a distinguished road
Oh, sorry! For me shell conduction is confusing. It expects you to specify a heat generation rate as a constant. I don't know what to put there.

Instead, I personally select convection option in the thermal tab, and supply the value of

1/ (L2/k2 + L1/k1)

as the heat transfer coefficient there. The free stream temperature is the ambient temperature on the outside of the wall.
Светлана is offline   Reply With Quote

Old   June 19, 2017, 09:30
Default
  #9
New Member
 
BlackHeartInertia
Join Date: May 2017
Posts: 29
Rep Power: 7
BlackHeartInertia is on a distinguished road
Quote:
Originally Posted by Светлана View Post
Oh, sorry! For me shell conduction is confusing. It expects you to specify a heat generation rate as a constant. I don't know what to put there.

Instead, I personally select convection option in the thermal tab, and supply the value of

1/ (L2/k2 + L1/k1)

as the heat transfer coefficient there. The free stream temperature is the ambient temperature on the outside of the wall.
Thank you very much . I used temperature and shell conduction. But im not sure if the temperature is for the inner or outer surface of the "wall" :s

Sent from my SM-G570M using CFD Online Forum mobile app
BlackHeartInertia is offline   Reply With Quote

Reply

Tags
heat tranfer, wall

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
Heat transfer using all modes bhups45 FLUENT 0 June 19, 2016 08:02
Error finding variable "THERMX" sunilpatil CFX 8 April 26, 2013 08:00
Question about heat transfer simulation Anna Tian Main CFD Forum 0 January 25, 2013 19:53
Heat Transfer in Porous Medium eryan STAR-CD 0 September 28, 2010 14:14
Convective Heat Transfer - Heat Exchanger Mark CFX 6 November 15, 2004 16:55


All times are GMT -4. The time now is 21:05.