CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Main CFD Forum

COMSOL - turbulent flow over a plate

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

Reply
 
LinkBack Thread Tools Display Modes
Old   October 2, 2013, 13:09
Default COMSOL - turbulent flow over a plate
  #1
New Member
 
Join Date: Oct 2013
Posts: 7
Rep Power: 3
stenzer is on a distinguished road
Hi guys,

I calculated the cooling of a plate by a turbulent forced convection analytically. Now I want to check my results with COMSOL 4.3 but I have some troubles, maybe someone would be so kind and help me.

My plate is 0.075 m long, to keep the plate at +4 C i need a power of ~130 W. The cooling fluid is air and has a temperature of -30 C with a "inflow" - velocity of 45 m/s.

I tried to model my plate in COMSOL with a rectangle ( 0.075 m x 0.005 m ), this plate is in the upper right corner of an "larger" rectangle. The inlet is on the left. The material of my plate is copper.

My first problem is how to fit the power, because for my analytic approach i have just a surface (~0.017 m^2) but no volume, which is necessary for a heat source with a unit of W/m^3. When I try to run the simulation with "Total Power" equal my required 130 W, the result is far away from my analytical one.

I'm thankful for any advice, I'm pretty new at COMSOL and an electrical engineer so I'm not really familiar with themal stuff ;-).

BR

Last edited by stenzer; October 7, 2013 at 12:33.
stenzer is offline   Reply With Quote

Old   October 2, 2013, 13:26
Default
  #2
Senior Member
 
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 1,600
Rep Power: 23
FMDenaro will become famous soon enough
If I understand correctly your question, you should work by setting the heat flux in W/m^2:

q = - k grad T

so that, by fixing q, you set a non-homogeneous Neumann BC.s

dT/dn|wall = -q/k
FMDenaro is offline   Reply With Quote

Old   October 2, 2013, 14:34
Default
  #3
New Member
 
Join Date: Oct 2013
Posts: 7
Rep Power: 3
stenzer is on a distinguished road
Hi,

I don't know if I understand you correctly.

I calculated the power which is needed to keep my plate at a certain temperature (+4C). So in my opinion I have to model the plate as a heat source and not as heat flux ?!?!????

BR
stenzer is offline   Reply With Quote

Old   October 2, 2013, 17:32
Default
  #4
Senior Member
 
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 1,600
Rep Power: 23
FMDenaro will become famous soon enough
Quote:
Originally Posted by stenzer View Post
Hi,

I don't know if I understand you correctly.

I calculated the power which is needed to keep my plate at a certain temperature (+4C). So in my opinion I have to model the plate as a heat source and not as heat flux ?!?!????

BR

Could you explain your problem by means of a sketch?
FMDenaro is offline   Reply With Quote

Old   October 3, 2013, 04:08
Default
  #5
New Member
 
Join Date: Oct 2013
Posts: 7
Rep Power: 3
stenzer is on a distinguished road
Hi,

here is the link for a sketch, I hope you can read everything.

https://www.dropbox.com/s/ggs1e7wrfvk2y5c/Cooling.jpg

thx
stenzer is offline   Reply With Quote

Old   October 3, 2013, 04:24
Default
  #6
Senior Member
 
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 1,600
Rep Power: 23
FMDenaro will become famous soon enough
it is a 2D model? therefore, your power for m^3 must be considered for 1m of unit lenght in the third direction (outward the sketch plane) in such a way you have a volume.
I think you could model a mixed fluid-copper problem, so that the heat exchange at wall is due to the heat flux. In the copper region you can solve a standard diffusion equation for the temperature which is governed by a parabolic equation like

dT/dt = k Lap T
FMDenaro is offline   Reply With Quote

Old   October 7, 2013, 12:10
Default
  #7
New Member
 
Join Date: Oct 2013
Posts: 7
Rep Power: 3
stenzer is on a distinguished road
Hi,

I did it like you suggested. But it doesn't fit with my "analytical" result. I already checked my calculations, but in my opinoin they a are right.

At +4C the kinematic viscosity (nu) of airis v =13.85e-6 m^2/s, Pr = 0.7116 and the heat conductivity k = 24.6e-3 W/mK.

Thus my Reynolds number is: Re = 243682

Because I want to investigate a plate with a plunt edge I assumed a complete turbulent flow, thus I can calculate my Nusselt number by

Nu = [0.037 * Re^(0.8) * Pr]/[1 + 12.7 * sqrt{ 0.037 * Re^-0.2} * (Pr^(2/3) - 1)] = 626.795

Now I can determine my heat transfere coefficient h and the needed power P to keep the surface at +4C.

h = 205.5 W/(m^2 K)
P = 0.176 m^2 * h * (4C + 30C) = 133 W


I think I made no mistake, but maybe someone can find a mistake or give me any advise how to model that in COMSOL. I'm useing Conjugate Heat Transfer and k - epsilon Turbulent Model.

thx
stenzer is offline   Reply With Quote

Old   October 7, 2013, 12:19
Default
  #8
Senior Member
 
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 1,600
Rep Power: 23
FMDenaro will become famous soon enough
Quote:
Originally Posted by stenzer View Post
Hi,

I did it like you suggested. But it doesn't fit with my "analytical" result. I already checked my calculations, but in my opinoin they a are right.

At +4C the kinematic viscosity (nu) of airis v =13.85e-6 m^2/s, Pr = 0.7116 and the heat conductivity k = 24.6e-3 W/mK.

Thus my Reynolds number is: Re = 243682

Because I want to investigate a plate with a plunt edge I assumed a complete turbulent flow, thus I can calculate my Nusselt number by

Nu = [0.037 * Re^(0.8) * Pr]/[1 + 12.7 * sqrt{ 0.037 * Re^-0.2} * (Pr^(2/3) - 1)] = 626.795

Now I can determine my heat transfere coefficient h and the needed power P to keep the surface at +4C.

h = 205.5 W/(m^2 K)
P = 0.176 m^2 * h * (4C + 30C) = 133 W


I think I made no mistake, but maybe someone can find a mistake or give me any advise how to model that in COMSOL. I'm useing Conjugate Heat Transfer and k - epsilon Turbulent Model.

thx

well, standard results of a flow over a flat plate established that a fully turbulent flow should be achieved for Re number greater than yours ... I think you are still in a transitional region and I am doubtful a k-eps model can manage succesfull such a condition
FMDenaro is offline   Reply With Quote

Old   October 7, 2013, 12:32
Default
  #9
New Member
 
Join Date: Oct 2013
Posts: 7
Rep Power: 3
stenzer is on a distinguished road
Hi,

thank you for your fast reply. I already thougt about that, because the turbulent flow can be assumed for Reynolds numbers between 5*10^5 and 10^7. To be honest I thought that would be modeled by setting the boundary/wall condition as Wall function .

I will calculate the model for a laminar flow and check if the result is correct. But my problem is still that I have to know how a plate with a plunt edge would act. Is there a possibility to get results for such a model???
stenzer is offline   Reply With Quote

Old   October 7, 2013, 12:35
Default
  #10
Member
 
SergeAS's Avatar
 
Serge A. Suchkov
Join Date: Oct 2011
Location: Moscow, Russia
Posts: 73
Blog Entries: 5
Rep Power: 5
SergeAS is on a distinguished road
Send a message via Skype™ to SergeAS
The use of the wall function (as shown on your sketch) for k-eps turbulence model assumes that y+ on the plate is in the range of 30-200, but for heat transfer problems the recommended value of y+ ~ 1 and no wall function (for reasonable results)
SergeAS is offline   Reply With Quote

Old   October 8, 2013, 05:34
Default
  #11
New Member
 
Join Date: Oct 2013
Posts: 7
Rep Power: 3
stenzer is on a distinguished road
Hi SergeAS,

I use conjugate heat transfer, so I think that should be considered by the model automatically!?!?!???

My idea is to calculate and simulate the whole model for a longer plate, thus I get a larger Reeynolds number. And because of the Similitude the result for my smaller plate should be correct. Can I do it that way???

BR

stenzer is offline   Reply With Quote

Old   October 8, 2013, 05:59
Default
  #12
Member
 
SergeAS's Avatar
 
Serge A. Suchkov
Join Date: Oct 2011
Location: Moscow, Russia
Posts: 73
Blog Entries: 5
Rep Power: 5
SergeAS is on a distinguished road
Send a message via Skype™ to SergeAS
Quote:
Originally Posted by stenzer View Post
Hi SergeAS,

I use conjugate heat transfer, so I think that should be considered by the model automatically!?!?!???
I'm not familiar with this product, but I do not think that the inclusion of the option "conjugate heat transfer" is automatically refine your mesh to y + ~ 1

PS: Take a look http://www.comsol.com/blogs/which-tu...d-application/

Quote:
Low Reynolds Number k-epsilon
The Low Reynolds number k-epsilon is similar to the k-epsilon model but does not use wall functions; it solves the flow everywhere. It is a logical extension to k-epsilon and shares many of its advantages, but uses more memory. It is often advisable to use the k-epsilon model to first compute a good initial condition for solving the Low Reynolds number k-epsilon model. Since it does not use wall functions, lift and drag forces and heat flux can be modeled with higher accuracy.

Last edited by SergeAS; October 8, 2013 at 10:11.
SergeAS is offline   Reply With Quote

Old   October 10, 2013, 10:19
Default
  #13
New Member
 
Join Date: Oct 2013
Posts: 7
Rep Power: 3
stenzer is on a distinguished road
Thank you for the link, I will try it with Low Reynolds number k-epsilon.

thx
stenzer 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
problem in turbulent flow over flat plate with stagnation point mb.pejvak Main CFD Forum 0 September 12, 2012 21:25
Turbulent Flow in Straight Square Duct - k-ep Validation mcclud STAR-CCM+ 2 August 7, 2012 16:56
laminar and turbulent flow in one simulation msna FLUENT 0 January 27, 2007 18:35
Flow passing a porous plate. Hao Yu Main CFD Forum 2 October 19, 2000 01:52
Turbulent flow over flat plate Narayanan Main CFD Forum 1 May 8, 2000 07:03


All times are GMT -4. The time now is 02:16.