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

Unexpected Temperature Profile in Rectangular Pipe

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

Reply
 
LinkBack Thread Tools Display Modes
Old   July 10, 2013, 07:51
Default Unexpected Temperature Profile in Rectangular Pipe
  #1
New Member
 
Join Date: Jul 2013
Posts: 9
Rep Power: 0
AlexVin is on a distinguished road
Hi.

I am using CFX 14.0 to get the temperature profile of water flowing into a rectangular micro pipe. The pipe is 100x100x10000 micrometers and it is placed at the center of a substrate made of aluminum. The two plates at the top and bottom surface of the substrate generate 1 W each and the flow in the pipe is laminar with 1.2 [m s^-1] normal velocity at the inlet. Water and Aluminium are taken from the default materials.

See the attached image and the resulting output file for more details.

The problem is that, despite convergence, the average temperature at the outlet is higher than expected. Indeed, in CFX-Post I get:

areaInt (Heat Flux) @ Outlet = 2 [ W ]

and, if Q = C_p MassFlowRate DeltaT,

(areaAve(Temperature)@Outlet - areaAve(Temperature)@Inlet) * (1.2e-8 [m^3 s^-1] * 997.0 [kg m^-3]) * 4181.7 [ J kg^-1 K^-1 ] = 2.214 [ W ]

How is it possible that the heat that should have been generated to cause the DeltaT from inlet to outlet is always 10% higher than the heat flux at the outlet? Does anybody have an explanation? This result is independent from the accuracy of the solution (target residual and domain imbalance) and also from the amount of heat put as source. Always ~10% higher in both steady state or transient with timestep 5e-3 [ s ].

Thanks

AlexVin
Attached Images
File Type: jpg PipeMesh.jpg (86.1 KB, 9 views)
Attached Files
File Type: txt RectMicroPipe_001.txt (51.6 KB, 4 views)
AlexVin is offline   Reply With Quote

Old   July 10, 2013, 08:28
Default
  #2
Senior Member
 
Join Date: Jul 2011
Location: Berlin, Germany
Posts: 120
Rep Power: 6
monkey1 is on a distinguished road
What is the result with areAve(Heat Flux) @ Outlet?
There are significant differences between areaInt and areaAve
monkey1 is offline   Reply With Quote

Old   July 10, 2013, 09:29
Default
  #3
New Member
 
Join Date: Jul 2013
Posts: 9
Rep Power: 0
AlexVin is on a distinguished road
areaInt (Heat Flux)@Outlet = -1.996e+00 [W]
areaAve (Heat Flux)@Outlet = -1.996e+08 [W m^-2]

btw, the outlet is indeed 100x100 um^2 (1e-8 m^2)
AlexVin is offline   Reply With Quote

Old   July 10, 2013, 10:10
Default
  #4
Senior Member
 
Edmund Singer P.E.
Join Date: Aug 2010
Location: Minneapolis, MN
Posts: 495
Rep Power: 11
singer1812 is on a distinguished road
Please check massFlowAve(T)@inlet-outlet instead of areaAve.
singer1812 is offline   Reply With Quote

Old   July 10, 2013, 10:35
Default
  #5
New Member
 
Join Date: Jul 2013
Posts: 9
Rep Power: 0
AlexVin is on a distinguished road
areaAve(T)@Outlet = 343.7 [K]
massFlowAve(T)@Outlet = 338.2 [K]

therefore now

(massFlowAve(T)@Outlet - massFlowAve(T)@Inlet) * (1.2e-8 * 997.0) [kg s^-1] * 4181.7 [J kg^-1 K^-1] = 1.998e+00 [W]

which matches with the 2 W given as total source. Thank You singer1812 !!
AlexVin is offline   Reply With Quote

Old   July 10, 2013, 11:03
Default
  #6
New Member
 
Join Date: Jul 2013
Posts: 9
Rep Power: 0
AlexVin is on a distinguished road
Hi again

do you mind helping me with another last issue? I'd like to profile the quantity massFlowAve(T) over a plane that moves along the direction of the channel.

I created a plane CrossSection in the domain "Channel" and placed on the plane XY at Z=100 micron. Now,

massFlowAve(T)@CrossSection = 300 K

how can I make a plot, or extract a csv file with Z = 0:100:10000 ?

Thanks again

AV
AlexVin is offline   Reply With Quote

Old   July 10, 2013, 11:27
Default
  #7
Senior Member
 
Edmund Singer P.E.
Join Date: Aug 2010
Location: Minneapolis, MN
Posts: 495
Rep Power: 11
singer1812 is on a distinguished road
Not sure what you mean. You want a plot of average cross section T at 3 different locations (z= 0 , 100, and 1000)?

Cant you just do that by hand?
singer1812 is offline   Reply With Quote

Old   July 10, 2013, 11:46
Default
  #8
New Member
 
Join Date: Jul 2013
Posts: 9
Rep Power: 0
AlexVin is on a distinguished road
Nope ... every 100. for (i=0 ; i != 10000 ; i += 100)
AlexVin is offline   Reply With Quote

Old   July 10, 2013, 14:58
Default
  #9
Senior Member
 
Edmund Singer P.E.
Join Date: Aug 2010
Location: Minneapolis, MN
Posts: 495
Rep Power: 11
singer1812 is on a distinguished road
Are you familiar with PERL? You can use that within CFX post. This will allow you to automate the plane movement, data collection, and data write out.
singer1812 is offline   Reply With Quote

Old   July 11, 2013, 13:31
Default
  #10
New Member
 
Join Date: Jul 2013
Posts: 9
Rep Power: 0
AlexVin is on a distinguished road
Ok. I'll have a look to PERL. I was expecting some automatic way, as chart or export

Thanks again
AlexVin is offline   Reply With Quote

Reply

Tags
fluid flow, heat flux, micropipe, temperature problem

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
Calculation of the Governing Equations Mihail CFX 7 September 7, 2014 06:27
whats the cause of error? immortality OpenFOAM Running, Solving & CFD 11 April 22, 2014 12:32
how to get surface temperature of pipe at cross section using iso-surface ashgun FLUENT 8 June 2, 2013 02:03
velocity and temperature profile vickrenz FLUENT 0 August 30, 2009 23:58
fluid flow fundas ram Main CFD Forum 5 June 17, 2000 21:31


All times are GMT -4. The time now is 02:53.