# Unexpected Temperature Profile in Rectangular Pipe

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

July 10, 2013, 07:51
Unexpected Temperature Profile in Rectangular Pipe
#1
New Member

Join Date: Jul 2013
Posts: 9
Rep Power: 0
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
 PipeMesh.jpg (86.1 KB, 10 views)
Attached Files
 RectMicroPipe_001.txt (51.6 KB, 4 views)

 July 10, 2013, 08:28 #2 Senior Member   Join Date: Jul 2011 Location: Berlin, Germany Posts: 153 Rep Power: 7 What is the result with areAve(Heat Flux) @ Outlet? There are significant differences between areaInt and areaAve

 July 10, 2013, 09:29 #3 New Member   Join Date: Jul 2013 Posts: 9 Rep Power: 0 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)

 July 10, 2013, 10:10 #4 Senior Member   Edmund Singer P.E. Join Date: Aug 2010 Location: Minneapolis, MN Posts: 512 Rep Power: 12 Please check massFlowAve(T)@inlet-outlet instead of areaAve.

 July 10, 2013, 10:35 #5 New Member   Join Date: Jul 2013 Posts: 9 Rep Power: 0 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 !!

 July 10, 2013, 11:03 #6 New Member   Join Date: Jul 2013 Posts: 9 Rep Power: 0 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

 July 10, 2013, 11:27 #7 Senior Member   Edmund Singer P.E. Join Date: Aug 2010 Location: Minneapolis, MN Posts: 512 Rep Power: 12 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?

 July 10, 2013, 11:46 #8 New Member   Join Date: Jul 2013 Posts: 9 Rep Power: 0 Nope ... every 100. for (i=0 ; i != 10000 ; i += 100)

 July 10, 2013, 14:58 #9 Senior Member   Edmund Singer P.E. Join Date: Aug 2010 Location: Minneapolis, MN Posts: 512 Rep Power: 12 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.

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

 Tags fluid flow, heat flux, micropipe, temperature problem

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Mihail CFX 7 September 7, 2014 06:27 immortality OpenFOAM Running, Solving & CFD 11 April 22, 2014 12:32 ashgun FLUENT 8 June 2, 2013 02:03 vickrenz FLUENT 0 August 30, 2009 23:58 ram Main CFD Forum 5 June 17, 2000 21:31

All times are GMT -4. The time now is 04:20.