|
[Sponsors] |
Unexpected Temperature Profile in Rectangular Pipe |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
July 10, 2013, 08:51 |
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 |
|
July 10, 2013, 09:28 |
|
#2 |
Senior Member
Join Date: Jul 2011
Location: Berlin, Germany
Posts: 173
Rep Power: 15 |
What is the result with areAve(Heat Flux) @ Outlet?
There are significant differences between areaInt and areaAve |
|
July 10, 2013, 10:29 |
|
#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, 11:10 |
|
#4 |
Senior Member
Edmund Singer P.E.
Join Date: Aug 2010
Location: Minneapolis, MN
Posts: 511
Rep Power: 21 |
Please check massFlowAve(T)@inlet-outlet instead of areaAve.
|
|
July 10, 2013, 11:35 |
|
#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, 12:03 |
|
#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, 12:27 |
|
#7 |
Senior Member
Edmund Singer P.E.
Join Date: Aug 2010
Location: Minneapolis, MN
Posts: 511
Rep Power: 21 |
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, 12:46 |
|
#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, 15:58 |
|
#9 |
Senior Member
Edmund Singer P.E.
Join Date: Aug 2010
Location: Minneapolis, MN
Posts: 511
Rep Power: 21 |
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, 14:31 |
|
#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 | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
whats the cause of error? | immortality | OpenFOAM Running, Solving & CFD | 13 | March 24, 2021 08:15 |
Calculation of the Governing Equations | Mihail | CFX | 7 | September 7, 2014 07:27 |
how to get surface temperature of pipe at cross section using iso-surface | ashgun | FLUENT | 8 | June 2, 2013 03:03 |
velocity and temperature profile | vickrenz | FLUENT | 0 | August 31, 2009 00:58 |
fluid flow fundas | ram | Main CFD Forum | 5 | June 17, 2000 22:31 |