
[Sponsors] 
January 19, 2014, 20:45 
Extremely high fluid temperatures with simple model

#1 
New Member
Jason
Join Date: Jan 2014
Posts: 5
Rep Power: 4 
Hi all,
I recently ran into an issue with extremely high solved steady state temperature values within the solid and fluid when a volume/surface heat source is defined (in Watts, or Watts/m^2) in FloEFD. The model was simplified to have an external air flow (v(x) = 1 m/s) past a rectangular block (3.56 x 4.32 x 2.20 mm), where the rectangular block was a heat source of 5 W. The rectangular block was a solid made of Stainless steel 321 (Predefined) with k = 15.1 W/mK @ 300K. The resulting temperature profile looks correct: stagnant flow on the front edge of the block, with flow trails on the other faces. The issue here is that the maximum temperature of the fluid is about 900 K. A quick calculation shows that the change in temperature should only be about 15 K, and not 600 K. Is there something I am missing in the physics, or is there something I am not addressing when creating the model? Thank you. More information: Quick calculation: Q_out (rectangle block) = Q_in (into fluid) 5 W = dm/dt * c(air) * dT 5 W = v * (cross sectional area of computational domain) * density (air) * c(air) * dT 5 W = 1 m/s * 0.015 m * 0.0175 m * density(air) * c(air) * dT 5 W = 1 m/s * 0.015 m * 0.0175 m * ~1.2 kg/m^3 * ~ 1000 J/kgK * dT dT = 15.9 K Mesh had an initial refinement of level 3, but partial cells were further refined by 1 level. Gravity was turned on (a(y) = 9.81 m/s^2). Radiation was turned on, and the rectangular block was assumed to be a blackbody. The goals that were set were GG Average temperature and VG (of the rectangle block) Max Temperature. 

January 23, 2014, 05:33 

#2 
Senior Member
Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,160
Rep Power: 19 
What you are estimating is the temperature difference of the fluid if all of the fluid crossing the domain would take the same amount of heat.
It clearly does not, the fluid further away from the centerline does not take any heat. Then still, the solid temperature would have to be higher than this estimation because there has to be a temperature gradient to transfer the heat. Those 900K seem quite realistic to me. To be sure you should compare the energy flux at the interface between solid and fluid to the heat source. They should be equal. 

January 24, 2014, 00:12 

#3 
New Member
Jason
Join Date: Jan 2014
Posts: 5
Rep Power: 4 
Thank you Alex, I see where I went wrong with my physics. I checked the energy flux at the solid/fluid interface, and I got a surface generation of 3.9 W ignoring radiation and 2 W when I included radiation. The model defined the solid to have a volume heat generation of 5 W. Can I consider this as equal?
Also, what happens if the solid I am using says it is melting (because the melting point is below 900 K)? Does that mean there is heat being conducted away in the real system that I am not accounting for in such a simplified model? 

January 24, 2014, 04:14 

#4  
Senior Member
Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,160
Rep Power: 19 
Quote:
But since the heat fluxes dont match the heat generation rate anyway, we cant consider this solution converged. It would be best to monitor the temperature of the body along with the heat fluxes at the interfaces during the simulation. Based on these graphs, you can see better when the solution is converged. We should leave the rest of the discussion until we gain confidence in the simulation result. 

January 25, 2014, 00:35 

#5 
New Member
Jason
Join Date: Jan 2014
Posts: 5
Rep Power: 4 
I tightened the convergence criteria of the heat transfer rate from Auto (1 W!! Silly me) to 0.1 W. Ignoring radiation, I get the expected value of 5 W at the solid/fluid interface. Including radiation, I get a heat transfer rate of 2.6 W at the solid/fluid interface. I guess I am missing something fundamental in the radiation model? Thank you for your patience Alex


January 26, 2014, 05:52 

#6  
Senior Member
Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,160
Rep Power: 19 
Help me out a bit since I dont know the program you are using.
Quote:
Quote:
Additionally, we need to know which kinds of heat fluxes the software postprocesses. Specifically, If we can tell apart the conductive and the radiative heat flux at the interface. 

January 27, 2014, 20:39 

#7  
New Member
Jason
Join Date: Jan 2014
Posts: 5
Rep Power: 4 
Quote:


January 28, 2014, 04:17 

#8 
Senior Member
Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,160
Rep Power: 19 
In this case it all makes sense, although there has to be a way to postprocess the radiative heat flux aswell.
In the simulation without radiation, the convective heat flux of around 5W at the interface equals the heat generation rate. That is what we wanted. In the simulation with radiation, the convective heat flux is only 2.6 W, so the difference between this and the heat generation rate has to be the radiative heat flux if the simulation is converged. The temperature of the solid body should be lower in this simulation. You could check if the radiative heat flux is in the range of the analytic formula 

January 29, 2014, 20:31 

#9  
New Member
Jason
Join Date: Jan 2014
Posts: 5
Rep Power: 4 
Quote:


March 5, 2014, 08:43 

#10 
Senior Member
Boris Marovic
Join Date: Jul 2009
Posts: 443
Rep Power: 13 
Hi Jason,
The surface parameter can give you clear answer in the post processing if you haven't defined a surface goal for the "heat transfer rate" (convection) and the "net radiation rate" (emitted radiation). So you should see 2.4W radiation and 2.6W convection. The results are plausible if you consider the size of the body and a similar body would be a light bulb with 6 W that reaches even higher temperatures but under natural convection and typically just a thin wire. 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Multiphase simulation of bubble rising  Niru  CFX  5  November 25, 2014 14:57 
ansys cfx solver exit with return code 1!!!!!  mhabibnia  CFX  7  August 19, 2013 03:53 
Best meshfree fluid model?  muffinman123  Main CFD Forum  0  June 27, 2012 05:37 
Reaching too high Temperatures using turbulentHeatFluxTemperature BC  Wokl  OpenFOAM Running, Solving & CFD  0  March 28, 2012 09:19 
Combustion model  Fluid Material  geothokar  CFX  60  August 11, 2009 07:31 