
[Sponsors] 
August 24, 2017, 22:08 
Temperature dependant heat flux BC

#1 
New Member
VRam
Join Date: Aug 2017
Posts: 3
Rep Power: 8 
I am carrying out HVAC flow and thermal analysis in a box like region and my domain is the interior of the box  domain boundaries are the inner walls of the box. The input that i have is the outer wall temperature of the box. I tried giving a heat flux boundary condition at the wall using the expression
(Thermal conductivity of wall)*(Outerwall temp  Temperature)/(wall thickness) Temperature  CEL Variable. temperature computed by the solver at the wall, the other terms are fixed values The solution diverges very rapidly. I get either a "overflow" error or "density out of bounds" error Is there something fundamentally wrong about such a boundary condition? If not is are there some tweaks to acheive convergence with such boundary conditions? 

August 24, 2017, 23:45 

#2 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,771
Rep Power: 143 
Not, there is nothing fundamentally wrong with this approach. In fact I have used it many times myself so similar approaches have worked for me.
But you are changing the numerical stability of the system, so you may need double precision numeric, tighter convergence tolerance or smaller time steps to converge. Of course this assumes you have the maths correct  if your maths is wrong and you have not applied the boundary correctly then it will never converge. 

August 25, 2017, 00:21 

#3 
Senior Member
Join Date: Jun 2009
Posts: 1,831
Rep Power: 33 
Whenever you use a nonlinear boundary condition, i.e. q_outer_wall =
f(T_inner_wall), you must linearize respect to the solution variable. Keep in mind the solution variable for ANSYS CFX is enthalpy, h. Then, here it goes q_outer_wall = K * (T_outer  T) / Thickness d q_outer_wall/dh =  K / Thickness * dT/dh = K /Thickness * (1/Cp_fluid) Question: how do we introduce the linearization coefficient in the setup? Answer: add an Energy boundary source on the boundary, set the Flux strength to 0, and the Flux Coefficient =  K / (Cp_fluid * Thickness) You should be able to converge monotonically w/o any issues. Hope you understand that using q = K * (T_outer  T ) / Thickness you are making the assumption the heat flow is 1dimensional normal to the wall. Such approximation is a function of the thermal conductivity ratio between the fluid and the solid and aspect ratio of the wall. Hope the above helps, 

August 25, 2017, 02:31 

#4  
New Member
VRam
Join Date: Aug 2017
Posts: 3
Rep Power: 8 
Quote:
I do think that I have the rest of the maths correct because the solution runs when I give a fixed heat flux as the BC at the wall. The maths at this particular location is whatever I had described. 

August 25, 2017, 02:46 

#5  
New Member
VRam
Join Date: Aug 2017
Posts: 3
Rep Power: 8 
Quote:
Thanks Opaque. I'll try this out. I still have one question. Where does the outer wall temperature figure in such a setup. What would the thermal boundary condition at the wall be? I am also not sure that I fully understood the linear Vs nonlinear BC. Assume that instead of heat flux BC, I gave a temperature BC at the same wall as Outer Wall Temp  Wall Heat Flux*thickness/k Would it work as T here is a linear function of a solution variable? 

August 25, 2017, 02:55 

#6 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,771
Rep Power: 143 
The approaches I described will only work if the effect is small so it is numerically stable regardless. Opaque's answer is more general  as he is talking about how the condition you are adding is linearised for the solver. So it is not the linear/nonlinear nature of the BC he is talking about, it is whether the solver has linearised your boundary correctly so it will converge robustly.
Rewriting the equation to give temperature rather than heat flux will not help. The linearisation of the solver is unchanged. 

August 25, 2017, 12:24 

#7 
Senior Member
Join Date: Jun 2009
Posts: 1,831
Rep Power: 33 
I may have misunderstood the question a bit.
You can also use the Heat Transfer Coefficient option since Q_wall = K/Thickness * (T_outer  T_inner) Just provide Outside Temperature = T_outer Heat Transfer Coefficient = K / Thickness The software should take care of the rest. 

August 26, 2017, 21:37 

#8 
New Member
haidermumtaz
Join Date: Mar 2017
Location: najaf
Posts: 5
Rep Power: 9 
thank for all
how can i input heat flux for persons and lights ....to cfx ansys 

August 27, 2017, 05:39 

#9 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,771
Rep Power: 143 
If this is for a HVAC simulation and the only thing which is important is the heat load then you can add these as source points.


Tags 
boundary condition., convergence issues 
Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
[openSmoke] libOpenSMOKE  Tobi  OpenFOAM Community Contributions  562  January 25, 2023 09:21 
Ansys CFX problem: unexpected very high temperatures in premix laminar combustion  faizan_habib7  CFX  4  February 1, 2016 17:00 
Temperature and heat flux wall boundary condition  L. Hamid  Main CFD Forum  3  February 22, 2014 21:10 
Heat flux and wall temperature divergence  Mat_fr  FLUENT  2  March 6, 2013 08:58 
Concentric tube heat exchanger (AirWater)  Young  CFX  5  October 6, 2008 23:17 