Temperature dependant heat flux BC

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

 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 non-linear 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 1-dimensional 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, Lance likes this.

August 25, 2017, 02:31
#4
New Member

VRam
Join Date: Aug 2017
Posts: 3
Rep Power: 8
Quote:
 Originally Posted by ghorrocks 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.
Thanks Glenn. I'll try the double precision and see if it works. This is a steady state problem - Do you think using a lower timescale would help?

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:
 Originally Posted by Opaque Whenever you use a non-linear 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 1-dimensional 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,

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 non-linear 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/non-linear 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. haideralshami likes this.

 Tags boundary condition., convergence issues