CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > CFX

Temperature dependant heat flux BC

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

Like Tree2Likes
  • 1 Post By Opaque
  • 1 Post By ghorrocks

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   August 24, 2017, 22:08
Default Temperature dependant heat flux BC
  #1
New Member
 
VRam
Join Date: Aug 2017
Posts: 3
Rep Power: 8
VRam is on a distinguished road
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?
VRam is offline   Reply With Quote

Old   August 24, 2017, 23:45
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,771
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
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.
ghorrocks is offline   Reply With Quote

Old   August 25, 2017, 00:21
Default
  #3
Senior Member
 
Join Date: Jun 2009
Posts: 1,831
Rep Power: 33
Opaque will become famous soon enough
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.
Opaque is offline   Reply With Quote

Old   August 25, 2017, 02:31
Default
  #4
New Member
 
VRam
Join Date: Aug 2017
Posts: 3
Rep Power: 8
VRam is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
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.
VRam is offline   Reply With Quote

Old   August 25, 2017, 02:46
Default
  #5
New Member
 
VRam
Join Date: Aug 2017
Posts: 3
Rep Power: 8
VRam is on a distinguished road
Quote:
Originally Posted by Opaque View Post
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?
VRam is offline   Reply With Quote

Old   August 25, 2017, 02:55
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,771
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
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.
ghorrocks is offline   Reply With Quote

Old   August 25, 2017, 12:24
Default
  #7
Senior Member
 
Join Date: Jun 2009
Posts: 1,831
Rep Power: 33
Opaque will become famous soon enough
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.
Opaque is offline   Reply With Quote

Old   August 26, 2017, 21:37
Default
  #8
New Member
 
haidermumtaz
Join Date: Mar 2017
Location: najaf
Posts: 5
Rep Power: 9
haideralshami is on a distinguished road
thank for all
how can i input heat flux for persons and lights ....to cfx ansys
haideralshami is offline   Reply With Quote

Old   August 27, 2017, 05:39
Default
  #9
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,771
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
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.
ghorrocks is offline   Reply With Quote

Reply

Tags
boundary condition., convergence issues

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

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 Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


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 (Air-Water) Young CFX 5 October 6, 2008 23:17


All times are GMT -4. The time now is 23:45.