# negative net heat transfer rate

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

 July 10, 2013, 00:35 negative net heat transfer rate #1 Member   Join Date: Mar 2013 Posts: 57 Rep Power: 4 hi I am simulating heat transfer if flow through two concentric cylinders, with the inner cylinder rotating with specified wall temperature and outer cylinder stationary with zero heat flux (adiabatic). I used 2d axisymmetric with swirl, pressure inlet and pressure outlet in Fluent. Sum of mass flow rate at inlet pressure and outlet pressure gives me very small values, which I think I can conclude that mass conservation is met. However, when I sum the total heat transfer rate of pressure inlet, pressure outlet, inner cylinder wall and outer cylinder wall, I got a large negative value which mean energy conservation is not met according to some literatures. May I know what might be the cause of energy imbalance? and how can I overcome this problem?

 July 10, 2013, 09:02 #2 Senior Member   François Grégoire Join Date: Jan 2010 Location: Laval University, Canada Posts: 366 Rep Power: 8 Hi, In your case, the energy balance of the whole domain is between the inlet and outlet. The remaining boundary, the outer cylinder wall, is adiabatic. The inner cylinder wall is not a boundary of your domain.

 July 10, 2013, 09:32 #3 Member   Join Date: Mar 2013 Posts: 57 Rep Power: 4 Hi Thank you for quick response. I do not understand why the energy balance of the whole balance is only the pressure inlet and pressure outlet boundaries. I checked the total heat transfer rate of the rotating inner cylinder wall in fluent and it gives me negative value. I guess this indicates that there is a heat transfer out from the fluid domain across the rotating inner cylinder wall due to temperature difference between the fluid and the specified wall temperature. Please kindly advise what's wrong with my thinking. Also, I wonder whether there will be heat generated due to friction between the rotating inner cylinder wall and fluid (something like disc friction). If yes, how can I check how much heat is generated by friction? Please advice as well. Lastly, FLUENT manual says that we have to use axis boundary for the rotational axis for 2d axisymmetric with swirl. Fluent has a tutorial on this. The rotational axis is part of the domain. For two concentric cylinders with inner cylinder rotates, the domain is above the rotational axis and therefore there is no way to set axis boundary. I doubt whether my application of 2d axisymmetric with swirl is correct or not. I it is incorrect, does it mean defining the problem with 3D periodic model is the only way? Please kindly advise as well. Thank you in advance.

July 10, 2013, 10:02
#4
Senior Member

François Grégoire
Join Date: Jan 2010
Posts: 366
Rep Power: 8
Quote:
 Originally Posted by newbie384 I do not understand why the energy balance of the whole balance is only the pressure inlet and pressure outlet boundaries.
When you verify overall energy conservation, you look at what enters and what exits your whole domain, and in your case, the energy inlets/outlets are strictly the pressure inlet/outlet. As simple as that.

Quote:
 Originally Posted by newbie384 I checked the total heat transfer rate of the rotating inner cylinder wall in fluent and it gives me negative value. I guess this indicates that there is a heat transfer out from the fluid domain across the rotating inner cylinder wall due to temperature difference between the fluid and the specified wall temperature. Please kindly advise what's wrong with my thinking.
Your right, nothing wrong with your thinking. But this heat flux is not part of your overall energy balance, it's just an internal heat flux between two locations inside your domain. Will you also account for all the heat fluxes between each and every cells of your domain? No, you just check the energy fluxes at the external boundaries in order to verify energy balance.

Quote:
 Originally Posted by newbie384 Also, I wonder whether there will be heat generated due to friction between the rotating inner cylinder wall and fluid (something like disc friction). If yes, how can I check how much heat is generated by friction? Please advice as well.
I'm not familiar with that, can't help, sorry.

 July 11, 2013, 03:49 #5 Member   Join Date: Mar 2013 Posts: 57 Rep Power: 4 Hi Thank you for clarification. My net total heat transfer rate at pressure inlet and pressure outlet is a positive value and it is not near to zero at all. What does this mean? Does it mean I have a net energy gain in the fluid domain? May be I am confusing with the method to check energy balance. Is looking at net total heat transfer (like net mass flow rate) is the correct method?

 July 11, 2013, 04:12 #6 Senior Member   Join Date: Aug 2011 Posts: 315 Rep Power: 11 The enthalpy of the flow changes between inlet and outlet.

July 11, 2013, 07:39
#7
Senior Member

François Grégoire
Join Date: Jan 2010
Posts: 366
Rep Power: 8
Quote:
 Originally Posted by newbie384 My net total heat transfer rate at pressure inlet and pressure outlet is a positive value and it is not near to zero at all. What does this mean? Does it mean I have a net energy gain in the fluid domain? May be I am confusing with the method to check energy balance. Is looking at net total heat transfer (like net mass flow rate) is the correct method?
If the net total heat transfer rate between (thtr) inlet and outlet is positive, then the fluid is loosing energy. That's consistent with the negative thtr at the inner cylinder wall you mentioned in post #3.

Because the fluid is being cooled (or heated) between inlet and outlet, the energy balance of your problem should go like this: thtr inlet + thtr inner cylinder wall + thtr outlet ~ 0

If it's not the case, maybe you should lower the residual absolute criteria of the energy equation to, say, 1e-9 (Solutions\Monitors\Edit...), and see if the thtr balance improves.

Maybe you should play with a simple model of a 2D pipe flow with constant T at the wall, or constant q" at the wall, play with the thtr balance, etc., in order to understand what's going on in the flux reports.

 April 1, 2014, 00:39 Help in interpreting this flux report #8 New Member   Ankur Join Date: Jan 2013 Location: Austin, USA Posts: 26 Rep Power: 4 Hi Francois, Can you help me interpret the total heat transfer flux data described below. Model: There are various tubes that runs through a Furnace in which combustion occurs. A different reaction (methane -- > Hydrogen) takes place inside the tube which uses the heat released by combustion in the furnace. To see if my solution is converged, I checked the heat balance for every tube. Every tube has an inlet, an outlet and a side cylindrical wall. Total heat transfer Flux report for individual tube: inlet -474060 W outlet 338332 W side wall 135725 W Total --- ~0 Since the heat is supposed to flow inside the tube from outside (i.e. furnace) so a positive flux of 135725 W makes sense. But I don't understand how can outlet heat content be smaller (in magnitude) than that of inlet heat content. Energy balances says, Enthalpy of inlet + Heat absorbed/received = Enthalpy of Outlet. Since temperature of both inlet (800 K) and outlet (1050 K) is greater than the reference temperature (~298 K), enthalpy is positive for both inlet and outlet. So the data should have been something like this -(inlet) + heat flux through side = outlet ; since inlet is negative and outlet is positive by Fluent sign convention. Please help if you can suggest anything. Thanks, Ankur

 April 1, 2014, 18:08 #9 Senior Member   François Grégoire Join Date: Jan 2010 Location: Laval University, Canada Posts: 366 Rep Power: 8 Hi Ankur, The sign convention is the opposite: heat flux into the domain is positive and heat flux out of the domain is negative. Maybe radiation in the tubes shuffles the total heat transfer rates? Run the model without radiation and see if you get normal results with positive total heat transfer rate at the inlet and the tube wall, and negative at the outlet.

 April 1, 2014, 22:35 follow-up #10 New Member   Ankur Join Date: Jan 2013 Location: Austin, USA Posts: 26 Rep Power: 4 Hi Francois, Thanks for the reply. I will run a model without radiation and see if it clarifies anything.

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Anna Tian Main CFD Forum 0 January 25, 2013 19:53 Attesz CFX 7 January 5, 2013 04:32 Archangel2424 STAR-CCM+ 1 May 27, 2010 17:19 Sigrid Andreae CFX 1 February 26, 2005 08:13 Mark CFX 6 November 15, 2004 16:55

All times are GMT -4. The time now is 23:21.