How the heat fluxes for inlets/outlets in Fluent are calculated

trimarantrimaran Member

Hello!

I am simulating in Fluent a heating system in a ventilated room. After achieving quite stable results I checked the heat fluxes through all BCs. All of them make sense to me and are predictable according to hand calculations. All of them except inlet and outlet for which I have no idea how the heat fluxes are calculated. I cannot find any detailed explanation in the manual, except that depending on the models different enthalpy is taken into account and that the reference temperature for all enthalpy calculation is 298.15K. Where can I find any more information about how it is calculated?

When multiplying mass flow rate by weighted-average values of specific heat and temperature difference (the inlet or outlet avg. air temp. minus the reference temp.) I got around the same heat flux for the outlet as calculated by the Fluent, but 3 times higher for the inlet then the one given by the Fluent.

Best regards

Jakub

Comments

  • KremellaKremella Admin
    edited May 12

    Hello,

    To estimate the total heat transfer rate at the inlet and outlet, please go to 'Surface Integrals', choose 'Flow Rate' for the 'Report Type', select 'Enthalpy' (in the Temperature category), and select your inlet and outlet surfaces over which you would like to integrate. 

    The total Q reported by Fluent crossing the inlet and outlet is the surface integral of 

    [enthalpy x density x velocity vector x dA]

    For additional details, please have a look at the following link (Fluent Users Guide: Section 14.2.3.4. Reporting Heat Transfer Through a Surface) - https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v201/en/flu_ug/flu_ug_sec_hxfer_report.html%23x1-110100014.4.1

    Specific enthalpy is calculated based on the temperature as well as the reference temperature. 

    For additional information, look at 'The Energy Equation' in the Fluent Theory guide (Section 5.2.1.1) using the following link: https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v201/en/flu_th/flu_th_sec_hxfer_theory.html

    I hope this helps.

    Best,

    Karthik

  • trimarantrimaran Member
    edited May 13

    Dear Karthik,

    thank you very much for your reply.

    After using the method you described with Surface Integrals and Flow Rate for inlet and outlet, the values are the same as calculated by hand and everything is as predicted.

    Unfortunately I still do not understand how it works for Total Heat Transfer Rate in Flux Reports. There the outcome for outlet is similar to the expected one, however inlet is much different. The second link you recommended gave me an idea that maybe turbulence properties are too high for the inlet and that some of the turbulent energy is hidden in this Flux Report. I checked the results for much lower as well as 0 turbulence kinetic energy and dissipation rate. The inlet heat flux hardly changed after this.

    The more converged my calculations are, the lower Net Result (for all BCs) of Total Heat Transfer Rate is. What worries me is that without understanding why the inlet heat flux is so much different than expected I can not be sure that the heat fluxes Net Results represent the real energy balance of the system.

    Is there any explanation available?

    Best regards

    Jakub

  • KremellaKremella Admin
    edited May 14

    Hello,

    Could you please post screen shots of your flux reports you are seeing? Also, what is your convergence? Also, what is your inlet boundary condition? Can you please provide some screenshots so we can infer these better?

    Thanks.

  • trimarantrimaran Member
    edited May 14

    Dear Karthik,

    here are the screen shots of flux reports, enthalpy flow rate, convergence (residuals + some of the points in the room monitored), inlet and outlet settings. The convergence now does not look perfect, because around 1k iterations before I changed inlet and outlet from velocity type to mass flow type (before outlet was a negative velocity inlet). Nevertheless, before these changes, when all the results were already quite stable, all of the heat fluxes were almost the same (inlet heat flux was around 5W less).

    On the screen shot with all BCs' heat fluxes you can see some external and internal walls of the room, surfaces of humans' models and some heaters (in this simulation only conventional heaters are turned on). All of these fluxes as reasonable according to hand calculations, except inlet and outlet.

    Outside_temp (for inlet thermal condition) is 273.15K. Average temperature for the whole domain is around 295.6K and for outlet is around 297.2K.

    Best regards

    Jakub

  • KremellaKremella Admin
    edited May 14

     Hello,

    When you have radiation included in your model, the total heat transfer flux reports both convective and radiative heat transfer. It is the sum of both. However, the flow rate of enthalpy will only predict the convective portions. If you were not solving the radiation model, these two values would match.

    Thanks.

  • trimarantrimaran Member
    edited May 15

    Dear Karthik,

    as you can see I included also radiation heat fluxes for inlet and outlet. For inlet it is around -2.8W, which means that inlet convective heat flux should be around: -530.6 - (-2.8) = 527.8W.

    If I am not right, what is the Radiation Heat Transfer Rate then?

    Black Body Temperature for inlet = internal_temp, which is set to 294.15K (the radiation heat flux from the inlet should be close to negligible then).

    Best regards

    Jakub

     

  • trimarantrimaran Member
    edited May 20

    So, if I understand right, the total heat transfer rate should be the sum of: total radiation transfer rate and enthalpy flow rate? What can be the reason for this to be very different? If this is not calculated as the sum of these two values, then how is it exactly calculated?

  • KremellaKremella Admin
    edited May 22

    Please converge your solution more deeply. Fluxes do not get computed properly if you do not have proper convergence. I'd first make sure you are converging deeply and your net heat flux reported by Fluent is less than 1% of the smallest flux you are seeing in those reports. Once you are able to achieve this, please try these hand calculations and see if these match up with your Fluent calculations.

    Otherwise, please try and use an existing and converged solution and check your hand calculations to understand what Fluent is doing. 

    Thanks. 

    Best,

    Karthik

Sign In or Register to comment.