

April 10, 2018 at 6:27 pmhugo CFDSubscriber
Hello.
I have some doubts that i would like to clarify. Consider a fixed plate heat exchanger airair with quasi counter flow. The heat exchange is through forced convection.
How should I calculate the coefficient of heat transfer? Directly from the fluent across the surfaces integrals > area weighted average or through the formula h = q / at, where do I take the values of twall and tref and q from the fluent?
The next question is about boundary conditions. when defining the boundary conditions, is it necessary to consider heat transfer by convection between the air and the plate, by selecting the CONVECTION point in the THERMAL conditions?
Thanks

April 14, 2018 at 3:23 pmRaef.KobeissiSubscriber
Hello Hugo,
Question 2 first: It depends on how you're simulating your case, if it is forced convection I would assume air flow is involved around the fixed plate HE and in this case you don't need to use convection.
Question1: I am assuming that you are using a solid wall(meshed) to simulate the HE, in that case you can calculate it through fluent as you mentioned. Can you attach the case file and I can show you how to do it through a small video or series of pictures.
Regards

April 19, 2018 at 8:48 amhugo CFDSubscriber
Hello
I am sending the study case. I have read that in certain situations, a UDF is required to calculate h. Am i correct? What are these situations?
Regards

April 26, 2018 at 1:56 pmraul.raghavSubscriber
For laminar flow in Ansys Fluent, the convective heat transfer coefficient (h) is calculated based on the equation:
h = q / (T_wall  T_ref); where T_ref is the reference temperature you provide. You need to be careful providing the T_ref value, as that can result in the underestimation or overestimation of convective heat transfer coefficient (h) value. I'd highly recommend you to go through the following paper which compares the convective heat transfer coefficient obtained with T_ref value evaluated in different ways:
Determination of surface convective heat transfer coefficients by CFD
You can plot contours of the local heat transfer coefficients. And you can use "Surface integrals" to plot the average heat transfer coefficient (see image below):
PS: I haven't checked any of the inputs or outputs in your case file, so I won't be commenting on the results.

April 29, 2018 at 10:31 amRaef.KobeissiSubscriber
Hi Hugo, have you been able to resolve your issue?

May 3, 2018 at 11:26 amhugo CFDSubscriber
No. I am looking for another way to get heat transfer coefficient, instead to calculate by T ref method.
Hugo

May 3, 2018 at 1:53 pmraul.raghavSubscriber
Hugo, as far as I'm aware of, heat transfer coefficient can either be calculated using the standard definition as I mentioned my previous post or by the Reynolds Analogy as turbulent heat transfer is modeled using the analogy.
From the Reynolds analogy: h = (Cf/2) * density * U_ref * Cp
where Cf is the skin friction coefficient, and U_ref is the reference velocity, which is difficult to be estimated. For turbulent flows, you can use wall functions to evaluate h:

May 3, 2018 at 11:14 pmhugo CFDSubscriber
yes. you are right. maybe i didn´t express well.
i considered follow expression to calculte heat transfer coefficient: h = q / ( T _ wall  T _ adj)
q is heat flux and I get this value from fluent (surface integralswall flux total surface heat flux) referring to the boundary condition "heat transfer 1".
T_wall is a temperature of the wall and i get this value from fluent referring to the boundary condition ""heat transfer 1shadow".
T_adj is the temperature of the first fluid layer following the wall referring to the boundary condition "heat transfer 1".
My problem is how i get the values of the expression from fluent. I don t know if what i have considered is right.
Hugo

May 4, 2018 at 12:48 amraul.raghavSubscriber
You can define a custom field function with the formula shown in the image below [Total Surface Heat Flux / (Wall Temperature  Static Temperature)]. Once you've created the function, use a contour plot to display the function. Make sure when you create the contour plot, you have the "Node Values" unchecked.

May 4, 2018 at 4:59 pm

May 5, 2018 at 5:41 pmraul.raghavSubscriber
The heat transfer coefficient that is areaweighted average is the average heat transfer coefficient. The contour plot shows the local heat transfer coefficient. And the heat transfer coefficient depends on the fluid, hydrodynamic and thermal conditions and also on the geometry under consideration.
I'm not sure why the coefficient is negative though. Again as I mentioned in my earlier posts, the way you calculate the coefficient makes a whole lot of difference.

May 22, 2018 at 8:58 amhugo CFDSubscriber
Hi.
How can I obtain/calculate the local heat transfer coefficient along the length of the heat exchanger? And make a chart of this behavior?
hugo

May 22, 2018 at 2:55 pm

February 10, 2020 at 8:59 amatulsingh92Subscriber
@Raul.raghav Could you please explain in more detail, as to how, can one define this reference temperature? The thing is, this value, is good enough to make the nusselt number negative.
So, lets say I am simulating for internal flow in a corrugated tube with periodic bc. (yes i have segregated solver and const heat flux bc as mentioned in Ansys manual). The reference temperature I have chosen, is by reverse calculating the nusselt number mentioned in an experimental paper. i.e the paper mentiones the fluid water entering at 26 degrees C and then showed a nusselt of 65 for example. The q applied is 21100.
This would leave me by htc= 21100 / (26  x); Nu = 60 = htc * 0.00575 / 0.61; I enter this x as my reference temperature.
But the question is , here, I knew my nusselt from an experimental data, what to give when I dont know this before hand
Also, the way I mentioned, is it the correct way? 
July 7, 2022 at 2:06 pmirineupetriSubscriber
Hi.
Follow the advice from colleagues above, but don't forget to consider the outer walls of your adiabatic system, setting the heat flux equal to zero (Q = 0) on the external walls.
Good luck

 You must be logged in to reply to this topic.
Simulation World 2022
Check out more than 70 different sessions now available on demand. Get inspired as you hear from visionary companies, leading researchers and educators from around the globe on a variety of topics from lifesaving improvements in healthcare, to bold new realities of space travel. Take a leap of certainty and check out a session today here.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Ansys Blog
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.
 Suppress Fluent to open with GUI while performing in journal file
 Heat transfer coefficient
 What are the differences between CFX and Fluent?
 Floating point exception in Fluent
 Difference between Kepsilon and Komega Turbulence Model
 Time Step Size and Courant Number
 The solver failed with a nonzero exit code of : 2
 Meshing
 Exporting Data Results
 error in cfd post

1180

1175

535

422

204
© 2022 Copyright ANSYS, Inc. All rights reserved.