CFD Online Discussion Forums

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   FLUENT (https://www.cfd-online.com/Forums/fluent/)
-   -   Problem - Natural Convection (https://www.cfd-online.com/Forums/fluent/214273-problem-natural-convection.html)

MarcosLima January 25, 2019 10:54

Problem - Natural Convection
 
Hello guys!
I am facing a transient cooling problem:
The physics of the problem is as follows: a body of 320K organic material should be cooled by natural convection in air at 283K.
Experimentally the cooling of this solid body takes place in 5 hours.
I am performing simulations in FLUENT 19.2. but I can not get satisfactory results in relation to the time versus temperature plot.
I'm using 100 time steps with 180s in size.

Can anyone help me with this?

Jiricbeng January 25, 2019 11:08

Just a question: 1000 timesteps with 180s is 50 hours, not 5. Is it mistype or mistake?

LuckyTran January 25, 2019 11:17

Quote:

Originally Posted by MarcosLima (Post 722939)
I'm using 1000 time steps with 180s in size.

180s time-steps, what numerical Fourier and Biot number is this for the solid? And what Courant number for the flow? Your time-steps are probably way too big.

Put some solution monitors, probably your solution isn't converged at all at each time-step.

MarcosLima January 25, 2019 11:19

Sorry
 
Yes! i messed up
There are 100 time steps with 180s in size.:)

MarcosLima January 25, 2019 11:26

This is one of the problems!
I do not have data of heat flow, besides the geometry and properties of the material the data that I have are those described above. That is, I want to check if the body really cools at the given time.
The input data are only the temperature of the solid, the domain and the total time for cooling.

MarcosLima January 25, 2019 11:39

Quote:

Originally Posted by LuckyTran (Post 722942)
180s time-steps, what numerical Fourier and Biot number is this for the solid? And what Courant number for the flow? Your time-steps are probably way too big.

Put some solution monitors, probably your solution isn't converged at all at each time-step.


In the problem in question I only need to impose deltaT and estimate an appropriate time step, this is what I am not succeeding!

MarcosLima January 25, 2019 12:06

If in this case, when finding a time step with the ideal size and that it is very small, could I increase the number of steps so that it covers all the physical time imposed by the real problem? That is my fundamental question.

LuckyTran January 25, 2019 15:00

Yes. You cannot pick arbitrarily your time-step size. You only need a temporal resolution of 180s because you only want to see 100 temperature points in time for comparison. But you need to pick one small enough that makes numerical sense for the solver. Yes you can always just increase the number of time-steps to get the desired total time.


I'll give you a warning though. You might be surprised that you will need a very small time-step size and very large number of time-steps. The physics are not complex, but this is a computationally expensive problem because the heat diffusion happens at very small length and time scales.


Also I don't follow what your domain is. Is it only the solid with a convective boundary condition or a conjugate problem (solid and fluid domain)?

MarcosLima January 25, 2019 15:41

1 Attachment(s)
Exactly LuckyTran! The problem is not complex, the case studied is the conjugate (heat transfer between a solid and a fluid). Follow the figure below.https://www.cfd-online.com/Forums/at...1&d=1548445257

LuckyTran January 25, 2019 18:05

Okay, cool. So just check to make sure your solution is converged every time-step. And keep shrinking the time-step until it does.


A fast easy check is to get the Courant number (it's a field in Fluent). Your Courant number should be low (less than 10, ideally less than 0.5 everywhere). Choose a small enough time-step size so that you can get the Courant number around this low. If your Courant number is too big, you flow solution will not be accurate or stable. The Biot and Fourier number for the solid will be even smaller than this Courant number, but you do not have stability problems to worry about over there.


I anticipate this problem needing a very long calculation time. It might be cool to try it anyway.

If it takes too long, one thing you can do is do a steady problem with the full domain. This lets you get the heat transfer coefficients on the surface of the solid body. Then you can run another simulation with only the solid body with the convection BC being applied. Of course you will miss out on non-linearities due to problem coupling.

MarcosLima January 25, 2019 22:27

Thank you very much for the help! I had many doubts about this case! During all this time working on this few gave me tips as valuable as you!

Thank you!


All times are GMT -4. The time now is 08:03.