[CaptainCombo]

Hello,


y+~1 is offered for enhanced wall treatment, I wonder using very low y+ value (for example 0.2) would be a problem for accuracy?


Thanks in advance.

[flotus1]

The criterium is y+ up to ~1. So y+ values lower than 1 are usually not a problem for wall-resolving boundary layer treatment in turbulence models.
You just have to pay attention with very low wall distances or very high aspect ratio cells near the wall. These can result in problems with numerical accuracy, and some solvers (e.g. Fluent) offer special numerical formulations for these cases.

[CaptainCombo]

Originally Posted by flotus1

The criterium is y+ up to ~1. So y+ values lower than 1 are usually not a problem for wall-resolving boundary layer treatment in turbulence models.
You just have to pay attention with very low wall distances or very high aspect ratio cells near the wall. These can result in problems with numerical accuracy, and some solvers (e.g. Fluent) offer special numerical formulations for these cases.

What do you mean with very low wall distances, for what value of y+ wall distance is not too low? How can I determine the appropriate value?

[flotus1]

It has less to do with the value of y+ and more with the absolute wall distance. There is no clear threshold for either of them.
When you import a mesh in fluent with very small cells at the boundaries (compared to the domain size?) or very high aspect ratio cells, you will get a warning and a hint to the counter-measures.
Some solvers (e.g. CCM+) just have a limiter for the smallest -dimensional- wall distance.

[AshwaniAssam]

You can use y+=0.2. It would not be much of a problem. However, as mentioned just have to be careful at very low y+ and high aspect ratio cell.

Also, you should check your y+ during the solution evolution and in the final solution, as y+ is a post-processing parameter.

[CaptainCombo]

Reduced the number of elements along wall normal direction. This caused increase in y+ (still lower than 1) and aspect ratio is halved but my heat transfer results didn't changed. So neither aspect ratio nor y+ was my problem. I am still digging.

[flotus1]

https://en.wikipedia.org/wiki/XY_problem

[CaptainCombo]

Originally Posted by flotus1

https://en.wikipedia.org/wiki/XY_problem

Since the problem is very simple(turbulent flow and heat transfer in straight channel) I was thinking the mesh was my "X". Now I am searching for other possibilites for the resons of error before asking new question.

[CaptainCombo]

If I swtich near wall tratement from "enhanced wall tratemnet" to "scaleable wall function" without changing any other thing. I am getting true results. Can anyone give me a clue, what is the reason could be?

[flotus1]

Two or more errors cancelling each other out?

[CaptainCombo]

I tried litterally everything to get true result by using enhanced wall treatement but all my efforts didn't change anything.

- Tried 40 layer for inflation, in order to put enough number of elements to boundary layer.

- Used elements with the aspect ratio 1 and y+ was ~1.1, this cost me 6M elements such a simple problem but it didn't work.

- Investigated the effect of turbulence intensity at the inlet by changing it between 1-5%, I saw that turbulence intensity does not have big influence.

- Used enhanced wall treatement options for pressure gradient and thermal effects but they didn't cause any difference.

I had other attemps but it does not worth to mention here.

As a result my numerical simulation gives local Nu number near the end of the channel 30% higher than Gnielinski correlation. I checked that thermal and hydraulic boundary layers becomes fully developed before the end of the channel.

I shared case and data of one of my tries. Maby someone see something I don't see.

Case: https://drive.google.com/open?id=1ul...DSl8AUmZ2byfNe

Data:https://drive.google.com/open?id=1yA...28Vp02BLtqdRUv

[flotus1]

You are really not giving us much to work with here.
1) What exactly are you trying to simulate?
2) How exactly did you do it - describe in a few words, add images of computational domain and mesh. Not everybody has Ansys Fluent readily available and has the time to go through the setup. And some might even be reluctant to download files from unknown sources.

[CaptainCombo]

I am trying to calculate convective heat transfer from the walls of straight channel under turbulent flow condition (Re = 10000). I am using relizable k-e turbulence model. The channel is 1.5m long and the problem is assumed to be two dimensional. Constant heat flux is applied at walls, distance between upper and lower walls is 0.01m. Uniform velocity and temperature profile is defined at inlet however I checked thermal and hydraulic boundary layers reach fully developed state where I calculate Nusselt number. I am sure about my calculation method of Nusselt number because I solved similar problem for laminar flow condition; my numerical simulation gives almost same results with analytical methods.


Here are mesh and y+ for one of my attemps;

[flotus1]

I checked thermal and hydraulic boundary layers reach fully developed state where I calculate Nusselt number. I am sure about my calculation method of Nusselt number because I solved similar problem for laminar flow condition

The length to reach a fully developed flow increases with Reynolds number.
Is there any particular reason why you did not use periodic boundary conditions for this study? It would eliminate any chance of the flow not being fully developed, while also cutting down computational cost drastically.
A mapped mesh would also make it easier on the eye.

I am not too firm on which turbulence model is the right one for heat transfer, but IIRC k-omega SST is the default recommendation by Ansys.

[CaptainCombo]

In this (https://www.sciencedirect.com/scienc...09250995000354) paper they compared various low Re turbulence models. So, I ran simulations for turbulent pipe flow for the same Reynolds number as in the paper (Re = 7000). I applied the streamwise periodic boundary condition to be sure about flow development. In addition, I added the constant heat flux boundary condition to the same simulations in order to calculate Nu. Here is the velocity profile in the viscous sublayer;


post a picture


Since bulk temperature does not change for all turbulence models, I think I need to focus on the viscous sublayer, is that true? My simulation with using Lam & Bremhorst gives closest heat transfer predictions. Nu is only higher 1.96% than empirical calculation. However, Realizable k-e overestimates 17.91% and SST k-w intermittency model overestimates 24%.



@flotus1 What is IIRC, I assumed you mean intermitency transition SST k-w.

[flotus1]

Sorry for the confusion. IIRC means "if I recall correctly", a common abbreviation to save precious time when communicating on the interwebs. Didn't really work this time

Since bulk temperature does not change for all turbulence models, I think I need to focus on the viscous sublayer, is that true?

Sounds reasonable, but since your study is on heat transfer, the temperature profile should be more important than the velocity profile.

Heat transfer isn't really my strong suit, maybe someone else can chime in?

[Blanco]

Hi,


are you simulating a constant density flow? Because that can change significantly the problem in my experience.
In addition, are you using the friction factor calculated directly using the Moody's diagram, w/ a known pipe roughness?

[CaptainCombo]

Originally Posted by Blanco

Hi,


are you simulating a constant density flow? Because that can change significantly the problem in my experience.
In addition, are you using the friction factor calculated directly using the Moody's diagram, w/ a known pipe roughness?

Hello,


I am using pressure-based solver and constant fluid properties. I didn't specify surface roughness, Fluent uses smooth surface by default. After I saw your post I calculated friction factor (f) for low Reynolds number model of Lam & Bremhorst and SST k-omega just as it is happening in the heat transfer low-re-ke model of LB predicts friction factor better than SST k-w. I think the reason behind the wrong estimation of heat transfer also causing wrong surface friction.



By the way are you author of this paper; https://www.sciencedirect.com/scienc...90072910000803

[Blanco]

Ok, in addition there's also the turbulent Prandtl number. It's typically set at 0.9 which is "reasonable" for air (and maybe water if I remember correctly, or at least it seems reasonable for most flows of these two fluids), but if you're simulating some exotic fluid I would expect different values. Unfortunately this as it is still a research area.



As far as the article is concerned, no I'm not in that pubblication, but you're guess on my name is still very close to reality

Originally Posted by CaptainCombo

Hello,


I am using pressure-based solver and constant fluid properties. I didn't specify surface roughness, Fluent uses smooth surface by default. After I saw your post I calculated friction factor (f) for low Reynolds number model of Lam & Bremhorst and SST k-omega just as it is happening in the heat transfer low-re-ke model of LB predicts friction factor better than SST k-w. I think the reason behind the wrong estimation of heat transfer also causing wrong surface friction.



By the way are you author of this paper; https://www.sciencedirect.com/scienc...90072910000803

[Andrea1984]

Just to add that not only the value of the turbulent Prandtl number is tricky to evaluate, but the assumption of a constant Pr_t is often a major simplification with little physical justification. Actually, the SGDH assumption for the turbulent heat flux is indeed a major simplification with no sound physical basis in most cases - we just use it because it's simple and robust and often it is the only option that we have in commercial codes

It's interesting to observe that the SGDH with Pr_t~1 breaks down even with non-exotic unity Prandtl number fluids in very basic flows in natural and mixed convection, such as Rayleigh-Benard convection and unstable stratified mixed convection in channels, as reported here: https://www.sciencedirect.com/scienc...29549319302407

One quick workaround to relax the constant Pr_t assumption in the SGDH context is to use a local correlation - see, for instance, section 3 here: https://core.ac.uk/download/pdf/82053898.pdf