Learning Forum

[Dio]

I run for different Desşred y+ values and get Nusselt and Heat transfer coeff.

for k-w SST, as I search online, desired y+<1, am I on the right way or should I try for different y+?

How can I check correct y+ on fluent solution

Also I am using facet average to get Nu and h, is that correct way to get these values or I should try different way?

I am following https://www.cfd-online.com/Tools/yplus.php

I am running periodic simulation.

Inlet mass flow rate: 0.0422509

D: 0.01m

Inlet temperature: 303.15K

density: 995.6

Dynamic viscosity: 0.000844 kg/ms

Cp: 4123 kj/kgK

Thermal conductivity: 0.636 W/mK

Constant heat flux at wall: 12752 W/m2

Any suggesttion?

[DrAmine]

What is your Prandtl Number?

[Dio]

it is Pr= 5.47
Calculated from this formula (2): https://www.engineeringtoolbox.com/prandtl-number-d_1068.html

[Dio]

it is Pr= 5.47
Calculated from this formula (2):https://www.engineeringtoolbox.com/prandtl-number-d_1068.html

[DrAmine]

Okay is not very large so I guess a good start is to have yplus around 1 if you want to resolve the viscous sublayer and properly model thermal effects.
It is however not only the yplus which is important the number of cells you put to resolve the boundary layer is equally important. I recommend to have at least 10-15 cells there (You can afford it for this simple case).
From that you can carry out a mesh sensitivity study and assess all numerical errors.

[Dio]

Thank you When I tried 10-15 layers, mesh quality is getting about 10e-3. When I try 20-50 layers, mesh quality increase above 0.15 and Nu and h results looks like in the table. for y+=5 Nu and h looks decreasing. I guess for k-w SST y+ below 1, Nu and h becomes very close to experimental results.

[Rob]

Remember y+ helps guide the near wall cell height, you still need enough mesh in the right place to resolve the flow and thermal boundary layers as well as the bulk flow.

[Dio]

Thank you I think I get some good results. Errors were between 2-6% compared to experimental results. But how can I get pressure loss? analysis was periodic so outlet is disappeared when I defined periodic.
10mm length and 10mm dia pipe, original length 1400 mm and 1200mm portion has constant heat flux 12752 W/m2

[Rob]

You set pressure drop to get mass flow, so if you compare the pressure drop you set with your data how close is the mass flow?

[Dio]

I have figure for pressure drop and I just want to see how close my simulation to experimental value and looking for d,d I simulate well or not. Around 10% error also ok for me. I am triyng for 0.025

[Dio]

I trid different mass flow and after calculation I realiezed that, in periodic condition, pressure gradient changeed 0 to -856.163 Pa/m
when I multiply this value with total pipe legth I get very close value with figure I shared. I believe this approach is correct ?
Can I see this value by using "Reports" ?

[Rob]

Periodics and reports are a bit messy as you have a pressure drop and "pressure" is relative as we have incompressible flow: have a look and see what you get. That's why the periodic panel is the way it is: you see the pressure loss per metre & mass flow.

[Dio]

Thank you it looks like it is better to write pressure drop formulation for turbulent flow as expression to see what I will get.

[DrAmine]

The Pressure loss will be that pressure gradient by the length of the pipe. So your approach is correct.