Hello, I have a problem with a long pipe (5m length and 12mm diameter) and 1m/s at inlet.

The study is realized in 2D axisymetric (a single rectangle) but Fluent don't converge, even if mesh is refined a lot (boundary layer is set, velocity profile is good, etc..). Fluent don't stop to "play yoyo" with residuals. Turbulence model is K-Epsilon and solver 2D axi all at order 2.

What 's the matter with the geometry/fluent? Are cells too far from inlet and too much numerical dissipation??

Thx

Which are oscillating residuals?

Hi

All residuals

Have a look to the screenshot : http://membres.lycos.fr/roscool/foru...fluenttube.gif

In that SS there are several refinements (BL and gradient), model change but always oscillations

I tried to simulate your pipe using water with axi solver and setting Momentum under-relaxation factor to 0.5 (all others are the standard value). Boundary conditions are velocity-inlet and outflow. I set turbulence bc at the inlet using 10% intensity and 0.012m as hydraulic diameter. I used all second order discretizations and SIMPLE as coupling method. The solution converged in about 120 iterations and residuals don't oscillates. I obtained a max velocity in the middle of the pipe (2.5 m) around 1.2 m/s.

What fluid are you using and what's your grid density?

Hi

I used water as fluid and 5% turbu at inlet (rest is same). Grid density is 6 cells B.L thickness and the rest is 1mm grid (center).

I'll try to decrease momentum relax to see difference. In this moment I try the Enhanced wall function for the refined BL and it seems to work better but Y velocity residual is always do yoyo

I'll try your setup in 2 minutes Thx for answering.

OK now it works, it was momentum relaxation a little too high to have CV. I changed all others parameters except this one LOL. It's a so current problem that I ask myself why I don't change that..

It's great now, thx a lot ap

You are welcome.

Good work

I forgot to say that if you use Enhanced wall function, you need y+ close to 1.

Hi again

Yep. Another question, my tube is now a copper tube with a 1mm wall all around water (classical copper tube) always using axisymetry (2 rectangles with a shadow edge for contact between water and copper).

I want to know how big are the power loss by natural convection with a difference between water at inlet and room temperature of 10°C or more (it's a variable). There is conduction in wall tube and natural CV with air of environnement but water temperature change all the time with the increasing distance to inlet because of power loss. For the moment I have put h=5W/m².K (typical value of natural convection I found) on the external wall of copper tube but h change all the time too.

So how to say Fluent to calculate itself h without modelize a room around the tube? Do you know that ap ??

I was thinking to implement it through a User Defined Function, but...I checked in FLUENT 6.0, and it doesn't allow you to select a user defined h. I don't know if you can in FLUENT 6.1. (Check the wall BC panel to see if you see User-defined in the drop down list near the value of h).

However, a good average value may be enough.

Hi

Oki I'll try 3 values of h to have a range and an idea of what I want.

Thx again for your answers