CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > FLUENT

CV problem with a long pipe..

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   May 6, 2003, 08:10
Default CV problem with a long pipe..
  #1
rosco
Guest
 
Posts: n/a
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
  Reply With Quote

Old   May 6, 2003, 08:58
Default Re: CV problem with a long pipe..
  #2
ap
Guest
 
Posts: n/a
Which are oscillating residuals?

Hi
  Reply With Quote

Old   May 6, 2003, 09:06
Default Re: CV problem with a long pipe..
  #3
rosco
Guest
 
Posts: n/a
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
  Reply With Quote

Old   May 6, 2003, 09:45
Default Re: CV problem with a long pipe..
  #4
ap
Guest
 
Posts: n/a
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
  Reply With Quote

Old   May 6, 2003, 09:55
Default Re: CV problem with a long pipe..
  #5
rosco
Guest
 
Posts: n/a
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.
  Reply With Quote

Old   May 6, 2003, 10:11
Default Re: CV problem with a long pipe..
  #6
rosco
Guest
 
Posts: n/a
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
  Reply With Quote

Old   May 6, 2003, 10:19
Default Re: CV problem with a long pipe..
  #7
ap
Guest
 
Posts: n/a
You are welcome.

Good work
  Reply With Quote

Old   May 6, 2003, 10:49
Default Re: CV problem with a long pipe..
  #8
ap
Guest
 
Posts: n/a
I forgot to say that if you use Enhanced wall function, you need y+ close to 1.

Hi again
  Reply With Quote

Old   May 6, 2003, 11:31
Default Re: CV problem with a long pipe..
  #9
rosco
Guest
 
Posts: n/a
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 10C 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/m.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 ??
  Reply With Quote

Old   May 6, 2003, 13:30
Default Re: CV problem with a long pipe..
  #10
ap
Guest
 
Posts: n/a
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
  Reply With Quote

Old   May 6, 2003, 13:48
Default Re: CV problem with a long pipe..
  #11
rosco
Guest
 
Posts: n/a
Oki I'll try 3 values of h to have a range and an idea of what I want.

Thx again for your answers
  Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
[DesignModeler] DesignModeler Pipe within pipe shields ANSYS Meshing & Geometry 8 March 7, 2011 12:24
convergence problem in a long pipe feizaghaee CFX 7 February 16, 2010 08:05
Problem with meshing long, thin faces in CFX Martin CFX 3 January 8, 2009 20:51
Pipe bend erosion problem John Yang FLUENT 2 December 12, 2007 04:06
Hydrostatic pressure in 2-phase flow modeling (long) DS & HB Main CFD Forum 0 January 8, 2000 15:00


All times are GMT -4. The time now is 12:13.