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

How to achieve a constant water level in a transient simulation?

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

Like Tree2Likes
  • 1 Post By ghorrocks
  • 1 Post By ghorrocks

Reply
 
LinkBack Thread Tools Display Modes
Old   July 14, 2014, 05:01
Default How to achieve a constant water level in a transient simulation?
  #1
New Member
 
Join Date: Jul 2014
Location: BW, Germany
Posts: 9
Rep Power: 4
armlic is on a distinguished road
Hello everyone,

Im trying to complete the parameters for a Multiphase Transient Flow simulation in a turbine.

Until now, everything seems to go fine except for one condition: I don’t know how to establish a CONSTANT water level in time downstream the rotor. As Initial conditions I configured the volume of fraction as:

WaterVF: if(y<Waterlevel,1,0)
Waterlevel:-200 mm
AirVF: 1-WaterVF

(Rotor=rotary domain, Rest=stationary domain)

But as time passes by, the water level decreases until I loose it completely. This is expected, since y have a downstream OUTLET (average static pressure -20kpa ) but how can I solve it?


I annexed 2 printscreens: t=0 and some seconds after


Thank you all in advance.
Attached Images
File Type: jpg volumefractioninitial.jpg (28.1 KB, 10 views)
File Type: jpg volumefraction.jpg (30.9 KB, 10 views)
armlic is offline   Reply With Quote

Old   July 14, 2014, 06:02
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,832
Rep Power: 100
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Isn't this simply saying that your exit pressure is too low? -20kPa sounds like a vacuum to me so no wonder it sucks

Work out what the pressure should be at your exit.
armlic likes this.
ghorrocks is offline   Reply With Quote

Old   July 15, 2014, 09:18
Default
  #3
New Member
 
Join Date: Jul 2014
Location: BW, Germany
Posts: 9
Rep Power: 4
armlic is on a distinguished road
Hello ghorrocks,

True. I realized that specific input data was improper so I changed the boundary to Mass Flow (equal to the inflow). Also, I think a proper counter pressure just enough to handle that water column might work fine.

Thank you for your advice.
AL
armlic is offline   Reply With Quote

Old   July 15, 2014, 18:42
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,832
Rep Power: 100
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
A mass flow inlet and mass flow outlet will not work either. First of all it is numerically ill-defined as the pressure level is not set. And secondly, as a numerical solution is approximate then the inlet flow will not EXACTLY match the outlet flow then you will get a small flow imbalance and this will slowly either fill or empty the domain.

You need to apply a pressure at the outlet equal to the static head of the water column height you want. You are going to have to correct it for the reference density static head as well - have a look at the flow over a bump tutorial for an idea of how to do this.
armlic likes this.
ghorrocks is offline   Reply With Quote

Old   July 17, 2014, 04:46
Talking
  #5
New Member
 
Join Date: Jul 2014
Location: BW, Germany
Posts: 9
Rep Power: 4
armlic is on a distinguished road
Hello, ghorrocks

Now I configured an Outlet with Pressure equal to the water table, I still need to correct it, but so far is looking very good.
Thank you for the advice!
armlic is offline   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
Adding layers goes wrong with SnappyHexMesh Elise OpenFOAM Native Meshers: snappyHexMesh and Others 1 April 22, 2013 02:32
Boundary Conditions - Transient Simulation miki256 CFX 2 May 18, 2012 01:22
Time step in transient simulation shib FLUENT 0 June 17, 2010 13:07
Terrible Mistake In Fluid Dynamics History Abhi Main CFD Forum 12 July 8, 2002 09:11
uptodate water distribution network fredius,magige,tanzanian,(e.a) Main CFD Forum 0 January 27, 2002 08:10


All times are GMT -4. The time now is 10:37.