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

Simulating the pressure loss of a valve

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

Reply
 
LinkBack Thread Tools Display Modes
Old   July 1, 2008, 08:18
Default Simulating the pressure loss of a valve
  #1
Hartmchr
Guest
 
Posts: n/a
Hi I am a new cfx-user and want to simulate the pressure loss of a valve. Maybe someone can help me improving my model...

I just created the mesh in ICEM and imported it to cfx-pre. For the calculation i chose the following boundaries:

Inlet: Mass flow=12kg/s

Opening (as outet): static pressure (entrain)=159 bar

Wall: smooth wall

I didnīt set any other parameters! My problem is now that the results of the calculation (pressure loss) are too low. So maybe someone can give me some hints to improve the result...

I would appreciate any help or tip

Greets Chris
  Reply With Quote

Old   July 1, 2008, 12:06
Default Re: Simulating the pressure loss of a valve
  #2
JT
Guest
 
Posts: n/a
are you sure that's 159 bar?
  Reply With Quote

Old   July 2, 2008, 01:57
Default Re: Simulating the pressure loss of a valve
  #3
Hartmchr
Guest
 
Posts: n/a
Yes, its water at 159 bar and 290°C
  Reply With Quote

Old   July 2, 2008, 07:34
Default Re: Simulating the pressure loss of a valve
  #4
pratik mehta
Guest
 
Posts: n/a
Why have you kept wall- smooth and I hope your wall has a no slip wall condition on it ? .
  Reply With Quote

Old   July 2, 2008, 07:44
Default Re: Simulating the pressure loss of a valve
  #5
Hartmchr
Guest
 
Posts: n/a
I have a no slip condition on my wall. Which parameters should i use for a rough wall when i want to simulate teh flow through a valve. (Housing and pipe consisting of steel)
  Reply With Quote

Old   July 2, 2008, 18:15
Default Re: Simulating the pressure loss of a valve
  #6
Glenn Horrocks
Guest
 
Posts: n/a
Hi,

Assuming you have the physics correct the mistake made by almost every new user is to use too coarse a mesh. You need to do a mesh refinement study to determine how fine a mesh is required to capture the flow.

Do this by increasing the mesh density (say reduce all element edge lengths by 25%) and compare. If the pressure loss changes significantly then your mesh is not fine enough and you need to keep refining the mesh until the pressure loss levels out.

Glenn Horrocks
  Reply With Quote

Old   July 3, 2008, 02:27
Default Re: Simulating the pressure loss of a valve
  #7
pratik mehta
Guest
 
Posts: n/a
Yes , I agreee with Glenn on mesh density near the wall. You must improve your mesh if its too coarse .

To check your mesh is good ,kindly plot your Yplus at the walls. It should be ideally less than 1 mm, but betweeb 1 to 5 mmm its still ok. If your mesh gives you this results of yplus ,its good cfd results

ALso check what is your required boundary conditions at the outlet. Whats your inlet, velocity or mass flow or something else you have inserted ?

anyways best of luck for your simulation.

  Reply With Quote

Old   July 3, 2008, 04:02
Default Re: Simulating the pressure loss of a valve
  #8
Hartmchr
Guest
 
Posts: n/a
Thanks for yor help, i really appreciate it!

But isnt yplus a dimensionless parameter and should be ideally between 20-200? Or what do you mean by: it should be 1mm?

So if i plot yplus-results and have a maximum value of 2500 it means i have to refine the mesh there, is that right??
  Reply With Quote

Old   July 3, 2008, 18:14
Default Re: Simulating the pressure loss of a valve
  #9
Glenn Horrocks
Guest
 
Posts: n/a
Hi,

y+ is dimensionless. Pratik incorrectly gave it units of mm.

The y+ you need depends on the turbulence model you are using. If standard wall functions are OK then y+ between 20 and 200 should be OK. If you are integrating to the wall you need y+ about 1. If y+ is in the intermediate range of 1 to 20 the only wall function approach which works is the automatic wall function approach.

Glenn Horrocks
  Reply With Quote

Old   July 4, 2008, 02:18
Default Re: Simulating the pressure loss of a valve
  #10
pratik mehta
Guest
 
Posts: n/a
ya, sorry I meant the mesh parameterto be like 1 mm near the wall .
  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
"Pressure Inlet" Boundary Setup Wijaya FLUENT 13 April 11, 2013 08:50
How to get the pressure and pressure loss in fluent while using periodic winnawinna FLUENT 1 May 6, 2011 03:44
Does star cd takes reference pressure? monica CD-adapco 1 April 19, 2007 11:26
Pressure drop in a valve system with recirculation sacha CFX 2 March 11, 2005 06:56
Hydrostatic pressure in 2-phase flow modeling (long) DS & HB Main CFD Forum 0 January 8, 2000 16:00


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