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

Pressure drop specification

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

Reply
 
LinkBack Thread Tools Display Modes
Old   December 12, 2002, 12:46
Default Pressure drop specification
  #1
Swapnil
Guest
 
Posts: n/a
Hi all,

In my geometry, i have periodic bounday condition with inlet and outlet acting as periodic pair.Thus, i can't define any inlet or outlet B.C. on the inlets and outlets. I want to define pressure drop in the domain. How can i define the value of pressure drop ?

Thanks, swapnil.
  Reply With Quote

Old   December 12, 2002, 14:17
Default Re: Pressure drop specification
  #2
Holidays
Guest
 
Posts: n/a
Source terms, momentum sources or resistances will drive the flow. This issue to control them so as to balance the flow.
  Reply With Quote

Old   December 12, 2002, 21:09
Default Re: Pressure drop specification
  #3
Neale
Guest
 
Posts: n/a
Search the archives for this. The topic has come up many times before on how to do this in CFX-5.

Neale
  Reply With Quote

Old   December 15, 2002, 12:20
Default Re: Pressure drop specification
  #4
Swapnil
Guest
 
Posts: n/a
Hi Neale and holidays,

Thanks for the reply.

Yaa, i know that for defining a pressure drop you have to define a Momentum source term or resistance coefficient. But for that one needs a subdomain(i believe).

In my geometry there is no subdomain. How can i define a pressure drop in the absence of a subdomain?

For example (a simple one and analogus)if you have a pipe and you want to define the pressure drop in the pipe. The pipe is acting as your domain. There is no subdomain here.

In my geometry (triangular duct), i have periodic boundary condition at inlet and outlet. so i can't define any B.C. on these boundaries and that's why i am defining pressure drop.

Regards, Swapnil
  Reply With Quote

Old   December 15, 2002, 13:42
Default Re: Pressure drop specification
  #5
Sharks
Guest
 
Posts: n/a
Swapnil

There are two solutions to your problem in CFX-5:

1) You can create a subdomain which is the entire geometry of your domain (use the same geometric solids). This allows you to specify momentum sources in combination with inlet/outlet bcs as per Neale's suggestion.

2) Use inlet/outlet bcs and employ user fortran to make the variables of interest (velocity) periodic. One way of doing this is to write the variables at the "exit" to an external file, and then read these values in to specify the "inlet".

Hope this helps,

Sharks

  Reply With Quote

Old   December 15, 2002, 22:25
Default Re: Pressure drop specification
  #6
Swapnil
Guest
 
Posts: n/a
Hi sharks,

Thanks for the reply. When i contacted CFX Support for this problem, they suggested me the way out that you suggested as second possibility ( using user Fortran) They called it custom periodic boundary condition and they also sent me an example of the fortran routine. But they don't have the db file for this type of particular example(custom periodic B.C.). Do you have a db file for this type of example? Let me know. If any body else has worked on specifying periodicity through user subroutines let me know.

Thanks and regards,

Swapnil.
  Reply With Quote

Old   December 16, 2002, 08:06
Default Re: Pressure drop specification
  #7
Holidays
Guest
 
Posts: n/a
1) is easy to test (this is what I meant in my previous post by the way.
  Reply With Quote

Old   December 16, 2002, 08:22
Default Re: Pressure drop specification
  #8
Michael Bo
Guest
 
Posts: n/a
Shift to STAR-CD! They have it as a default option where mass flow can be specified directly on periodic boundaries.
  Reply With Quote

Old   December 19, 2002, 20:41
Default Re: Pressure drop specification
  #9
Neale
Guest
 
Posts: n/a
Yes, but then you have to use a solver that sucks and a terrible user interface. No thanks to that suggestion.

Neale
  Reply With Quote

Old   December 19, 2002, 20:48
Default Re: Pressure drop specification
  #10
Neale
Guest
 
Posts: n/a
Swapnil, I think you may have misunderstood subdomains slightly. You don't need user fortran for this. Follow the suggestion of Sharks:

1) Make your entire domain a sub-domain in addition to being a "Fluid Domain".

2) Setup a momentum source term on the subdomain, which happens to be the entire domain. Set the momentum source to the required pressure drop.

3) Setup a translationally periodic condition on the two ends of the pipe.

4) Iterate on step 2 until you get the mass flow rate you desire. You can make a good estimate for 2 by using the Hagen-Pousille (sp?) rule if laminar and use the Moody diagram if turbulent.

There is no need to mess around with user fortran to do this.

Neale

  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
Constant pressure drop condition Jonny6001 FLUENT 0 December 19, 2009 08:36
Total and Static Pressure drop Jaggu FLUENT 3 December 9, 2008 07:03
Pressure Drop at entrance of a rotor-stator. Resnick Main CFD Forum 0 November 20, 2007 15:50
Does star cd takes reference pressure? monica CD-adapco 1 April 19, 2007 11:26
Pressure Specification and Determination J. Weiler FLUENT 1 May 11, 2001 13:37


All times are GMT -4. The time now is 10:49.