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

Different material in different domain

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

Reply
 
LinkBack Thread Tools Display Modes
Old   December 15, 2007, 07:29
Default Different material in different domain
  #1
cheeku
Guest
 
Posts: n/a
Hi,

how to give different material in different domains, if i change the material in one domain then it becomes material in all the domains
  Reply With Quote

Old   December 15, 2007, 09:28
Default Re: Different material in different domain
  #2
ajaymakawana
Guest
 
Posts: n/a
Dear sir,

I am at present using ansys 11 my problem is to analysis the rate of heat transfer from on fluid to another fluid through parallel-pipe heat exchanger.

1. When i am modelling a parallel pipe and use fill command to add fluid domain the outer pipe by default take whole reagion inside it. This means it take inside pipe as fluid domain.

kindly help me out
  Reply With Quote

Old   December 15, 2007, 14:37
Default Re: Different material in different domain
  #3
Greg
Guest
 
Posts: n/a
Hi,

there is a CEL function called "inside()@locator", it helps to create domain-dependent expressions. You will find more information in the CFX users guide.

Variable Density:

density=(1[kg*m^-3])*inside()@Domain1+(1.5[kg*m^-3])*inside()@Domain2

Hope it helps,

Greg
  Reply With Quote

Old   December 16, 2007, 17:45
Default Re: Different material in different domain
  #4
Glenn Horrocks
Guest
 
Posts: n/a
Hi,

Greg's suggestion is one way of doing it, it can also be done by defining one fluid to one domain and another fluid to another domain. I have never done it but I know it can be done.

Glenn Horrocks
  Reply With Quote

Old   December 17, 2007, 10:14
Default Re: Different material in different domain
  #5
cheeku
Guest
 
Posts: n/a
Hi,

I think it can be only done by Gregs way, i have tried in cfx 10&11 giving different fluid in different domain , it dosent work, but if u have one domain solid then its possible. thanks a lot
  Reply With Quote

Old   December 17, 2007, 10:42
Default Re: Different material in different domain
  #6
opaque
Guest
 
Posts: n/a
Dear Cheeku,

Greg's approach is an old trick used in other CFD codes. It works only when all the additional models are the same on both side of the solid. For example, k-epsilon in the inside and outside the pipe. If you want laminar on one side, and turbulent flow on the other side, Greg's approach breaks.

If you are using CFX-11.0, right click on Simulation, and turn off "Constant Domain Physics".. The behavior you have observed is to maintain all the fluid domains the same, turning it off will allow to setup your heat exchanger model. However, NOTE that CFX-Pre will stop making some consistency checks and it is up to you to guarantee a valid physics setup.

ANSYS CFX is a full multidomain physics package, no need for workaround like Greg explained. What you are trying to do, it has been done by several users since the release of CFX-5.7.1.

Hope this helps,

Opaque

  Reply With Quote

Old   December 27, 2007, 01:20
Default Re: Different material in different domain
  #7
Prateek jain
Guest
 
Posts: n/a
Hi cheeku As per my understanding your problem is that although you change the material for different it takes same in all domain. For this you do one thing.
:Right click on my computer
: in advance click on enviorment
: in variable create variable
:in new variable name and valu you feed CFX5_no_CONSTANT_PHYSICS for value -t ok by.........
  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
Domain Imbalance HMR CFX 3 March 6, 2011 21:10
Material identification between a flow domain and a porous domain Ervideiro CFX 1 June 1, 2010 09:50
mass flow in is not equal to mass flow out saii CFX 2 September 18, 2009 08:07
Two-Phase Buoyant Flow Issue Miguel Baritto CFX 4 August 31, 2006 12:02
domain material Juan Phoenics 0 March 29, 2006 11:58


All times are GMT -4. The time now is 23:03.