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

Convective boundary condition

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

Reply
 
LinkBack Thread Tools Display Modes
Old   May 24, 2002, 10:48
Default Convective boundary condition
  #1
STN
Guest
 
Posts: n/a
Dear all...

I'm try to introduce convective BC, d(Phi)/dt + Uc*d(Phi)/dX = 0.0, in to my 3D-transient code. My code based on SIMPLE with staggered grid arrangement.

The problem is : solution is not converge when Convective BC is used. The simulation starts with stagnant fluid at t=0. But ths code works well for the same problem when zero gradient, d(Phi)/DX = 0.0, is applied.

Any idea or suggestion is very please to me. Thank you very much
  Reply With Quote

Old   May 24, 2002, 23:17
Default Re: Convective boundary condition
  #2
versi
Guest
 
Posts: n/a
The time discretization of your CBC may be a factor. Explict marching may require very small Dt. Try to use implicit one.
  Reply With Quote

Old   May 25, 2002, 11:50
Default Re: Convective boundary condition
  #3
adarsh
Guest
 
Posts: n/a
use the stability crieteria to determine the largest permissible Dt and run the code for Dt smaller than this
  Reply With Quote

Old   May 28, 2002, 06:45
Default Re: Convective boundary condition
  #4
STN
Guest
 
Posts: n/a
Thank you for your response.

Actually, in my code, implicit time discretization is used. I try to follow your suggestion by reduce Dt to very small value compare to flow time scale but it still not converge. The residual oscilates over some value.

At this point, I wonder that Am I discretize CBC correct ?

d(Phi)/dt + Uc*d(u)/dx = 0

Phi(i,n) = Phi(i,n-1) + Uc*dt/dx*(u(i,n) - u(i-1,n))

where i represents spatial index and n represents time index.

Suggestion is very please to me. Thank you...
  Reply With Quote

Old   May 28, 2002, 08:43
Default Re: Convective boundary condition
  #5
Nicola
Guest
 
Posts: n/a
d(Phi)/dt + Uc*d(u)/dx = 0 Phi(i,n) = Phi(i,n-1) + Uc*dt/dx*(u(i,n) - u(i-1,n)) It seems correct, but problems may arise from wrong artificial boundary conditions. Remember: in 3D subsonic flows, at inlet 4 boundary conditions and only an artificial one (total 5), at exit 4 artificial boundary conditions and only a physichal one (total 5). At wall, 4 physical boundary conditions and only an artificial one (total 5). I have no experience in convective boundary conditions, so my questions may sound silly: what is Phi? What are Uc and u? CBD seem a scalar equation, so it means that you have 1 new boundary condition (i don't know if it is at wall or at inlet or exit plane): what of the other boundary conditions (i mean no slip condition, adiabatic wall, and so on)? Be sure your system is well posed, that is that physical and artificial boundary conditions are compatible. Hope it helps,

Nicola
  Reply With Quote

Old   May 29, 2002, 08:47
Default Re: Convective boundary condition
  #6
Enrico
Guest
 
Posts: n/a
It's not completely clear to me what you mean for *lack of convergence*: I assume no convergence within a time-step.

I noticed that you discretize:

d(Phi)/dt + Uc*d(u)/dx = 0

as:

Phi(i,n) = Phi(i,n-1) + Uc*dt/dx*(u(i,n) - u(i-1,n))

Although we use semi-implicit discretization in our FV codes (i.e. implicit diffusion and explicit convection), we found that it is important to use the following discretization:

Phi(i,n)= Phi(i,n-1)+Uc*dt/dx*(u(i,n-1) - u(i-1,n-1))

which is implemented as a standard Dirichlet BC.

In fact it's easy to show that using a velocity field, in the representation of du/dx, that is divergence-free (i.e. that obtained at the previous time-step), you are guaranteed that your mass is globally conserved, and this prevents divergence.

Good luck
  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
Convective boundary condition andrea_barbera OpenFOAM Running, Solving & CFD 4 March 4, 2010 05:36
convective boundary condition Mani CFX 7 February 2, 2008 17:25
Convective Boundary Condition garni FLUENT 0 September 25, 2005 13:00
Trimmed cell and embedded refinement mesh conversion issues michele OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 2 July 15, 2005 04:15


All times are GMT -4. The time now is 06:06.