# Convective boundary condition

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

 May 24, 2002, 10:48 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

 May 24, 2002, 23:17 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.

 May 25, 2002, 11:50 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

 May 28, 2002, 06:45 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...

 May 28, 2002, 08:43 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

 May 29, 2002, 08:47 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

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post HMR CFX 5 October 10, 2016 05:57 andrea_barbera OpenFOAM Running, Solving & CFD 4 March 4, 2010 05:36 Mani CFX 7 February 2, 2008 17:25 garni FLUENT 0 September 25, 2005 13:00 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 20:02.