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

Problem with laminar 2d channel flow

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

Reply
 
LinkBack Thread Tools Display Modes
Old   September 30, 2005, 04:53
Default Problem with laminar 2d channel flow
  #1
Quarkz
Guest
 
Posts: n/a
Hi all,

I'm trying to solve a simple 2d channel flow, uniform flow in, expected parabolic flow out. I'm using non-staggered unsteady fractional step FVM, solving momentum eqn then pressure poisson eqn for divergence free condition

My problem is large velocities appearing at the inlet, especially near the corners (large vertical velocity). The problem gets worse as time proceeds and diverges. The large velocities change happen after the poisson eqn and adding the pressure difference to the velocities.

For the initial condition: a uniform 1.0 velocity at the west face of the inlet cells. all other u,v,p =0

May I know if this is acceptable for an initial condition? Or must it be divergence-free?

For the BC: a uniform 1.0 velocity at the west face of the inlet cells. dp/dx=0 top & bottom walls zero velocities, dp/dx=0 Outlet has convective BC, p=0.

I can get the solutions by setting u=1 (cell center) throughout the channel, but in that case the unsteady nature can't be captured correctly.

Thank you Yours sincerely, Wee Beng

  Reply With Quote

Old   September 30, 2005, 06:10
Default Re: Problem with laminar 2d channel flow
  #2
diaw
Guest
 
Posts: n/a
You may want to be careful about applying u-velocity at the corner nodes of the inlet edge.

Perhaps you could look into loosening up your outlet condition. I don't know your particular code, but in many cases (FVM) I specify a 'free outlet' & let the system sort out its own pressure.

diaw...
  Reply With Quote

Old   September 30, 2005, 06:15
Default Re: Problem with laminar 2d channel flow
  #3
andy
Guest
 
Posts: n/a
The problem is likely to lie with your pressure smoothing. What do you do with your pressure smoothing mass flux at the boundary?

What does divergence free mean numerically to your scheme? If you do not have mass sources that sum exactly to zero your pressure Poisson equation will have no solution (the matrix is singular with normal boundary conditions) and, over time, your solution will blow up. This is trivial to check: simply sum your source terms in the Poisson equation. What is less trivial is working out how to handle the pressure smoothing on the boundary in a reasonable manner.

  Reply With Quote

Old   September 30, 2005, 09:52
Default Re: Problem with laminar 2d channel flow
  #4
ramp
Guest
 
Posts: n/a
Check your pressure subroutine.

Best regards, ramp
  Reply With Quote

Old   October 2, 2005, 04:41
Default Re: Problem with laminar 2d channel flow
  #5
zonexo
Guest
 
Posts: n/a
hi all,

I've tried letting dp/dx=0 at the outlet, but the solution also diverges. I've run cavity test before and it works very well.

andy: what do u mean by "pressure smoothing"? is it similar to the under-relaxation for SIMPLE schemes? I've tried that and it worked, but in that case, the unsteady behavior won't be captured accurately, right?

initially, if i impose a uniform velocity at the west face of the inlet cells, then the mass sources will not sum to zero, ie not divergence free. Is that why solution blows up?

So how should I impose the uniform inlet velocity and yet have a divergence free initial condition?

I'll be glad if anyone can give some leads or point me to some references.

Thank alot!

  Reply With Quote

Old   October 2, 2005, 07:50
Default Re: Problem with laminar 2d channel flow
  #6
andy
Guest
 
Posts: n/a
> what do u mean by "pressure smoothing"?

In a non-staggered scheme this is the extra terms involving pressure derivatives added to the mass flux to stop pressure/velocity decoupling. What to do at a wall is problematic because you will get mass flux through the wall if you add the term and severe jumps in the velocity if you do not given the presence of significant normal pressure gradients (e.g. swirling flow).

> ...then the mass sources will not sum to zero...

In which case your pressure equation has no solution. If the mass sources sum to a positive value then iteratively solving the pressure equation will simply drive the level of pressure up without converging it (no boundary conditions to pin the level). Or down for a negative source.

> So how should I impose the uniform inlet velocity and yet have a divergence free initial condition?

You do not need a divergence free initial condition for most schemes (there are one or two exceptions). But you do need the mass sources to sum to exactly zero. They are not the same thing. The simplest way to achieve this with a conservative scheme is to scale the outflow to match the imposed inflow. Since you scheme behaved with zero inflow and zero outflow it might work.
  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
CFX Treatment of Laminar and Turbulent Flows Jade M CFX 6 January 26, 2013 11:11
[GAMBIT] Gambit & 3d open channel flow mesh problem esgee ANSYS Meshing & Geometry 7 April 10, 2012 00:51
how to solve a problem involving both laminar and turbulent flow seefd FLUENT 1 June 3, 2011 03:20
Laminar Periodic flow problem Leigh FLUENT 0 February 14, 2006 07:04
Periodic flow boundary condition problem sudha FLUENT 3 April 28, 2004 08:40


All times are GMT -4. The time now is 04:01.