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

Convergence criteria for pressure correction method solving Unsteady N-S equtions

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

Like Tree2Likes
  • 1 Post By FMDenaro
  • 1 Post By andy_

Reply
 
LinkBack Thread Tools Display Modes
Old   March 7, 2013, 03:24
Default Convergence criteria for pressure correction method solving Unsteady N-S equtions
  #1
Member
 
Osman
Join Date: Oct 2012
Location: Japan
Posts: 51
Rep Power: 4
o_mars_2010 is on a distinguished road
I am using a pressure correction method for solving Unsteady Navier-Stokes equations, i want to know what is the convergence criteria i have to use for every time step.
Attached Images
File Type: jpg Equations.jpg (15.2 KB, 33 views)
o_mars_2010 is offline   Reply With Quote

Old   March 7, 2013, 04:49
Default
  #2
Senior Member
 
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 1,569
Rep Power: 20
FMDenaro will become famous soon enough
Quote:
Originally Posted by o_mars_2010 View Post
I am using a pressure correction method for solving Unsteady Navier-Stokes equations, i want to know what is the convergence criteria i have to use for every time step.

Convergence must imply that you fulfill the divergence-free constraint (at some tolerance).
o_mars_2010 likes this.
FMDenaro is offline   Reply With Quote

Old   March 7, 2013, 04:57
Default
  #3
Member
 
Osman
Join Date: Oct 2012
Location: Japan
Posts: 51
Rep Power: 4
o_mars_2010 is on a distinguished road
So, for example, the maximum cell value in the Divergence matrix must be less than 1e-6 for a time step!!!
what is the criteria for this value i.e 1e-6 ??
what if the maximum cell value in the Divergence matrix is not satisfying this condition ??
which equations i have to iterate in the same time step??
o_mars_2010 is offline   Reply With Quote

Old   March 8, 2013, 19:50
Default
  #4
Member
 
Osman
Join Date: Oct 2012
Location: Japan
Posts: 51
Rep Power: 4
o_mars_2010 is on a distinguished road
Any reply?
o_mars_2010 is offline   Reply With Quote

Old   March 9, 2013, 13:15
Default
  #5
Senior Member
 
Lefteris
Join Date: Oct 2011
Location: UK, Greece
Posts: 187
Rep Power: 5
Aeronautics El. K. is on a distinguished road
What you ask is not very clear, at least to me. I will refer you again to Ferziger and Peric's book "computational methods for fluid dynamics", pages 124-127.
__________________
Lefteris

Aeronautics El. K. is offline   Reply With Quote

Old   March 9, 2013, 20:24
Default
  #6
Member
 
Osman
Join Date: Oct 2012
Location: Japan
Posts: 51
Rep Power: 4
o_mars_2010 is on a distinguished road
I am not talking about the convergence criteria of poisson Eq. solver.
I am talking about the convergence criteria for one unsteady time step.
I think the answer of Filippo Maria Denaro is correct.
however, what i want to know if i am using a staggered grid, then:
(for example)
U matrix will be 100x99 cells
V matrix will be 99x100 cells
the Divergence matrix will be 100x100

So what i want to know:

1- Is the cell with with the maximum value in comparison with all other cells in the divergence matrix must be less than the tolerance we assume?
2- how can we decide the value of the tolerance?
3- Do I have to iterate all the equations i attach in the 1st post to reach to the required tolerance?
4- Isn't these iterations means that i am going forward in time although i am doing iteration for the same time step ?
o_mars_2010 is offline   Reply With Quote

Old   March 10, 2013, 06:46
Default
  #7
Senior Member
 
andy
Join Date: May 2009
Posts: 129
Rep Power: 8
andy_ is on a distinguished road
If you wish to iterate out the non-linearity in the momentum equation I would suggest using a different scheme which includes an estimate of the u^n+1 value in the differencing of the convection terms. Including the diffusion terms implicitly in the momentum equation is normally done primarily for reasons of stability not accuracy. If the diffusion number remains stable it would be more efficient to use a fully explicit momentum equation. In practice a tight tolerance on the diffusion terms which are by definition small in high Reynolds number flows is unlikely to be worth the computational cost so long as the linear solver is one that gives reasonable values with a few steps.

The solution of the pressure related quantity is going to take most of the computational time and so one tends to use a larger tolerance during any settling down phase and tighten it during the accurate phase. Some have put forward the view that the residual errors from not fully solving the Poisson equation only need to be significantly less than the truncation error. Although one can see where this is coming from, small violations in continuity have a long history in destabilising flows and causing problems at boundaries (boundary conditions for schemes using pressure related quantities like your phi also need care). Perhaps the simplest thing to do is to perform a representative simulation with the Poisson equation solved into roundoff and then repeat with looser tolerances and look at what changes.
o_mars_2010 likes this.
andy_ is offline   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
Moving mesh Niklas Wikstrom (Wikstrom) OpenFOAM Running, Solving & CFD 122 June 15, 2014 06:20
transsonic nozzle with rhoSimpleFoam Unseen OpenFOAM Running, Solving & CFD 7 April 16, 2014 03:38
pisoFoam with k-epsilon turb blows up - Some questions Heroic OpenFOAM Running, Solving & CFD 26 December 17, 2012 04:34
High Courant Number @ icoFoam Artex85 OpenFOAM Running, Solving & CFD 9 January 3, 2012 09:06
Parallel rasInterFoam openfoam_user OpenFOAM Running, Solving & CFD 4 November 1, 2008 05:14


All times are GMT -4. The time now is 09:47.