CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

Speedup with GAMG for simplefoam forward Step

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

Reply
 
LinkBack Thread Tools Display Modes
Old   June 11, 2007, 18:33
Default Hey all, I'm currentley worki
  #1
tutlhino
Guest
 
Posts: n/a
Hey all,
I'm currentley working on the tutorial case in of simpleFoam. For a comparison of the calculation time with cfx, I have set the solver to GAMG such that both use approximately the same Solver. But instead of a speedup, the calculations need more time than with the default PCG/PBiCG-Solvers- I took the following setting:

p GAMG
{
tolerance 1e-08;
relTol 0;

smoother GaussSeidel;

cacheAgglomeration true;

nCellsInCoarsestLevel 10;

agglomerator faceAreaPair;
mergeLevels 1;
};



I tried to change the smallest number of cells and 10 was the best setting for that case (I tried different dense meshes).
Do you have any suggestions why the time is worse or how I could improve it? By the way, does it make sense to use a preconditioner, 'cause in the tutorial case they don't?

Cheers
Florian
  Reply With Quote

Old   June 12, 2007, 02:25
Default Why do you need tolerance 1e-
  #2
Senior Member
 
Srinath Madhavan (a.k.a pUl|)
Join Date: Mar 2009
Location: Edmonton, AB, Canada
Posts: 698
Rep Power: 12
msrinath80 is on a distinguished road
Why do you need tolerance 1e-08? Won't 1e-06 do? How bad is your mesh? Do you use non-conformal faces (i.e. hanging nodes)? AMG will give very good results provided the discretization is decent and the case is fairly large (1 million plus is good). You can try to reduce the iteration count by using the DICGaussSeidel smoother. However, it will increase your computational expense a bit.

Personally, I have found great improvement in the multigrid solver. It beats the pants out of ICCG for my vortex shedding case; upto 3 times as fast!
msrinath80 is offline   Reply With Quote

Old   June 12, 2007, 03:31
Default The setting is just for a time
  #3
tutlhino
Guest
 
Posts: n/a
The setting is just for a time measurement, so tolerance doesn't matter as long as I use everywhere the same. Well I didn't change the tutorial case of the forward Step. I just increased the number of elements in all directions, so doubled it every time. So there should be no hanging nodes, it's a fairly simple mesh. What do you mean with descent discretization, the discretization methods!?

But I'll try your recommendations and increase the mesh density!

Thanks a lot!
Florian
  Reply With Quote

Old   June 12, 2007, 03:35
Default Apologies. I should have elabo
  #4
Senior Member
 
Srinath Madhavan (a.k.a pUl|)
Join Date: Mar 2009
Location: Edmonton, AB, Canada
Posts: 698
Rep Power: 12
msrinath80 is on a distinguished road
Apologies. I should have elaborated. By decent discretization, I refer to pure orthogonal grids with 0 skewness. Check out this[1] thread for more details.

[1] http://www.cfd-online.com/OpenFOAM_D...es/1/4094.html
msrinath80 is offline   Reply With Quote

Old   June 12, 2007, 05:22
Default Here is a recent OpenFOAM pres
  #5
Senior Member
 
Srinath Madhavan (a.k.a pUl|)
Join Date: Mar 2009
Location: Edmonton, AB, Canada
Posts: 698
Rep Power: 12
msrinath80 is on a distinguished road
Here[1] is a recent OpenFOAM presentation on the multi-grid solver.

Check out slide 29 'Computational examples' to see what I meant earlier.

[1] http://powerlab.fsb.hr/ped/kturbo/Op...nadaPrecon.pdf
msrinath80 is offline   Reply With Quote

Old   June 24, 2007, 10:09
Default Thanks a lot for the link to t
  #6
tutlhino
Guest
 
Posts: n/a
Thanks a lot for the link to the presentation!
I've run now several simulations up to 2 mio elements.But I realized that with increasing the number of elements I also have to change
nCellsInCoarsestLevel, 'cause otherwise the time for GAMG is even higher than with others like PCG.

Is there an approximate formula which tells me what is the best setting of nCellsInCoarsestLevel according to a certain number of cells? Something like:

nCellsInCoarsestLevel ~ C *#Cells

with C being a constant (e.g. 0.1...)

Regards
  Reply With Quote

Old   June 24, 2007, 11:26
Default Check the older posts in the f
  #7
Senior Member
 
Srinath Madhavan (a.k.a pUl|)
Join Date: Mar 2009
Location: Edmonton, AB, Canada
Posts: 698
Rep Power: 12
msrinath80 is on a distinguished road
Check the older posts in the forum[1,2]. If I recall correctly, I think the recommendation was anything from a dozen to a couple hundred cells in Serial mode and around 20-30 cells in Parallel mode. This is of course the recommendation for OpenFOAM 1.3 (i.e. AMG solver). I am not sure if it can be readily translated to the GAMG solver in OpenFOAM 1.4. On second thoughts however, I think you are doing the right thing, i.e. experimenting with different values.

[1] http://www.cfd-online.com/OpenFOAM_D...tml?1162930507

[2] http://www.cfd-online.com/OpenFOAM_D...tml?1172129883
msrinath80 is offline   Reply With Quote

Old   June 24, 2007, 11:30
Default Oh, and by the way, if you use
  #8
Senior Member
 
Srinath Madhavan (a.k.a pUl|)
Join Date: Mar 2009
Location: Edmonton, AB, Canada
Posts: 698
Rep Power: 12
msrinath80 is on a distinguished road
Oh, and by the way, if you use a uniformly spaced purely orthogonal grid, I've noticed that changing

mergeLevels 1;

to

mergeLevels 2; or even mergeLevels 3; speeds up the GAMG solver.
msrinath80 is offline   Reply With Quote

Old   June 24, 2007, 11:58
Default How these changes affect the f
  #9
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,894
Rep Power: 26
alberto will become famous soon enoughalberto will become famous soon enough
How these changes affect the final result, if they do? What about stability of the solution?

Regards,
A.
__________________
Alberto Passalacqua

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as live DVD/USB, hard drive image and virtual image.
OpenQBMM - An open-source implementation of quadrature-based moment methods
alberto is offline   Reply With Quote

Old   June 24, 2007, 21:44
Default To my knowledge, multi-grid is
  #10
Senior Member
 
Srinath Madhavan (a.k.a pUl|)
Join Date: Mar 2009
Location: Edmonton, AB, Canada
Posts: 698
Rep Power: 12
msrinath80 is on a distinguished road
To my knowledge, multi-grid is merely a solution approach. Deep down it also uses conventional solvers such as the conjugate gradient. So I don't quite see why the final result would be affected unless you change tolerance and/or reltol to other values. As for the stability of the numerical solution, it is primarily affected by the choice of numerical schemes used for space/time discretization.

Someone please correct me if I'm wrong!
msrinath80 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
SimpleFoam and Time Step continuity errors philippose OpenFOAM Running, Solving & CFD 55 April 11, 2010 06:29
forward step: treating singularity pt for WENO FV DSS Main CFD Forum 1 January 18, 2007 03:15
Forward step shuo OpenFOAM Running, Solving & CFD 1 October 23, 2006 02:15
Inviscid flow over a forward/backward facing step Abhijit Tilak Main CFD Forum 3 February 16, 2005 10:18
Supersonic flow over a forward facing step Chan K I Main CFD Forum 1 October 19, 2000 16:43


All times are GMT -4. The time now is 22:33.