|
[Sponsors] |
August 3, 2016, 11:40 |
No speedup observed after using renumberMesh
|
#1 |
Senior Member
Tarak
Join Date: Aug 2010
Location: State College, PA
Posts: 111
Rep Power: 15 |
Hi,
I have been using renumberMesh to speed up my parallel calculation of pimpleDyMFoam (for 17 million cells sperad across 256 processors, having AMI interface) but didn't observe any increase in speed compared to a similar case without using renumberMesh. I used the utility after the parallel decomposition and the bandwidth decreased significantly to 2379 from 67180 after using the utility. Can someone let me know if he/she has obtained any increase in speed using this utility? |
|
August 3, 2016, 11:54 |
|
#2 |
Member
Bruno Blais
Join Date: Sep 2013
Location: Canada
Posts: 64
Rep Power: 12 |
I am not sure, but I believe you need to renumber before you decompose?
Also, if you have a large number of processor, the impact of renumbering will be much smaller. |
|
March 19, 2022, 02:14 |
|
#3 | |
Senior Member
Join Date: Mar 2010
Posts: 173
Rep Power: 17 |
Quote:
Thanks in advance |
||
March 19, 2022, 14:05 |
|
#4 |
Senior Member
Herpes Free Engineer
Join Date: Sep 2019
Location: The Home Under The Ground with the Lost Boys
Posts: 932
Rep Power: 12 |
-- Can anyone confirm this - ie that you should run renumberMesh before you decomposePar??
Yes. Please use "renumberMesh" in serial prior to the decomposition step. But I can't recall the main reason why we should avoid "renumberMesh" in parallel (but there was a reason - if I am not wrong, it was about sampling.) If you still want to run the "renumberMesh" in parallel, please use its "-parallel" flag.
__________________
The OpenFOAM community is the biggest contributor to OpenFOAM: User guide/Wiki-1/Wiki-2/Code guide/Code Wiki/Journal Nilsson/Guerrero/Holzinger/Holzmann/Nagy/Santos/Nozaki/Jasak/Primer Governance Bugs/Features: OpenFOAM (ESI-OpenCFD-Trademark) Bugs/Features: FOAM-Extend (Wikki-FSB) Bugs: OpenFOAM.org How to create a MWE New: Forkable OpenFOAM mirror |
|
March 19, 2022, 21:28 |
|
#5 | |
Senior Member
Join Date: Mar 2010
Posts: 173
Rep Power: 17 |
Quote:
Thanks for your answer but the question was not whether renumberMesh should be executed in parallel or serial, but rather whether renumberMesh should be run on the undecomposed mesh or the decomposed mesh. Since renumbering algorithms are designed to move the coefficients closer to the diagonal (reduce coefficient matrix bandwidth) then its not immediately clear whether if you did this before a decomposePar, whether the better conditioned coefficient matrix would be persist (and be optimal) after a domain decomposition. |
||
March 21, 2022, 01:04 |
|
#6 |
Member
David GISEN
Join Date: Jul 2009
Location: Germany
Posts: 68
Rep Power: 16 |
I tried renumberMesh several times over the years and never had a significant effect, no matter the order of execution.
In my most recent test (4.7 mio cells, 64 procs, interFoam, v2012), I observed no speedup if renumbered before decomposition and even a speed loss if renumbered after decomposition. Even though the bandwidth reported decreased strongly in both cases. |
|
March 21, 2022, 01:11 |
|
#7 | |
Senior Member
Join Date: Mar 2010
Posts: 173
Rep Power: 17 |
Quote:
I had thought a stronger diagonal in the coefficient matrix might improve stability but from memory, I think thats probably more the conditioning of the matrix i.e. the ratio of the largest / smallest eigen values rather than the bandwidth / diagonal ... |
||
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
[mesh manipulation] Some questions on blockMesh, decomposePar and renumberMesh | Leech | OpenFOAM Meshing & Mesh Conversion | 19 | April 5, 2019 19:21 |
renumberMesh problems | Jonathan | OpenFOAM Pre-Processing | 1 | May 10, 2016 16:38 |
RenumberMesh causing divergence | altair279 | OpenFOAM Running, Solving & CFD | 0 | April 1, 2015 18:33 |
Superlinear speedup in OpenFOAM 13 | msrinath80 | OpenFOAM Running, Solving & CFD | 18 | March 3, 2015 05:36 |
Parallel efficiency and speedup info | lakeat | OpenFOAM Running, Solving & CFD | 2 | August 31, 2009 11:05 |