CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > CFX

parallelization problem

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

Like Tree2Likes
  • 2 Post By ghorrocks

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   June 29, 2022, 05:26
Default parallelization problem
  #1
New Member
 
Tahmineh
Join Date: Apr 2022
Posts: 8
Rep Power: 3
TahminehAd is on a distinguished road
Hello Everyone,
Is it possible to have different results of a transient simulation on a personal laptop and a cluster with 28 cores?
I have this problem that I run one simulation on my laptop and on the cluster to speed up the simulation time, but the results of the same file, with the same simulation set up are different. For example, on my laptop the courant number is relatively small while on the cluster it is so much high. Or on my laptop the simulation converges with lower number of iterations but on the cluster it doesn't converge or in high number of iteration the convergence happens.
I want to know if that is even possible and if yes under what conditions this problem happens.
Thank you in advance.
TahminehAd is offline   Reply With Quote

Old   June 29, 2022, 06:04
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,623
Rep Power: 142
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
This is uncommon, but it does happen. It is usually caused by a strong gradient (eg a free surface, shockwave or other very severe gradient) lying on top of a domain partition boundary.

The fix for this is to change to a different partitioning algorithm which keeps the mesh partition boundaries away from the strong gradients, or if it needs to cross them crosses them around 90 degrees.

So if you have a free surface which is horizontal, if you use vertical partitions it will be much better than horizontal partitions.

The default partitioning algorithm is METIS, so try one of the recursive bisection or directional methods.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   June 29, 2022, 06:29
Default
  #3
New Member
 
Tahmineh
Join Date: Apr 2022
Posts: 8
Rep Power: 3
TahminehAd is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
This is uncommon, but it does happen. It is usually caused by a strong gradient (eg a free surface, shockwave or other very severe gradient) lying on top of a domain partition boundary.

The fix for this is to change to a different partitioning algorithm which keeps the mesh partition boundaries away from the strong gradients, or if it needs to cross them crosses them around 90 degrees.

So if you have a free surface which is horizontal, if you use vertical partitions it will be much better than horizontal partitions.

The default partitioning algorithm is METIS, so try one of the recursive bisection or directional methods.
Thank you for your answer. Exactly after I added free surface into my simulation, that problem happened. So instead of METIS algorithm there are four alternative methods: MeTiS Recursive Bisection, Simple Assignment, Directional Recursive Coordinate Bisection, Optimized Recursive Coordinate Bisection, Recursive Coordinate Bisection. Which one do you think can solve the problem better than others?
TahminehAd is offline   Reply With Quote

Old   June 29, 2022, 07:44
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,623
Rep Power: 142
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
You have to choose which ever one keeps the partition boundaries away from the free surface. You can view the partition boundaries by loading a res file into CFD-Post and look for the variable Partition number (or something like that).
Opaque and TahminehAd like this.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Reply

Tags
parallel calculation

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Problem with parallelization and a constant field located at constant folder rucky96 OpenFOAM 7 January 29, 2021 17:54
DEFINE_PROFILE parallelization problem sakura006 Fluent UDF and Scheme Programming 2 November 26, 2019 11:20
BuoyantBoussinesqSimpleFoam_Facing problem Mondal131211 OpenFOAM Running, Solving & CFD 1 April 10, 2019 20:41
Gambit - meshing over airfoil wrapping (?) problem JFDC FLUENT 1 July 11, 2011 06:59
Adiabatic and Rotating wall (Convection problem) ParodDav CFX 5 April 29, 2007 20:13


All times are GMT -4. The time now is 21:29.