|
[Sponsors] |
[ANSYS Meshing] Cant get parallel meshing to work in V18.2 |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
December 19, 2018, 14:26 |
Cant get parallel meshing to work in V18.2
|
#1 |
New Member
Kevin Jones
Join Date: Feb 2011
Posts: 17
Rep Power: 15 |
Sorry if this is a repeat question. I've done some searching, but other questions related to this don't seem to help. I'm using ANSYS V18.2 and can easily get many cores to work in CFX, but when meshing I can't seem to get it to use more than one core. This is frustrating, as I have a pretty robust machine (Dual Xeon 8-core, 96GB RAM). In the task manager, I see the AnsMeshingServer.exe using 5% CPU, and the AnsysWB Module using another 5%.
I've tried a couple of things already. In the "Details of Mesh" under Advanced, there is a "Number of CPUs for Parallel Part Meshing," but that has no effect. Also, under Tools > Options > Meshing > Meshing I can set the number of cores for Meshing Methods and also for Parallel Part Meshing, but these also do not seem to have an effect. Is there a licensing option for parallel meshing separate from parallel operation of CFX and FEM sims? Thanks in advance for any useful advice. |
|
December 20, 2018, 06:55 |
|
#2 |
Member
Baris PULAT
Join Date: Sep 2016
Location: Italy
Posts: 59
Rep Power: 10 |
Just a quick question how is your geometry is it only one part or multiple parts?
Because as long as I know with one part parallel meshing doesn't work. |
|
December 20, 2018, 13:32 |
|
#3 | |
New Member
Kevin Jones
Join Date: Feb 2011
Posts: 17
Rep Power: 15 |
Quote:
I was afraid that this might be the issue - it's just one part. Will it only perform parallel meshing if I partition the domain myself? |
||
November 3, 2020, 08:12 |
|
#4 |
Member
Join Date: Apr 2020
Posts: 76
Rep Power: 6 |
Hello Jones
Were you able to resolve this? How do I partition the mesh for parallel meshing? Thanks |
|
November 3, 2020, 12:47 |
|
#5 |
New Member
Kevin Jones
Join Date: Feb 2011
Posts: 17
Rep Power: 15 |
Yes. I can't claim to be an expert on this, but the way I resolved it was to cut up the domain in SolidWorks, where I originally generated the domain. I reassemble the parts into an assembly in SW, and then import the assembly into CFX. Then CFX will process each block individually using a different core for each. If you create the blocks intelligently, then you can use them to provide location-specific sizing control. Further, if you alter meshing parameters that only affect one block, for example face or body sizing, then only that block will need to be remeshed, so grid refinements can also be pretty fast. Natively, the mesher will not force the meshes to match across inter-block connections. I think there may be a way to do this, but I usually just play around with face-sizing controls until I get a size-match that is close enough for me. If the splits are in regions where not much is happening, then it probably doesn't matter if element sizing is similar, but if you have a split in a high-gradient area, then you should take some care to get them close.
|
|
November 3, 2020, 17:06 |
|
#6 |
Senior Member
Erik
Join Date: Feb 2011
Location: Earth (Land portion)
Posts: 1,183
Rep Power: 23 |
I'm no expert either, but I wouldn't mesh the blocks separately if they are one domain if I didn't absolutely have to. Then you will have to use GGI interfaces instead of having a continuous mesh. This will make the solution less accurate, and also take longer, and use more memory to solve. You won't gain much time in the mesh process, and you will likely lose that time solving, setting up the interfaces in Pre, and have a less accurate solution. Not worth it in my opinion.
|
|
November 3, 2020, 17:17 |
|
#7 | |
New Member
Kevin Jones
Join Date: Feb 2011
Posts: 17
Rep Power: 15 |
Quote:
|
||
November 4, 2020, 07:52 |
|
#8 |
Member
Join Date: Apr 2020
Posts: 76
Rep Power: 6 |
Hi
Thanks for your reply. Although my aim is to mesh it in the mesh component rather than CFX/fluent. But I see what you mean, so can you create separate parts in the mesh component? Regards |
|
November 4, 2020, 13:18 |
|
#9 | |
New Member
Kevin Jones
Join Date: Feb 2011
Posts: 17
Rep Power: 15 |
Quote:
If evcelica is opposed to this approach, perhaps they can provide alternate approaches for tackling jobs that are impractical or impossible to run on a single core. The challenge that I have run into is that modern computer architectures that are optimized for high speed solving typically have a large number of slower cores. If you can take advantage of all of the cores, then they are faster than their counterparts that have fewer, but higher speed cores. It's trivial to run the flow solvers using parallel processing to take advantage of multiple cores. However, my experience has been that if you give the mesher a single block domain, it will only use a single core, so machines that have fewer, faster cores will excel for meshing. Since I don't really want to use one machine for meshing and another for solving, domain decomposition has been my workaround. Some of my larger jobs have on the order of 40 million nodes and 120 million cells. Grid generation on a single block was requiring about 7 to 8 hours. If the mesher failed or you were unhappy with the mesh, it was another day to get a new mesh. This was on a machine with a pair of Xeon Silver chips, and 96GB of RAM, but during meshing, just one core was in use by the mesher. Once I had a mesh, I could use something like 20 cores for the solver, and I could get a converged CFX solution using SST and GT transition modeling in less time than the it took to get a mesh. I hope this helps. |
||
November 5, 2020, 11:40 |
|
#10 |
Member
Join Date: Apr 2020
Posts: 76
Rep Power: 6 |
Hi
Thanks for your reply and suggestion. Sadly I am not too well versed with Ansys to understand your method. I have a domain with some building geometry in them (urban airflow simulation). I aim to generate about 15-20million mesh elements. It takes about 30-40 minutes currently, I just want to speed up with parallel. I will look up some videos/tutorials online. If you do find some basic tutorial on parallel meshing please share. Regards |
|
November 5, 2020, 12:15 |
|
#11 | |
New Member
Kevin Jones
Join Date: Feb 2011
Posts: 17
Rep Power: 15 |
Quote:
If you generated the volume inside Ansys using DesignModeler or SpaceClaim, I'm not quite sure what tools they give you do dice up a volume. I never use those to generate anything but the simplest of geometries. |
||
November 5, 2020, 14:16 |
|
#12 | |
Member
Join Date: Apr 2020
Posts: 76
Rep Power: 6 |
Quote:
Since my geometry is simple, I used Rhino to model that. I exported that as IGES format and imported into Mesh component (Ansys) and started meshing it. But since I know that meshing only works if you have more than one component, I created the model as a combination of various parts. Can I share my mesh file with you so that you can have a look? Regards |
||
November 5, 2020, 14:51 |
|
#13 | |
New Member
Kevin Jones
Join Date: Feb 2011
Posts: 17
Rep Power: 15 |
Quote:
|
||
November 6, 2020, 15:46 |
|
#14 |
Member
Join Date: Apr 2020
Posts: 76
Rep Power: 6 |
PFA the link to download the mesh file. Since it was over the upload limit, I am sharing via WeTransfer
https://wetransfer.com/downloads/65a...6194154/591e2c Thanks |
|
November 6, 2020, 15:58 |
|
#15 | |
New Member
Kevin Jones
Join Date: Feb 2011
Posts: 17
Rep Power: 15 |
Quote:
|
||
November 7, 2020, 07:06 |
|
#16 | |
Member
Join Date: Apr 2020
Posts: 76
Rep Power: 6 |
Quote:
Thanks |
||
November 7, 2020, 13:40 |
|
#17 | |
New Member
Kevin Jones
Join Date: Feb 2011
Posts: 17
Rep Power: 15 |
Quote:
Example.zip Hope this helps. |
||
November 9, 2020, 06:56 |
|
#18 | |
Member
Join Date: Apr 2020
Posts: 76
Rep Power: 6 |
Quote:
Yes, thanks. The parallel meshing works now |
||
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
simpleFoam parallel | AndrewMortimer | OpenFOAM Running, Solving & CFD | 12 | August 7, 2015 19:45 |
RP_Set_Integer does not work in parallel | 86lolo | Fluent UDF and Scheme Programming | 2 | July 3, 2014 12:37 |
Could SU2_V2.0.2 work properly with continuous_adjoint.py script in parallel mode? | Tommy Chen | SU2 Shape Design | 1 | April 18, 2013 14:06 |
Parallel meshing using XP64 with PVM in CFX Mesh | Huw | ANSYS Meshing & Geometry | 4 | July 12, 2010 11:24 |
CFX5.6 (Build) Parallel Meshing | David Hargreaves | CFX | 2 | January 12, 2005 13:39 |