June 7, 2023 at 3:41 pmNick WallishSubscriber
We are exploring potential speed-ups using GPGPU for our flow studies. Currently, we see no speed increase when using a fixed number of processor threads and with an Nvidia RTX A5000 GPU enabled or disabled.
Originally we attempted this in v2022 R2, but updated to 2023 R1 to see if that would help. Fluent is reporting that the GPU is there and selected, but we see nearly identical performance with/without the GPU. This is not in Native GPU mode, but with the GPU added in the Parallel tab of the launcher. Our case uses the following models: transient, VOF Multiphase, k-epsilon Realizable turbulence, and DPM. I have attempted to modify the settings under /solve/set/amg-options/amg-gpgpu-options to enable for limited equations, and while after iteration it reports "AMG on GPU" in the console, there is still no speed change.
Is it possible to accelerate this simulation on GPU?
June 8, 2023 at 3:05 pmRobAnsys Employee
It's covered here https://ansyshelp.ansys.com/account/Secured?returnurl=/Views/Secured/corp/v231/en/flu_ug/UsingGraphicsProcessingUnitsGPUsWit-EC38970B.html but the gpgpu benefits are limited in many cases.
Check how the load is balanced on the cpus. As VOF is a free surface tracker and DPM tends to have particles concentrated on some nodes you may find one or both of those models to slow the system down. Have a look at Parallel Load Balancing to see if that helps (with or without gpgpu).
The native GPU solver will give you a perfomance improvement, but not (yet) with all physics.
June 8, 2023 at 3:36 pmNick WallishSubscriber
Hello, thank you for the response. I have followed the instructions in that documentation, but that has only gotten me to where I was when I posted: enabling the GPU for some of the physics using the TUI options does not have ANY impact on performance. To provide some numbers: 4 CPU and 0 GPU is approximately 10.9 sec/iter, 4 CPU and 1 GPU is 10.7 sec/iter. 32:0 results in 2.44 sec/iter and 32:1 results in 2.42 sec/iter. These numbers imply the GPU is having zero effect on calculation speeds.
Am I missing something? The documentation refers to the GPU working on coupled systems but not scalar systems unless enabled, but I see no benefit with or without enabling for scalar systems (implying it is also doing nothing for the coupled calculation). Furthermore, I see no change in GPU resource usage through system monitoring (no change in memory usage, etc.).
Can you provide further insight into expected benefits and ensuring the GPU is being used?
June 8, 2023 at 4:02 pmRobAnsys Employee
With VOF you'll only have P-V coupled, which may not give you much of a boost in this case. It should be more noticeable with the single phase models with more coupled equations.
June 12, 2023 at 9:50 pmNick WallishSubscriber
Hello, I have an update: After enabling pressure and momentum manually to use the GPU (and getting the message before iteration about AMG and compilation with CUDA runtime), I checked nvidia-smi to see if Fluent was using any GPU. Next to both the fluent and cortex processes there is a n/a listed for GPU usage. I verified that the GPU was selected as well.
So in essence: with GPGPU enabled, my simulation is not using the GPU at all, which explains why there was no speed change. Can you provide some insight into why this might be? Are there further options to be checked? What is the expected workflow or behavior when adding a GPGPU?
June 13, 2023 at 1:57 pmRobAnsys Employee
The gpu acceleration was only ever used on a few bits of multigrid and some of the radiation tracking schemes. Turn off VOF and see if that gives you any load on the gpu: the VOF part itself wasn't gpu compatible. Development have since moved onto the dedicated gpu solver, which gives significant acceleration for the physics it currently supports: further models will be available in time.
- You must be logged in to reply to this topic.
Boost Ansys Fluent Simulations with AWS
Computational Fluid Dynamics (CFD) helps engineers design products in which the flow of fluid components is a significant challenge. These different use cases often require large complex models to solve on a traditional workstation. Click here to join this event to learn how to leverage Ansys Fluids on the cloud, thanks to Ansys Gateway powered by AWS.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.
- Floating point exception in Fluent
- What are the differences between CFX and Fluent?
- Heat transfer coefficient
- Difference between K-epsilon and K-omega Turbulence Model
- Getting graph and tabular data from result in workbench mechanical
- The solver failed with a non-zero exit code of : 2
- Suppress Fluent to open with GUI while performing in journal file
- Mesh Interfaces in ANSYS FLUENT
- Time Step Size and Courant Number
- error: Received signal SIGSEGV
© 2023 Copyright ANSYS, Inc. All rights reserved.