January 25, 2023 at 7:16 amFAQParticipant
The scalability depends on the physics and number of nodes per partition. 1000 nodes per partition is too small for ANSYS CFX. Assuming the physical models allow for good scalability, you can find the following information in the ANSYS CFX Modelling guide: 16.4.1. Optimizing Mesh Partitioning In the ANSYS CFX 17.2 Modelling Guide you will find: Do not run small jobs in parallel For tetrahedral meshes, you may want to use a minimum of 30,000 nodes per partition. For partitions smaller than this, you are unlikely to see any significant performance increase and may even see parallel slow down. For hexahedral meshes, good parallel performance improvements are usually not seen until a minimum of 75,000 nodes per partition is reached. These numbers are machine dependent and can be higher or lower. Dual CPU PCs usually give poorer performance due to lack of bandwidth in the memory bus. Essentially the two CPUs can demand more memory access than the memory bus can provide. Use a sensible number of partitions The partitioning of a mesh leads to the creation of overlap regions at the partition interfaces. These regions are responsible for communication and memory overhead during a parallel run. During partitioning, ANSYS CFX prints partitioning diagnostic information to the CFX-Solver Manager text window and output file about partition overlaps. The percentage of overlap nodes to the total number of mesh nodes should ideally be less than 10% for efficient partitioning. Values greater than 20% will impair performance and are not recommended. Additional comment: Overlap node percentage above 20% maybe ok, if the absolute number of nodes in this domain is small, e.g. you have huge fluid domain and a small solid domain. Radiation and Particle modelling usually do not scale as good. For particle it is very dependent to the particle distribution within the physical domain.
Introducing Ansys Electronics Desktop on Ansys Cloud
The Watch & Learn video article provides an overview of cloud computing from Electronics Desktop and details the product licenses and subscriptions to ANSYS Cloud Service that are...
How to Create a Reflector for a Center High-Mounted Stop Lamp (CHMSL)
This video article demonstrates how to create a reflector for a center high-mounted stop lamp. Optical Part design in Ansys SPEOS enables the design and validation of multiple...
Introducing the GEKO Turbulence Model in Ansys Fluent
The GEKO (GEneralized K-Omega) turbulence model offers a flexible, robust, general-purpose approach to RANS turbulence modeling. Introducing 2 videos: Part 1 provides background information on the model and a...
Postprocessing on Ansys EnSight
This video demonstrates exporting data from Fluent in EnSight Case Gold format, and it reviews the basic postprocessing capabilities of EnSight.
- ANSYS Fluent: Introduction to the GEKO Turbulence Model Part I
- Delete or Deactivate Zone in Fluent
- ANSYS Polyflow: Adaptive Meshing Based on Contact
- What is meant by Warning: Flow boundary zone 18 is adjacent to a solid zone?
- Aero-Mechanical Simulation of Turbomachinery Blading
- Apply Custom Material Properties in Fluent
- ANSYS System Coupling: Two Way Fluid Structure Interaction – Part 1
- Check CPU Time in ANSYS FLUENT
- Predict Gearbox Lubrication, Oil Temperature and Churning Losses using CFD Simulation
- Running Python Script from Workbench