Tagged: 2020 R2, fluent, fluid-dynamics, General, General - FLUENT
March 17, 2023 at 8:59 amFAQParticipant
1. Start with converged steady-state solution when applicable (when the initial transient solution is not important). 2. You could use either SIMPLEC (will be fastest if holds together) or coupled solver. Alternatively, depending on the simulation, you could start with SIMPLEC and then switch to the coupled solver. 3. All Under Relaxation Factors are to be kept at 1 ( or close to 1 provided stability is achieved). 4. Courant = infinity (1e+06) in pressure based coupled solver (which is no relaxation). 5. dt is chosen such as to maintain convective CFL =1 (this value can be reported under velocity) and acoustic CFL =1 (if solving for acoustics). 6. No more than 10 iterations / time step. More than that are not needed if CFL ~1. 7. You could “ignore” the residuals as long as they drop per time step. Dropping of residuals to 3 orders of magnitude is not absolutely necessary, especially continuity. 8. In transient solution, residuals do not represent converged solution. Flow variables are not converged during sub iterations, what is updated during sub iterative cycle is flux values which come from the previous step and then are updated using the flow variables at the current step. However, to monitor convergence, you could use the variable of interest and monitor the variation as the simulation progresses.
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
- ANSYS System Coupling: Two Way Fluid Structure Interaction – Part 1
- ANSYS Polyflow: Adaptive Meshing Based on Contact
- Delete or Deactivate Zone in Fluent
- Apply Custom Material Properties in Fluent
- How can I create a Cell Register from a Cell Zone?
- Check CPU Time in ANSYS FLUENT
- What is meant by Warning: Flow boundary zone 18 is adjacent to a solid zone?
- Aero-Mechanical Simulation of Turbomachinery Blading
- Running Python Script from Workbench
© 2023 Copyright ANSYS, Inc. All rights reserved.