What are the suggested steps if I am having convergence issues for conjugate heat transfer problems?
January 25, 2023 at 7:16 amFAQParticipant
Suggested solutions if you run into convergence issues: 1) Make sure that the grid at the interface is not too dissimilar. 2) Grid should ideally be very fine at the wall becoming coarser away from the wall 3) Ensure good grid quality by checking equiangle skew and aspect ratio etc. 4) First obtain converged solution using flow equations only, then solve the flow and energy equations simultaneously 5) Obtain converged first order solution first and then switch to second order solution 6) Use velocity inlet instead of pressure inlet BC. 7) Lower the energy under-relaxation factor. Try 0.98 (don not go lower than 0.95) 8) Use Pressure-based solver with coupled option, lower the Courant number. 9) In Define-> Model-> Solver, select ‘node-based’ for gradient option. 10) If using tetrahedral grid, turn off secondary gradients using the following TUI command: (rpsetvar ‘temperature/secondary-gradient? #f) 11) Change multigrid settings (solve->controls->multigrid) for energy. Set it to W cycle with a termination criteria of 0.01 (or smaller) 12) Increase the upper limits of pressure and temperature in Solve-> Controls->Limits
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 Polyflow: Adaptive Meshing Based on Contact
- Delete or Deactivate Zone in Fluent
- Apply Custom Material Properties in Fluent
- Aero-Mechanical Simulation of Turbomachinery Blading
- What is meant by Warning: Flow boundary zone 18 is adjacent to a solid zone?
- 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