Error: divergence detected in AMG solver: pressure correction — what does this mean and how do I fix the problem?
January 25, 2023 at 7:16 amFAQParticipant
This error message is an indication that the “pressure correction” equation is diverging. The most likely cause is that the under-relaxation factor (URF) for that equation is too large. Reduce the URF by 10% and repeat the calculation. Try turning on “AMG verbosity” from the Multigrid Controls panel. Try a setting of verbosity=1. This will display AMG residuals for each equation during the iteration. Setting a value larger than one will report vast quantities of information. During the iteration, you will see the residuals of the multigrid sub-iterations. The default number of sub-iterations is 30. It normally takes under 10 sub-iterations for equations to converge to the default tolerance. However, if a particular equation does not converge, it will “cycle-out,” requiring all 30 iterations, before giving up. This will consume a lot of CPU time and is an indication that the solution is nearly divergent. If this happens, try reducing the URF for that equation, also by 10%. If the sub-iterations diverge, you will get the error message. Another cause, albeit more fundamental, is a problem with the mesh quality. Mathematically, skewed cells induce source terms, which cause the equations to become unstable. You may not be able to resolve this problem without remeshing the domain. As a general rule, please make sure the minimum orthogonal quality for the mesh is 0.01 with an average value that is significantly higher (Fluent 13 or higher), or if you are using Fluent 12.1 or older, the maximum skewness reported in Mesh > Quality is less than 0.93-0.95. Especially important is that you should have low skewness in regions where gradients are large. It is in these regions that errors multiply. A final possible cause of AMG divergence is incorrectly defined boundary conditions. If the grid quality is believed to be good enough and reducing the under-relaxation factors does not work, it is recommended to review all boundary conditions for consistency and correct inputs.
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