How to monitor percentage of area with backflow on a certain boundary or internal region, during solver run using Solver Monitor?
June 6, 2022 at 8:32 amFAQParticipant
Follow these steps:
1)Use for mesh regions or boundaries normal to one of the X, Y or Z axes.
2)Define expressions and one additional variable to get information on the percentage of area of that region or boundary with backflow. Expressions: (example here: BOUNDARY normal to global Z axis) Backflow = areaInt(AV Backflow Step)@BOUNDARY / area()@BOUNDARY Backflow Step = 1 – step(Velocity w / 1[m/s])
3) Additional Variable: LIBRARY: ADDITIONAL VARIABLE: AV Backflow Step Option = Definition Tensor Type = SCALAR Units =  Variable Type = Unspecified END END
4)Setting for “AV Backflow Step” in all Domains, under “FLUID MODELS”: ADDITIONAL VARIABLE: AV Backflow Step Additional Variable Value = Backflow Step Option = Algebraic Equation END
5)Monitor the expression “Backflow” in Solver Manager to get percentage of area of BOUNDARY, where backflow into the negative Z direction occurs. Value will be between 0 and 1.
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.
- How can I create a Cell Register from a Cell Zone?
- Left-handed faces troubleshooting
- How to overcome the model information incompatible with incoming mesh error?
- ANSYS Fluent: Introduction to the GEKO Turbulence Model Part I
- Delete or Deactivate Zone in Fluent
- ANSYS System Coupling: Two Way Fluid Structure Interaction – Part 1
- How to create and execute a FLUENT journal file?
- Running Python Script from Workbench
- What are the requirements for an axisymmetric analysis?
- How to export plots automatically during a Fluent simulation using execute commands?