We’re putting the final touches on our new badges platform. Badge issuance remains temporarily paused, but all completions are being recorded and will be fulfilled once the platform is live. Thank you for your patience.
General

General

  1. All Categories
  2. Fluids - General
  3. How to monitor percentage of area with backflow on a certain boundary or internal region, during solver run using Solver Monitor?

How to monitor percentage of area with backflow on a certain boundary or internal region, during solver run using Solver Monitor?

Tagged: ansys-fluent, backflow, percentage area, Solver Monitor
    • June 6, 2022 at 8:32 am
      FAQFAQ
      Participant

      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.

Featured Articles

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.

© 2025 Copyright ANSYS, Inc. All rights reserved.