How to evaluate the difference of a local variable to its circumferential averaged value on a Turbo Surface?
Tagged: 11, cfd-post, fluid-dynamics, General, rotating-machinery
March 17, 2023 at 8:58 amFAQParticipant
This can be achieved with the following steps: â€¢ Initialize the turbo components â€¢ Generate a Turbo Surface: Location > Turbo Surface â€¢ Define the Turbo Surface as required, e.g.: o Geometry > Method > Constant Streamwise Location o Color – Variable: Velocity – Circ Average: Length – Max Samples: 100 o Apply â€¢ When you click on â€œâ€¦â€ a new variable named â€œVelocity LCA on Turbo Surface 1â€ occurs * â€¢ Create an Expression: Insert > Expression > exp1 = Velocity – Velocity LCA on Turbo Surface 1 > Apply â€¢ Create a Variable: Insert > Variable > var1 > Expression: exp1 > Apply â€¢ Go to the Turbo Surface again o Variable: var1 o Circ Average: None o Apply The difference is now displayed on the turbo surface. * The abbreviation LCA means circumferentail averaging by length: When the Circ. Average setting is set to Length, circumferential averaging of values at a sampling point is carried out internally by forming a circular arc, centered about the turbo axis, passing through the sampling point. Values are interpolated to n equally-spaced locations along the arc, using values from nearby nodes, where n is a number that is inversely proportional to the mesh length scale, and limited by the Max. Samples setting. The n values are then averaged in order to obtain a single, circumferentially-averaged value for the sampling point.
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
- Delete or Deactivate Zone in Fluent
- ANSYS Polyflow: Adaptive Meshing Based on Contact
- Apply Custom Material Properties in Fluent
- What is meant by Warning: Flow boundary zone 18 is adjacent to a solid zone?
- Aero-Mechanical Simulation of Turbomachinery Blading
- Check CPU Time in ANSYS FLUENT
- Running Python Script from Workbench
- How can I create a Cell Register from a Cell Zone?
© 2023 Copyright ANSYS, Inc. All rights reserved.