January 25, 2023 at 7:16 amFAQParticipant
Yes, the dynamic mesh feature can be used in steady state applications to perform a parametric study of different object/boundary positions in the fluid flow. Typical applications include check valves, steady state FSI etc, often to calculate the object equilibrium positions. The primary advantage of using steady state dynamic mesh feature is that it will eliminate the repeated time-intensive mesh generation process for the series of intended runs. When creating the base mesh the user should have the same topological and meshing considerations as for a transient run. Set up is similar to a transient case set up. First define the dynamic mesh parameters, Define -> Dynamic Mesh -> Parameters (note that In-Cylinder and Six DOF Solver are incompatible with steady state solver). A DEFINE_CG_MOTION or DEFINE_GRID_MOTION user function is required to move the object (note that motion profiles are incompatible with steady state solver). The mesh will have to be manually updated using Solve -> Mesh Motion feature (or using the TUI command /Solve/mesh-motion). However, this process can be automated for a series of object positions using journal files and/or execute commands. It is important to remember that a default time step of 1 s will be used to update the mesh and so the user will have to set an appropriate velocity in user functions to achieve the desired object movement.
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
- What is meant by Warning: Flow boundary zone 18 is adjacent to a solid zone?
- Apply Custom Material Properties in Fluent
- Aero-Mechanical Simulation of Turbomachinery Blading
- 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