January 25, 2023 at 7:16 amFAQParticipant
Use one of the the following solving strategies: Strategy 1 (robust), works only for subsonic outlet, i.e. the outlet must be downstream of the shock: 1) Create 2 meshes for the Laval nozzle geometry: 1 quite coarse mesh for getting an initial solution and a fine mesh for getting the final solution 2) Apply CFD best practice guidelines to the mesh generation process (quality and density of meshes) to minimize numerical errors 3) Start with the coarse mesh: a) Set the outlet pressure b.c. and the initial pressure to the value of the outlet b.c. pressure. Set initial velocities to nearly zero and initial temperature to the inlet (total) temperature. b) Define a ramp function for the inlet total pressure to ramp up from the value of the outlet pressure to the final desired inlet total pressure value. This ramp function can be written in CEL form as follows: InletPressureRamp = min( (OutletPressure + (InletFinalPressure – OutletPressure) * aitern / RampIterations) , InletFinal Pressure) with “aitern” being the solver variable for the accumulated iteration number and “RampIterations” being the number of time steps until the final inlet pressure should be reached. After the final inlet presssure is reached, the solver continues with a constant (final) inlet pressure. c) Get a converged solution of the flow field on the coarse mesh. 4) Interpolate the coarse mesh results onto the fine mesh. 5) Get the final converged solution of the supersonic flow field on the fine mesh. Strategy 2, works both with sub- and supersonic outlet: 1) Create a coarse mesh, if desired to get initial solution. 2) Define an initial guess that contains different pressure, velocity and temperature values for different sub- and supersonic regions. The values can be either taken from tables on 1-dimensional non-viscous supersonic flows or from the following web link: http://www.aoe.vt.edu/~devenpor/aoe3114/calc.html 3) After getting a converged solution on the coarse mesh, interpolate the solution to the fine mesh and continue the calculation to get the final fine mesh solution.
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
- Delete or Deactivate Zone in Fluent
- ANSYS Polyflow: Adaptive Meshing Based on Contact
- What is meant by Warning: Flow boundary zone 18 is adjacent to a solid zone?
- Aero-Mechanical Simulation of Turbomachinery Blading
- Apply Custom Material Properties in Fluent
- ANSYS System Coupling: Two Way Fluid Structure Interaction – Part 1
- Predict Gearbox Lubrication, Oil Temperature and Churning Losses using CFD Simulation
- Check CPU Time in ANSYS FLUENT
- How to Predict Performance of Bioreactors and Mixing Tanks