January 25, 2023 at 7:16 amFAQParticipant
Pressure-based and density-based solvers differ in the way how the continuity, momentum, and energy and species equations are solved. Pressure-based technology solves the pressure equation to conserve mass, and can be used in any flow simulation except with the following features: non-reflecting boundary conditions, and wet steam multiphase model. Two algorithms exist under pressure based solver: segregated and coupled. With pressure based segregated solver the governing equations are solved sequentially, while with the coupled solver continuity and momentum are solved in a coupled manner. Density-based (explicit or implicit formulations) algorithm solves the continuity equation along with momentum, energy and species transport as a coupled set of equations. Additional equations (for example turbulence or radiation) are solved sequentially. This solver is not available for cavitation model, VOF model, multiphase mixture model, Eulerian multiphase model, non-premixed combustion model, premixed combustion model, partially premixed combustion model, composition PDF transport model, Soot model, Rosseland radiation model, melting/solidification model, shell conduction model, floating operating pressure, fixed variable option, physical velocity formulation for porous media, relative velocity formulation, and specified mass flow rate for streamwise periodic flow. Generally speaking pressure-based solver is traditionally for incompressible or low compressible flows, however pressure based coupled solver can handle moderate compressible flows. The density based solver is mainly recommended for high speed compressible flows. The model availability in Fluent, solver performance and mesh size (coupled solvers will require more memory on large meshes) are three criteria to select the correct solver. For more information open ANSYS Help Viewer click on the Go To Page icon and enter the command help/flu_ug/flu_ug_sec_solve_using_overview.html in the pop-up window then click on Go.
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
- Aero-Mechanical Simulation of Turbomachinery Blading
- What is meant by Warning: Flow boundary zone 18 is adjacent to a solid zone?
- 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