Free Courses Fluids Structures Electronics 3D Design Optics Photonics Materials Installation Python Optimization Safety & Cybersecurity Embedded Software MBSE Digital Mission Engineering STEM NVH Student Teams Semiconductors Indo Kursus Partner Courses My Courses

[FAQ]

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.