I computed the species mass fraction in a setup where the convective velocity at the inlets/outlets is negligible, that is, the species transport over inlets and outlets is diffusion dominated. I activated the Inlet Diffusion option in the Species Model dialog box and the species mass fraction is computed correctly. However, the mass fraction gradient shows considerable over- and undershoots at the inlet and outlet boundaries. What is the reason and how can I correct this?
January 25, 2023 at 7:17 amFAQParticipant
The over-/undershoots in the gradient of the mass fraction are due to use of cell averaged values for computing the gradients in the boundary cells (Least-Squares or Green-Gauss cell-based gradient reconstruction schemes) and should not occur with a node-based scheme. In the default Least-Squares gradient reconstruction formulation, the cell center values are used for computing the cell gradients adjacent to the inlet/outlet boundaries. In order to resolve this issue, you need to change the default Least-Squares-gradient correction be setting the value of recon/cell-lsq/cortype to 2: (rpsetvar ‘ recon/cell-lsq/cortype 2) More information regarding the Least-Squares gradient correction options: There are three gradient correction options available in ANSYS Fluent for correcting the Least-Squares gradients at the boundaries which are controlled by recon/cell-lsq/cortype. One can set the value of this rpvar to 0,1(default), or 2. Here 0 means that the solver will zero out the gradients at the boundary face, 1 means that solver will zero out the normal gradient at the boundary faces, and 2 means that the boundary values are extrapolated implicitly at the boundaries faces. In general, the default value is recommended for most of the applications as it was tested vastly and was found to be fairly accurate and robust, but the setting can be changed when the obtained solutions are not satisfactory.
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.
- I am running an electrochemistry simulation in Fluent. How can I access the electrochemistry reaction rates with UDF?
- How do I model humidity in Fluent?
- ANSYS Internal Combustion Engine (ICE): Port Flow Part 1 – Getting Started
- LES Simulation of Turbulent Flames Using ANSYS Fluent
- How can volume fraction be plotted in a species transport simulation?
- ANSYS Fluent: Describing Non-premixed Combustion using the Steady Flamelet Model
- What is a DASAC failure and how can I correct it?
- Error “…Cannot find thermo database file …Reverting to default…” while reading PDF Table. How to link a specific thermodynamic database file to a case?
- ANSYS Internal Combustion Engine (ICE): Engine Sector Combustion Part 6 Results
- ANSYS Internal Combustion Engine: (ICE) Engine Sector Combustion Part 1 Getting Started