In particle tracking in CFX, why can the particle source coefficient affect the solution and not just convergence? I thought that, in CFX, source coefficients only affected convergence.
Tagged: 10, cfxsolver, fluiddynamics, particletracking, postprocessing


March 17, 2023 at 8:58 amFAQParticipant
1. The particle source coefficient affects the accuracy of the track calculation and can therefore change the solution. This can be explained by the fact that particle momentum equation is solved as an ordinary differential equation (ODE). If we take a simple ODE like du/dt = k*u Integrating it with a source coefficient is like solving it by passing the linearised term on the left hand side, ending up solving something like: du/u = kdt which has the solution u=u0 exp (kt) (*) Integrating it without linearising it (or setting the source coefficient to 0) is equivalent to solving the equation by keeping the source term on the right hand side. This way the solution obtained is: u = k*u*t + u0 (**) Now the solution obtained without linearisation (**) is an approximation to the exact solution (*), which will only be accurate when using very small timesteps. One way to test whether the linearisation is appropriate for achieving an accurate solution is to increase the parameter â€˜Number of Integration Steps per Elementâ€™ under SOLVER CONTROL/PARTICLE CONTROL. The default value is 10. If this value is increased to e.g. 100 (this will increase CPU time!) and if the solution doesnâ€™t change much then the linearisation is reasonable. 2. However, for the other models in CFX, it is true that the source coefficients only affect the convergence and not the final 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 HighMounted Stop Lamp (CHMSL)
This video article demonstrates how to create a reflector for a center highmounted 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 KOmega) turbulence model offers a flexible, robust, generalpurpose approach to RANS turbulence modeling. Introducing 2 videos: Part 1Â 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 System Coupling: Two Way Fluid Structure Interaction – Part 1
 Delete or Deactivate Zone in Fluent
 ANSYS Polyflow: Adaptive Meshing Based on Contact
 Apply Custom Material Properties in Fluent
 What is meant by Warning: Flow boundary zone 18 is adjacent to a solid zone?
 AeroMechanical Simulation of Turbomachinery Blading
 Check CPU Time in ANSYS FLUENT
 Running Python Script from Workbench
 How can I create a Cell Register from a Cell Zone?
Â© 2023 Copyright ANSYS, Inc. All rights reserved.