Why does the solver stop with the message “Run duration reached – Maximum simulation time” before the specified Total Time is reached?
Tagged: 2020 R1, cfx, fluid-dynamics, General - CFX
March 17, 2023 at 8:57 amFAQParticipant
This can occur when the timestep size is varying strongly, i.e. from 5[s] to 1e-3[s] from one timestep to the next, close to the Total Time. The reason is that the solver uses a tolerance to check if the total time is reached. This tolerance is by default set to 0.01. That tolerance value is multiplied with the current timestep (i.e. 5[s]) to obtain a dimensional tolerance value (here 0.05[s]). If the Simulation Time is closer than this tolerance to the Total Time , then the solver is stopped. Generally it is not advised to apply such strong changes in the timestep. But if that is required, then the problem can be solved by setting an appropriate tolerance with the following expert parameter: FLOW: EXPERT PARAMETERS: transient maxtime tolerance = 0.01 END END A value of 0.0 is allowed, but it is recommended to use a value such that the dimensional tolerance is smaller than the smallest timestep even for the largest timestep value. In the above example the tolerance should be set to a value smaller than 2e-4, so for example to 1e-4. (1e-4 * 5[s] = 5e-4[s] < 1e-3[s])
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
- ANSYS System Coupling: Two Way Fluid Structure Interaction – Part 1
- ANSYS Polyflow: Adaptive Meshing Based on Contact
- Delete or Deactivate Zone in Fluent
- Apply Custom Material Properties in Fluent
- How can I create a Cell Register from a Cell Zone?
- Check CPU Time in ANSYS FLUENT
- What is meant by Warning: Flow boundary zone 18 is adjacent to a solid zone?
- Aero-Mechanical Simulation of Turbomachinery Blading
- Running Python Script from Workbench
© 2023 Copyright ANSYS, Inc. All rights reserved.