January 25, 2023 at 7:34 amFAQParticipant
Erosion controls are defined under Analysis Settings. A material element can be eroded (removed) when its geometric strain limit is reached (default 1.5), or when the material in the element fails (default yes), or when the time step controlled by the element reaches a given minimum value (default no). The attached image “analysis_settings.png” shows the typical settings of the erosion controls. The inertia of the eroded material was retained by default, so elements that were eroded away still had their mass continuing to contribute to the results as opposed to just completely removing all traces of the eroded elements because the fragments should still play a part in the outcome predicted. For a typical impact simulation such as a circular cylinder impacting a flat plate, attached three images in pdf file show how the erosion controls affect the outcome of the impact simulation. The first attached image “no_erosion.png” shows the material location plot when all of the erosion controls are set to “No”. You will find that material elements are distorted and the calculation is stopped before the end time is reached due to error messages such as “time step too small” or “degenerate cell”. The second attached image “erosion_mat_failure_yes.png” shows the material location plot when “On Material Failure” is set to “Yes” under erosion controls, where the material elements in failure are eroded away. The calculation runs successfully to the end time. The third attached image “erosion_geom_strain_yes_mat_failure_yes.png” shows the material location plot when both “On Material Failure” and “On Geometric Strain Limit” are set to “Yes” under erosion controls. The “Geometric Strain Limit” is set to much less than the default value. You will find that both the material elements in failure and the material elements that reach the specified geometric strain limit (may not fail yet) are eroded away. Since some material elements that have not failed are eroded away by geometric strain limit, please be aware that material strength will be under-estimated. Thus it is not advisable to use very small geometric strain limit for erosion.
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.
- The warning message is: “The maximum contact stiffness is too big. This may affect the accuracy of the results.” Why does large contact stiffness affect results accuracy?
- Contact Definitions in ANSYS Workbench Mechanical
- After Workbench crashes, how can I recover the project from a .mechdb file?
- Model has a large number of contacts – how to reduce them?
- How to resolve “Error: Invalid Geometry”?
- How to deal with “”Problem terminated — energy error too large””?”
- How to display the color of each body based on the material in Mechanical?
- The LS-DYNA equivalent of *MODEL_CHANGE card (in ABAQUS). Which keywords can be used to introduce(activate)/delete(deactivate) elements in the middle of a calculation (at user-specific time/load steps).
- How to locate an element of a particular ID number in Mechanical?
- Please explain the warning message “coefficient ratio exceeds 10e8” ?
© 2023 Copyright ANSYS, Inc. All rights reserved.