The default 0.1 numerical damping value used in transient analysis must have a reason. Is there any test correlation to validate the damping values? Or it’s just a random number the program picks?
January 25, 2023 at 7:34 amFAQParticipant
Numerical damping, it is numerical – not physical – so it’s not related to test correlation. Please see Section 5.6.3 “Transient Dynamic Analysis Settings Based on Application” below: https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v192/ans_str/Hlp_G_STR5_12.html There, one will see different defaults. MAPDL actually defaults to gamma=0.005 while Mechanical defaults to gamma=0.1. The setting for Mechanical is the same as “Moderate Speed Simulation” case. To provide some background, when we have transient structural analyses, we can often get additional ‘noise’ – for example, spurious high-frequency content can be excited. Models may not be set up ‘perfectly’ by the user (not through any fault of the user, but to get an efficient solution, there may be some modeling short-cuts taken, such as using a coarse mesh). Using numerical damping can reduce such ‘noise’. It can also have a different effect – faster convergence. These benefits come at the expense of some numerical dissipation (larger numerical damping means larger numerical dissipation). The defaults in Mechanical of gamma=0.1 are a tradeoff between these effects (pros and cons) for structural simulations. Note that for purely acoustic simulations, it’s a bit different – we don’t have contact/impact in purely acoustic simulations, and everything is always linear. Thus, using no numerical damping (no numerical dissipation) is probably desired for this situation Albert has where amplitude is lower than expected. In short, numerical damping comes about mainly for structural analyses, and defaults are with structural analyses in mind. For purely acoustic simulations, numerical damping can add unwanted numerical dissipation, so user may wish to set it to zero.
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 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).
- 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
- How to deal with “”Problem terminated — energy error too large””?”
- After Workbench crashes, how can I recover the project from a .mechdb file?
- How to display the color of each body based on the material in Mechanical?
- How to resolve “Error: Invalid Geometry”?
- Model has a large number of contacts – how to reduce them?
- Please explain the difference between Point Mass and Distributed Mass.
- How to locate an element of a particular ID number in Mechanical?