March 17, 2023 at 9:00 amFAQParticipant
NLAD resolves the convergence issue without any remesh because the code automatically removes â€œETCON,setâ€ from the ds.dat file when NLAD is activated. You can read more about this command here: https://ansyshelp.ansys.com/account/Secured?returnurl=/Views/Secured/corp/v192/ans_cmd/Hlp_C_ETCONTROL.html This basically turns off enhanced strain formulation. This is the same as setting Element Control to â€œManualâ€ under Geometry branch in WB-Mechanical. Because of this, in some cases, one might observe convergence with the B-Bar formulation(KEYO,,1,0), but not with the default enhanced strain (KEYO,,1,2) formulation. It has nothing to do with NLAD actually. Please note that, even when there is an addition of a command snippet such as â€˜keyo,1,1,0â€™ (which changes the element formulation for plane 182 element) located under the geometry branch it would still not resolve the issue. The reason is that as long as â€˜ETCON,setâ€™ has been executed, it will override any previously set KEYOPT settings. So the prescribed command object is being ignored. This explanation is actually found in the ETCONTROL command manual for â€˜ETCONTROLâ€™: â€œThe program informs you of the best settings and resets any applicable KEYOPT settings automatically. This action overrides any previous manual settings.â€ Keywords: NLAD, Element Formulation, Remeshing
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?