March 17, 2023 at 8:59 amFAQParticipant
IGNORE = 0 is the default option in contacts with SOFT = 0 or 1. When IGNORE = 0, if an initial penetration is detected, the contact algorithm will move the penetrating node outwards to eliminate the initial penetration. This will perturb the initial geometry, but it will not apply contact forces at time 0. When IGNORE = 1, the initial penetration (d0) is stored as the reference penetration. At each time step, if the current penetration (d) is greater than the reference penetration, the contact force (F) corresponds to the current minus the reference penetration based on the relation F = k * (d – d0) where k is the penalty stiffness. If the current penetration is less than the reference penetration, the reference penetration is updated to the current penetration and no contact force is developed. IGNORE = 2 is the same as IGNORE = 1 but prints warning messages for the penetrations. SOFT = 2 contact is implemented with IGNORE = 1 and also supports IGNORE = 2 to report the initial penetrations. In MORTAR contacts, IGNORE = 2 is the default option, but it has a different meaning from the other contacts. For this option, the initial penetrations are not tracked, but the contact surface is fixed at its initial location. By default, the initial penetrations are given zero contact pressure. An initial contact pressure can be imposed on the interface by setting MPAR1 to the desired contact pressure, when IGNORE = 2. In MORTAR contacts, IGNORE can be also set equal to 3 or 4. For details on these options please see the remark “Overview of Mortar Contact” in Manual Vol I.
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””?”
- How to display the color of each body based on the material in Mechanical?
- After Workbench crashes, how can I recover the project from a .mechdb file?
- How to resolve “Error: Invalid Geometry”?
- How do I request ANSYS Mechanical to use more number of cores for solution?
- Model has a large number of contacts – how to reduce them?
- Please explain the difference between Point Mass and Distributed Mass.