June 5, 2023 at 7:04 amFAQParticipant
The contact stiffness is not affected by the time step size, when SOFT=0 (*CONTACT, Optional Card A). It can be affected, if SOFT=1 and it is affected when SOFT=2 is set. When SOFT=1, contact stiffness is calculated as follows: k = max[SLSFAC*SFS*k0, SOFSCL*k1] where k is the penalty stiffness SLSFAC is user input on *CONTROL_CONTACT SFS is user input on *CONTACT (Card 3) SOFSCL is user input on *CONTACT (Optional Card A) k0 is the stiffness calculated from material bulk modulus and element dimensions. This is the stiffness used when SOFT=0 (see Section 23.7 in the LS-DYNA Theory Manual). k1 is the stiffness calculated from nodal masses and the solution time step (analogous to how Courant time step is determined based on mass and stiffness). k1 is proportional to 1/(time step)^2. Thus, if the time step is cut in half, the contact stiffness increases by a factor of 4. When SOFT=2, contact stiffness is calculated in similar fashion to k1 above and can be scaled by SLSFAC and by SFS. So again, the contact stiffness is proportional to 1/(time step)^2. Time step can affect contact behavior aside from contact stiffness. The bucket sorting interval is based on a number of time steps. Thus, if the time step is reduced, there will be less time between bucket sorts. Also, the incremental penetrations will likely be smaller if the time step is reduced.
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?