Tagged: ls-dyna, LS-DYNA Suite, lsdyna, structural-mechanics
March 17, 2023 at 8:59 amFAQParticipant
In certain cases components are intentionally designed with initial interference so that they do not fit with each other. These parts are shrink fitted together to develop a prestress. In LS-DYNA, there are two types of contact that can be used to resolve the interference between the components and consequently generate the desired level of initial stress, the INTERFERENCE contact, and the MORTAR contact. The contact is defined between the two initially interfering parts in the unstressed configuration. The INTERFERENCE contact is defined by either of: *CONTACT_NODES_TO_SURFACE_INTERFERENCE, *CONTACT_ONE_WAY_SURFACE_TO_SURFACE_INTERFACE, or *CONTACT_SURFACE_TO_SURFACE_INTERFERENCE. This option turns off the nodal interpenetration checks at the start of the simulation and allows the contact forces to develop to remove the interference. The load curves LCID1 and LCID2 specified in the mandatory Card 4 scale the interface penalty stiffness such that the stiffness can gradually increase from zero to the final value with respect to the time. As a result, the contact forces also increase gradually to remove the overlap and generate the initial stresses in the bodies. Usually, the INTERFERENCE contact is combined with dynamic relaxation. In that case, LCID1 defines the stiffness scale factor with respect to the time in the dynamic relaxation phase. The curve must originate at (0,0) at time 0 and gradually increase typically to an ordinate of 1. The duration of the ramp should be selected such that it does not exceed the duration of the dynamic relaxation. Curve LCID2 scales the contact stiffness during the transient phase. If this follows a dynamic relaxation phase, the curve has typically a constant value of unity for the duration of the analysis. For the INTERFERENCE contacts, the orientation of the segments is important. The outward normal vector of the segments of the one contact surface should point towards the opposing contact surface after the interference is resolved. Finally, it is important to note that the INTEREFERENCE contact is limited to reasonably small initial penetrations. The threshold of the initial penetrations needs to be comparable to the length of the element side. Otherwise, this contact type should be avoided. The MORTAR contact resolves the initial interferences when IGNORE is set equal to 3 or 4. Typically, *CONTACT_AUTOMATIC_SURFACE_TO_SURFACE_MORTAR is used. IGNORE=3 should be used only for relatively small penetrations that are comparable to the element depth. The penetrations are resolved between time zero and the time given by DPRFAC (also termed MPAR1). IGNORE=4 is recommended for larger penetrations (several elements deep). The field DTSTIF (also termed MPAR2) should be equal to the order of the maximum initial penetration; otherwise, an error termination will be the result. This parameter helps the contact algorithm to locate the contact surface for arbitrary initial penetration depths. MPAR1 is specified as in IGNORE=3. When the interference is deep, it is recommended to use *SET_SEGMENT to define the contact surfaces. Note that IGNORE=3 or 4 is not supported in dynamic relaxation.
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?
- After Workbench crashes, how can I recover the project from a .mechdb file?
- Contact Definitions in ANSYS Workbench Mechanical
- Model has a large number of contacts – how to reduce them?
- How to resolve “Error: Invalid Geometry”?
- How to display the color of each body based on the material in Mechanical?
- How to locate an element of a particular ID number in Mechanical?
- Please explain the warning message “coefficient ratio exceeds 10e8” ?
- How to Connect Excel to Workbench
- How can I plot bodies colored by material property in Workbench?
© 2023 Copyright ANSYS, Inc. All rights reserved.