How to deal with the following error in WB LS-DYNA? *** Error 30186 (INI+186) the inertia tensor of rigid body # 8 is too small for the accuracy of the computer to handle. Please add mass or increase inertia.
March 17, 2023 at 8:59 amFAQParticipant
The error is stemming from the keycard *CONSTRAINED_NODAL_RIGID_BODY, which is generated for remote points. I have the following comments/questions? 1.Try using mm, t, N as the Unit System in Mechanical. 2.Use the double precision solver: 3.Please make sure that part no. specified in the error is not repeated by opening it is LS-PrePost? 4.Constrained nodal rigid bodies are treated internally in LS-DYNA like a rigid body part, which uses the MAT_RIGID material model. A set of nodes is defined for each nodal rigid body definition with a minimum number of 2 nodes. Nodal rigid bodies with one node are deleted. So, to add a lumped mass or an inertia tensor to a single nodal point, use the respective keyword commands: *ELEMENT_MASS or *ELEMENT_INERTIA. 5.This error will occur if a nodal rigid body’s inertia is sufficiently small to where it could cause numerical instability in the rigid body subroutines. Generally, “too small for the accuracy of the computer” means that when certain quantities are computed using the inertias, (like an inverse), the numbers will result in an NaN. To resolve this issue, the user wouldâ€™ve to investigate whether the rigid body is important to the simulation and if it is important, modify the model in some way to raise the inertia of the rigid body as suggested in the error message. Another option which might work is to set *CONTROL_RIGID, NORBIC=1. As noted in remarks section of this keyword in User’s Manual Vol. I, during initialization, the determinant of the rigid body inertia tensor is checked. If it falls below a tolerance value of 10^âˆ’30, LS-DYNA issues an error message and the calculation stops. In some rare cases (for example with an unfavorable system of units), such tiny values would still be valid. In this case, NORBIC should be set to 1 to circumvent the implied inertia check.
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?
- Contact Definitions in ANSYS Workbench Mechanical
- After Workbench crashes, how can I recover the project from a .mechdb file?
- 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?
- Please explain the warning message “coefficient ratio exceeds 10e8” ?
- How to locate an element of a particular ID number in Mechanical?
- How to Connect Excel to Workbench
- How can I plot bodies colored by material property in Workbench?
© 2023 Copyright ANSYS, Inc. All rights reserved.