Tagged: lsdyna, LSDYNA Suite, lsdyna, R13.x, structuralmechanics


March 17, 2023 at 8:59 amFAQParticipant
Eigenvalue analysis is performed by selecting IMFLAG=1 on *CONTROL_IMPLICIT_GENERAL and specifying a nonzero value for NEIG on *CONTROL_IMPLICIT_EIGENVALUE. If NEIG>0, the lowest NEIG eigenvalues will be computed at time 0 and LSDYNA will terminate. If NEIG<0, intermittent eigenvalue analyses will be performed to compute the modelÃ¢â‚¬â„¢s eigenvalues at specified times during the analysis. A detailed description of NEIG<0 can be found in the Manual Vol I. When an eigenvalue analysis is performed the eigenvectors are written by default to the binary database d3eigv. This can be viewed in LSPrePost in the same way as the d3plot database. The database d3eigv contains NEIG states with each state corresponding to the computed eigenvector (mode shape) at an eigenfrequency. The mode shape displacement at a node can be accessed through history plot. The horizontal axis of the plot corresponds to the eigenfrequency which is given in units of cycles per unit time. Tables with the eigenvalues, modal participation factors, modal effective mass are written in the ascii file eigout by default. Eigenvalues and eigenvectors can be also written to the file Eigen_Vectors by using a nonzero value for EVDUMP on *CONTROL_IMPLICIT_EIGENVALUE. This feature is available only in SMP. If EVDUMP>0, an ascii file is used, while if EVDUMP>0, a simple binary format is used. When the ascii file is used, the file is organized as follows. The first line shows the number of eigenvalues extracted (NEIG). The second line shows the number of the independent degrees of freedom. The first NEIG entries starting from line 3 show the computed eigenvalues (omega^2). The remaining lines show the nodal displacements and rotations of each eigenvector starting from the one with the lowest eigenvalue. For each eigenvector the degrees of freedom are read rowwise starting from degree of freedom 1. The eigenvectors are orthonormalized to the mass matrix. This is different than the scaling used in LSPrePost. The mass matrix is written in an ascii file when MTXDMP>0 in *CONTROL_IMPLICIT_SOLVER. The numbering of the degrees of freedom can be found in the ascii file Node_Data_xxxx_yyy when MTXDUMP>0. The file lists the independent degrees of freedom at each node with the zero entries corresponding to the constrained degrees of freedom. If the model has rigid bodies, their IDÃ¢â‚¬â„¢s and corresponding degrees of freedom are listed after those of the final node. The degrees of freedom assigned to the rigid bodies correspond to the center of mass. After the list of the rigid bodies, the file shows the coordinates of each node, and then the coordinates of the center of mass of each rigid body.

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 HighMounted Stop Lamp (CHMSL)
This video article demonstrates how to create a reflector for a center highmounted 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 KOmega) turbulence model offers a flexible, robust, generalpurpose approach to RANS turbulence modeling. Introducing 2 videos: Part 1Â 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 LSDYNA 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 userspecific 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?
Â© 2023 Copyright ANSYS, Inc. All rights reserved.