In ANSYS nCode DesignLife is it possible to do a fatigue analysis for a Sine-On-Random vibration loading?
January 25, 2023 at 7:34 amFAQParticipant
Yes. To do a sine-on-random vibration fatigue evaluation in DesignLife, you need to convert the sine signal and random vibration spectrum to a combined time-history loading. You then need to run a mode-sup transient analysis using that time history loading (you need to save the modal stresses and the .mcf file). You then need to run a Time Series SN analysis using that time history. The steps are summarized below: 1. Open DesignLife 2. Drag TSGenerator Glyph (from Input Palette) onto Workspace 3. Open Properties for TSGenerator Glyph a. Set Operation to be “SineOnRandom” b. Enter data for PSD spectra and sinusoidal loading (note: this glyph will the convert PSD and sinusoidal input into time history loading) 4. Drag TS_to_FE_Table Glyph (from DL Palette) onto Workspace and connect its input to an output from the TSGenerator 5. Open Properties for TStoFETable and Set Program to “ANSYS” (note: this glyph will convert the time history loading generated by TSGenerator into loading versus time table for use in the FE. It will be stored in xml file that can be imported into ANSYS Mechanical to be used as tabular force input for a mode-supe, time-history analysis) 6. Run DL to create time the Time Series loading (note: XYDisplay and DataValueDisplay glyphs can be connected to TSGenerator to view the created time history loading) 7. Exit DL 8. Open Workbench and set-up mode-supe transient analysis (note: DL needs the modal stresses from the modal analysis and the mode coefficients from the transient analysis) 9. In the modal analysis: save only the stress 10. In the transient analysis a. do not save anything (Mechanical will always store DOF results, but they are not needed b. issue TRNOPT,MSUP,,,,YES from within a Command Object to store mode coefficients in a file.mcf file c. import the time history loading from the XML file previously generated as a table load for the appropriate force 11. Solve Mechanical 12. On WB project schematic, connect SN TimeSeries system to the Solution cell of the modal system and the Engineering Data cell of the transient system 13. Within DL: a. delete the TSInput Glyph b. drag a Modal Coord Input Glyph (from DL palette) onto the workspace c. connect Modal Coord Input Glyph to SNAnalysis Glyph d. From Available Data: i. drag modal stress results file (file.rst) onto FEInput Glyph ii. drag modal coordinates file (file.mcf) onto Modal Coord Input Glyph 14. Run DL analysis and post-process
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 deal with “”Problem terminated — energy error too large””?”
- How to display the color of each body based on the material in Mechanical?
- 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).
- How to locate an element of a particular ID number in Mechanical?
- Please explain the warning message “coefficient ratio exceeds 10e8” ?
© 2023 Copyright ANSYS, Inc. All rights reserved.