Why does the prestress from Static analysis does not add up to the stress in Random Vibration analysis?
Tagged: 18.1, General, mechanical, structuralmechanics


January 25, 2023 at 7:34 amFAQParticipant
PSD stresses are statistical and reported as standard deviations from a zero mean (always positive numbers). These stresses take into account stiffening effects of a prestress analysis, but are themselves simply statistical deviations from a zero mean. On a componentbycomponent basis you can add or subtract PSD stress values to component values from your prestress to find the â€˜worst caseâ€™ max/min stress that can occur in that component. This can be thought of as rigidly shifting the stress distribution reported by the PSD run away from its zero mean. You cannot simply use the Von Mises Equivalent Stress equation to calculate PSD equivalent stresses, as that algebraic equation is not mathematically suited for statistical values. If you want to Superpose Random Vibe Stress with Static Structural then there are a couple of points for your consideration on this issue: The default output from a Random Vibration analysis will be 1sigma values (i.e., standard deviations about a zero mean). Therefore, we have a Gaussian distribution of stress at each node. If you have prestressed the modal analysis, then the effect of the static loading is accounted for in the stiffness that is used to determine the natural frequencies. This consequently filters down into the PSD analysis. You could add/subtract the 1sigma component value (i.e., Normal Stress in X, Y, and Z) at each node to/from the static analysis to get a sense for the 1sigma variation of the component stresses about that mean value. This would be the same as rigidly shifting the Gaussian distribution from zero mean to be centered about the static condition. There will not be a way to directly plot contours like this in ANSYS Mechanical. However, I can think of one possible workaround: Right Click on the PSD result and select Export. This will give you a text file containing stress at each node. It will also contain the X, Y, and Z coordinates of the nodes if you have specified this on Tools > Options > Mechanical > Export > Include Node Location. Repeat this process for the Static result Add and subtract appropriately to get the min/max values in Excel Save separate Text files with the Node locations and Min/Max values Read in the Text Files using External Data in ANSYS Workbench. Make sure to specify the appropriate column data, especially Stress (and units!) Link the External Data cell to the Setup of a duplicate Static Structural Right Click on the Imported Load folder in ANSYS Mechanical and specify â€˜Initial Stressâ€™ Specify â€˜Apply Toâ€™ > Corner Nodes and â€˜Componentâ€™ > Desired Component ANSYS Mechanical will then try to map the stress to the duplicated mesh. The result should be an Imported Initial Stress that really is the combination of your static and PSD results.

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.
 How to deal with “”Problem terminated — energy error too large””?”
 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).
 Contact Definitions in ANSYS Workbench Mechanical
 How do I request ANSYS Mechanical to use more number of cores for solution?
 There is a unit systems mismatch between the environments involved in the solution.
 After Workbench crashes, how can I recover the project from a .mechdb file?
 How to restore the corrupted project in ANSYS Workbench?
 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.
Â© 2024 Copyright ANSYS, Inc. All rights reserved.