Why does the prestress from Static analysis does not add up to the stress in Random Vibration analys
September 16, 2020 at 5:53 pmHuiLiuAnsys EmployeePSD stresses are statistical and reported as standard deviations from a zero mean (always positive numbers). These stresses take into account stiffening effects of a pre-stress analysis, but are themselves simply statistical deviations from a zero mean.nOn a component-by-component basis you can add or subtract PSD stress values to component values from your pre-stress to find the 'worst case' 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.nYou 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:nThe default output from a Random Vibration analysis will be 1-sigma values (i.e., standard deviations about a zero mean). Therefore, we have a Gaussian distribution of stress at each node. If you have pre-stressed 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.nYou could add/subtract the 1-sigma 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 1-sigma 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:nRight 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.nnRepeat this process for the Static resultnAdd and subtract appropriately to get the min/max values in ExcelnSave separate Text files with the Node locations and Min/Max valuesnRead in the Text Files using External Data in ANSYS Workbench. Make sure to specify the appropriate column data, especially Stress (and units!)nLink the External Data cell to the Setup of a duplicate Static StructuralnRight Click on the Imported Load folder in ANSYS Mechanical and specify 'Initial Stress'nSpecify 'Apply To' > Corner Nodes and 'Component' > Desired ComponentnANSYS 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.n
September 23, 2020 at 2:53 amKRAdministratorThank you, for sharing this tip.nKarthikn
September 23, 2020 at 12:36 pmMTBXCSubscriberRecently, I did such an analysis -> Static + Prestress-> Modal-> Random Vibration. You have increased my knowledge of it. Thank younnMichaln
- The topic ‘Why does the prestress from Static analysis does not add up to the stress in Random Vibration analys’ is closed to new replies.
Boost Ansys Fluent Simulations with AWS
Computational Fluid Dynamics (CFD) helps engineers design products in which the flow of fluid components is a significant challenge. These different use cases often require large complex models to solve on a traditional workstation. Click here to join this event to learn how to leverage Ansys Fluids on the cloud, thanks to Ansys Gateway powered by AWS.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.
- Solver Pivot Warning in Beam Element Model
- Saving & sharing of Working project files in .wbpz format
- Understanding Force Convergence Solution Output
- User manual
- An Unknown error occurred during solution. Check the Solver Output…..
- What is the difference between bonded contact region and fixed joint
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- whether have the difference between using contact and target bodies
- Defining rigid body and contact
- Colors and Mesh Display
© 2023 Copyright ANSYS, Inc. All rights reserved.