November 3, 2020 at 2:56 pmSamir KadamAnsys EmployeeHow to plot the strain energy in modal analysis?n
November 3, 2020 at 3:12 pmpeteroznewmanSubscriberWhy do you want to plot strain energy in a modal analysis? nIn my experience, only the modal frequency, mode shape (normalized by mass or displacement) and the participation factor summary are important. Maybe others will comment.n
November 4, 2020 at 2:50 pmRahul KumbharAnsys Employeeto plot the strain energy results in modal analysis, use following commands:n/sho,pngnset,1,1 ! reads in mode 1 datanplns,send,elasticnset,1,2 ! reads in mode 2 datanplns,send,elasticnnAlso, one may use:netab,sene,senenpletab,senen
December 11, 2020 at 8:23 pmshkieferSubscriberYou can create a User Defined Result and enter ENERGYPOTENTIAL for the expression to get a plot of continuum element strain energy. You need to have had energy and possibly stress as selected outputs in output control.nIn my experience the plots of element strain energy are less insightful than total relative contribution of individual regions / components. The magnitudes mean nothing in a modal analysis but the relative proportion can tell you what components / regions are contributing the most for each mode. nFor example if you had 3 components then for each mode you could sum all strain energy for each component and divide by the sum of the entire model. The mode will be most sensitive to the stiffness of the component with the highest percentage of strain energy. If they are all approx. the same then you will need to change all of them to move the frequency much. Frequency scales with the square root of stiffness so it take pretty significant changes to move the needle.nSee this Medium post for some other information:n
December 12, 2020 at 12:20 pmpeteroznewmanSubscriberGreat article!nIn my experience the plots of element strain energy are less insightful than total relative contribution of individual regions / components. The magnitudes mean nothing in a modal analysis but the relative proportion can tell you what components / regions are contributing the most for each mode.nCoincidentally, later in November 2020, I was taught exactly what you said in the quote above and describe in detail in your article. Thanks for the post!n
- You must be logged in to reply to this topic.
Simulation World 2022
Check out more than 70 different sessions now available on demand. Get inspired as you hear from visionary companies, leading researchers and educators from around the globe on a variety of topics from life-saving improvements in healthcare, to bold new realities of space travel. Take a leap of certainty and check out a session today here.
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.
- How to calculate the residual stress on a coating by Vickers indentation?
- An Unknown error occurred during solution. Check the Solver Output…..
- Saving & sharing of Working project files in .wbpz format
- Solver Pivot Warning in Beam Element Model
- Understanding Force Convergence Solution Output
- whether have the difference between using contact and target bodies
- Colors and Mesh Display
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- Massive amount of memory (RAM) required for solve
- What is the difference between bonded contact region and fixed joint
© 2022 Copyright ANSYS, Inc. All rights reserved.