I specified the number of modes to be extracted in a modal analysis using the unsymmetic solver but a lower number of modes are calculated. Also aplpies to the DAMP solver. Why are less modes calculated?


April 5, 2023 at 2:33 pmFAQParticipant
Both the UNSYM and DAMP eigensolvers may not calculate as many modes as requested The details on the UNSYM (and DAMP) eigensolvers can be found here: https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v192/ans_thry/thy_tool13.html The key point is the following: For a large number of eigenvalues, the UNSYM extraction algorithm is able to move automatically to a new shift if the first solve only finds a subset of eigensolutions. This process will be repeated until all the required eigenvalues are found, unless the algorithm fails several times to find any accurate eigenvalues. The shift is needed to get the higher frequency modes, but it will stop if it can no longer get accurate modes, as described above. Itâ€™s also worth noting that Sturm sequence checks canâ€™t be performed for UNSYM or DAMP: https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v192/ans_str/Hlp_G_STR3_15.html%23ajgQxq322mcm Thus, we mention that there may be missing modes at higher frequencies â€“ this is a bit of digression but worth noting since the user is extracting a lot of modes. There isnâ€™t a good workaround or solution to this since itâ€™s a limitation of the eigensolvers. I have two suggestions: If the user is doing a downstream harmonic analysis, solving with full method (rather than modesuperposition) is preferred If the user is not doing a downstream msup analysis but just wants to get the frequencies (modal analysis is last analysis type needed), then they can run multiple modal analyses with different shift points. For example, they can extract 100 modes between frequency A and frequency B, then they can extract 100 modes from frequency B to frequency C (you probably donâ€™t want to end/begin at the exact same frequency B but have some overlap). Extracting smaller numbers of frequencies within a frequency range (beginning frequency is most important, as that is the shift point) helps.

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.
 Why is damped frequency is lower than undamped frequency with viscous damping but larger with structural damping?
 How can I specify acceleration at a node? Could I use the ‘big mass method’?
 How can I change the normalization method of the vibration modes from modal analysis?
 Why does the prestress from Static analysis does not add up to the stress in Random Vibration analysis?
 ANSYS Mechanical: Vibration Housing Noise
 In a Modal Analysis of Mechanical, why aren’t the Participation Factors Summary under Solution Information displayed?
 A Shock absorber is represented as spring element with damping constant. Modal analysis is performed using Reduced Damped (QRDAMP) solver. How to perform a Modal super position harmonic or transient analysis further ?
 Can you output the frequency response for a total deformation?
 In the results of a modal analysis, how can I define that a frequency is an output parameter ?
 What is mass moment of inertia in Point Mass used for?
Â© 2023 Copyright ANSYS, Inc. All rights reserved.