

August 25, 2023 at 12:16 pmSolutionParticipant
Q: How do I extract the Min/Max stress values over the frequency in workbench? The table shows only the frequency values. I’m additionally saving a MAPDL db. Can this interfere with the results I’m trying to retrieve from Workbench? A: In the Details window, you can RMB on the “By” option to select which stress to plot. Please check the attached simple test model (2051430.wbpz). I plot sigma Z over the frequency range (at a specific phase) and over the phase range (at a specific frequency). Also, saving a .db file will not affect the plotted harmonic results. ********************** Q: It is still not clear to me what the Max Over Frequency/Phase option is showing if not the Max Stress value for each Frequency? A: We cannot directly provide the maximum principal stress at any location, at any frequency, and any phase angle. You can sweep over a frequency range at a specified phase angle or over the phase angles at a specified frequency. You cannot automatically sweep over all frequencies and all phase angles simultaneously. For example, if you specify the frequency and sweep “maximum over phase”, the result is the maximum value of the quantity at any phase angle for that specified frequency. ********************** Q: If I specify a frequency and sweep (maximum over phase) to get the maximal stress physically possible at that frequency, can I do that automatically for every frequency in my table? A: Yes, if you request the amplitude of that result. The amplitude is the sqrt of the sum of the real value squared plus the imaginary value squared. You cannot automatically sweep through all frequencies and all phase angle to obtain the result at every combination of frequency and phase angle. That action would create a huge amount of data and most of it would have no value. ********************** Q: I’m looking for the maximal physically possible stress in my part for a defined frequency range. What would be the best way to get this result? Do I have to manually sweep over the phase for every specified frequency and write down the value? A: No. You could request any desired result (e.g., maximum principal stress) and then in the Details Window, set Amplitude = “Yes” and By equal to “Maximum over Frequency”. The resulting plot would represent the maximum principal stress at each node across the entire frequency range. Note that these stresses may not occur at the same frequency and phase angle for each node. The result at node i might be from frequency a and phase angle b, whereas the result at node j might be from frequency c and phase angle d. If desired, you could then RMB on that result and select “Create Results At All Sets” to obtain a contour plot of the amplitude of that result (maximum principal stress) at each frequency. Also, if you have plotted a result over a frequency range, there will be a tabular data showing the frequencies. If you RMB on any row in that table, you can retrieve or create that result for just that frequency. That is, you can automatically create a contour plot of the result at just that frequency.
Attachments:
1. 2051430.zip

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 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.
 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’?
 In Workbench Mechanical, how can I obtain strain energy output for Modal analysis?
 How to define variable thickness shell elements in ANSYS Mechanical? Is there any verification example of the variable thickness shell modal analysis available?
 How to apply applicationbased settings to improve the performance and robustness of transient structural analyses?
 Is it possible to perform a sineonrandom vibration analysis in either Mechanical or Mechanical APDL?
 In a Modal Analysis of Mechanical, why aren’t the Participation Factors Summary under Solution Information displayed?
 ANSYS Mechanical: Vibration Housing Noise
 How to include effect of bolt pretension in a modal analysis?
 Acoustics analysis of a speaker using FEA tools from ANSYS
© 2024 Copyright ANSYS, Inc. All rights reserved.