June 20, 2018 at 7:24 pmmasud407Subscriber
I would like to do frequency response analysis of a nonlinear system. I am applying load with a function of time. As harmonic response in for linear system, I am doing the transient response analysis now. Is there any way to convert the transient response output to frequency domain in ANSYS workbench?
June 20, 2018 at 10:10 pmpeteroznewmanSubscriber
I don't know how to do that in ANSYS Workbench, but I know how to export a time history result from Workbench and I have matlab with a wonderful set of free scripts called vibrationdata that give me a GUI interface to compute all sorts of frequency domain information from a time-history signal.
June 20, 2018 at 10:39 pmmasud407Subscriber
Does the time history result mean the data that I receive as tabular data in ANSYS?
June 21, 2018 at 12:51 ampeteroznewmanSubscriber
Yes, tabular data of any result quantity from a transient structural analysis has time in the first column.
June 23, 2018 at 9:53 pmmasud407Subscriber
I have received the transient data fora particular frequency and now I would like to export it in the matlab as per your suggestion. Can you please give me some hints/sources from where I can get the idea to to compute all sorts of frequency domain information from a time-history signal by using matlab? thanks.
June 24, 2018 at 3:20 ampeteroznewmanSubscriber
I like the vibrationdata GUI for computing various frequency content from time-history data.
Download the Vibrationdata Signal Analysis Package, which is a zip file of a large number of scripts.
Put the folder you extract the zip file into in the matlab path, then type vibrationdata at the matlab command line to start the GUI.
Attach your time-history data in a zip file if you want me to show you an FFT of that signal.
June 25, 2018 at 8:49 pmmasud407Subscriber
I have attached the zip file of time-history data in my previous comment.
June 25, 2018 at 9:05 pmpeteroznewmanSubscriber
Here is the data from your first tab plotted.
This doesn't look like it is the output from a Transient simulation. This looks like the nonlinear convergence plot of a Static Structural analysis.
I was expecting thousands of rows of data sampled at each millisecond for several seconds.
If you want to attach your ANSYS Project Archive, I will take a look at your model.
June 25, 2018 at 11:06 pmmasud407Subscriber
I have added the file in .wbpj format. Let me know if it works or not. After applying gravitational load in the static structural structure module, I applied acceleration varying with time in the transient structural module. In the acceleration tab, I used the formula containing 30 Hz and 0.4mm amplitude. I used substeps in the analysis setting.So can I calculate the outputs (acceleration, stress, strain) for other frequencies in the matlab VibrationData?
June 25, 2018 at 11:22 pmpeteroznewmanSubscriber
You can't just send the .wbpj file, that is not enough. The folder Ansys vib practice 2_files is also required. If you use ANSYS to create a Workbench Project Archive, then those two things are combined into a compressed file called a .wbpz archive. Here is more information.
I will understand what you have done once I have your archive or the complete zip file.
June 27, 2018 at 3:21 ammasud407Subscriber
I am trying to make wbpz file but facing some problems in the server. Anyway, I will send you immediately once I am done with it. Would is meant by the time history data? Does it mean the tabular data after solving?
How should I proceed in the vibrationdata initially with these time history data? Thanks a lot.
June 29, 2018 at 8:15 ammasud407Subscriber
Would you please suggest me a way to proceed with the time history data (obtained from Transient Structural module) in Matlab Vibration data so that I can perform the nonlinear frequency response analysis? Thanks a lot.
June 29, 2018 at 12:01 pmpeteroznewmanSubscriber
I will show you when you attach some transient data to analyze.
June 29, 2018 at 5:16 pmmasud407Subscriber
Thanks for your reply. Your guidance is helping me a lot to proceed step by step. Currently, I am using a simple structure as my practice where I put maximum 30 substeps. If I need to create large thousands of rows of data sampled at each millisecond for several seconds in transient structural module, what should I need to do? Will increasing the substeps/step time help me in this regard? Thanks
June 29, 2018 at 5:38 pmpeteroznewmanSubscriber
In a transient dynamics solution, you provide an initial time step, and a maximum time step and an end time. Say your end time is 1 second, if your initial time step is 1 ms and your maximum time step is 1 ms (1000 Hz sampling frequency), then you will get a minimum of 1000 rows in your output.
ANSYS can integrate through time internally, without reporting any output, so if you were to allow a maximum time step of 10 ms (100 Hz sampling frequency), then you would get no less than 100 rows in your output.
Have you heard of the Nyquist frequency? That is half the sampling frequency. If you want to perform an FFT, you can only plot data up to 500 Hz if your sampling frequency is 1000 Hz. Likewise, you can only plot data up to 50 Hz if your sampling frequency was 100 Hz.
If you want to plot data up to 1000 Hz, then you must have a sampling frequency > 2000 Hz or a maximum time step of 0.0005 seconds.
I hope this clarifies things.
July 3, 2018 at 9:07 pmKaiAnsys Employee
You can also try APDL command "RESP" which can convert input in time domain to frequency domain. There are some knowledge materials on that topic if you search for "RESP" in customer portal. Hope it helps.
July 15, 2018 at 12:48 ammasud407Subscriber
Mr. Peteroznewman, I have gathered some knowledge on Nyquist frequency. If I want to initiate the FRF analysis in vibrationdata, how should I proceed through vibration data? Which tab will allow me to process those data obtained from transient structural analysis?
July 15, 2018 at 4:27 ampeteroznewmanSubscriber
vibrationdata provides a Modal FRF analysis, which assumes you have the force time history of the input location and the acceleration response at the output location, in the correct format.
kcao mentioned the "RESP" function, which computes the shock response spectrum. This can also be computed by vibrationdata, but is not a FRF.
Please attach a zip file of your data and your Workbench Project Archive so I can look at it.
August 6, 2018 at 8:57 pmPunnag ChatterjeeSubscriber
@peteroznewman I am following this post as I am interested in performing (geometrically nonlinear/large deflection) frequency response analysis. I have a beam (very thin) fixed at both ends. When I apply a base excitation sinusoidal acceleration [A*sin(2*pi*f*t), f= frequency, t=time, A=amplitude] the fixed-fixed beam undergoes transverse vibrations. Say that t = 2 seconds, such that my input acceleration signal is 2s long, I would get a corresponding 2s amplitude (displacement probe) signal of the beam measured at probe location, in the direction of the input acceleration.
I have been able to set up the above-described problem using modal + transient structural modules in ANSYS workbench (18.1). However, I am facing two issues.
1) Turn on large deflection option seems to have vanished, without this I would not be able to see the FRF backbone curves (geometrical nonlinearities).
2) How do I automate the process by sweeping through a range of different input frequencies (f) and calculate the FRF at every 'f' as a ratio of RMS(probe signal)/RMS(input signal)?
The entire project rar is in the link(around 1GB)
August 6, 2018 at 9:13 pmpeteroznewmanSubscriber
A modal analysis is a linear analysis, so large deflection does not apply. A modal superposition transient analysis is therefore also a linear analysis, so large deflection does not apply.
Create a Transient Structural model without any links to Modal and that will be a Full Transient, which can have large deflection turned on and can have nonlinear materials and nonlinear contacts as well.
I am attempting to download your rar file, but it will be much easier if you Clear Generated Data on the Solution, even Clear Generated Data on the Model to delete the mesh, then File > Save As a new name. Then File > Archive. You can Attach that .wbpz file to your note above as it will be < 120 MB.
I will reply to the automation question after I have looked your model.
August 6, 2018 at 9:21 pmPunnag ChatterjeeSubscriber
@peteroznewman clearing data and putting it back into the same link and attaching here right now as I am typing. Thank you so much.
August 6, 2018 at 9:25 pmPunnag ChatterjeeSubscriber
@peteroznewman could not attach the files here so I have uploaded to the google drive folder link shared above (https://drive.google.com/drive/folders/1uyY1_ENFbDx5uayGo2IFfzXWcN7sb1ql?usp=sharing) under a new folder named "Support_Ansys_2_cleared_data". New folder size is ~11 MB
August 6, 2018 at 10:56 pmpeteroznewmanSubscriber
Okay, I opened the original file and have some more comments.
1) You have too many contacts due to an overly large search tolerance for automatically generated contacts. You have four pzt to ribbon contacts, which is what you want, but you have two pzt to pzt contacts that "jump over the ribbon". You don't want those. Suppress them.
2) You can have no contacts if you put the five bodies into one part and use Shared Topology to mesh them together. Right click on Geometry and Edit in DesignModeler. Pick the five parts in the outline and RMB then pick Form New Part. Now you will have 1 part and 5 bodies. Suppress all the Contacts in Mechanical.
3) Your acceleration sinusoidal signal has a frequency of 9.44 Hz but was sampled at 40 Hz (200 segments in 5 seconds). For time domain analysis it is recommended to have a minimum of 10 samples and preferred to have 20 samples per period. You have 4.25 samples per period. This is not very good and you can see the poor quality of the signal by the variation in the peak values.
Change the number of segments from 200 to 1000 which means a 200 Hz sampling frequency which is > 20 samples/period.
4) You have one solid element though the thickness, and you are bending it. Solid elements don't give accurate results in bending of thin geometry. A special element was created that has better accuracy, SOLSH190. I have changed your model to use that element. It would be even more accurate to put several elements through the thickness, but that was greyed out and I didn't want to slow down this solution.
5) I removed the connection from Modal Solution to Transient Setup cell so that the Full Transient solution could be done with Large Deflection on. However, that changed the Acceleration load and it would no longer support Base Excitation. I have to review the Dynamics training, but perhaps Base Excitation is only available as a linear analysis.
Why do you think you need large deformation? Why not stay with a linear analysis? It will run much faster as a Modal Superposition analysis than a Full Transient.
ANSYS 19.1 archive attached
August 7, 2018 at 12:20 amPunnag ChatterjeeSubscriber
Hi Peter (@peteroznewman),
Thanks for the reply. I will check all the points you have mentioned, in detail. However, regarding your point (5), I have developed an analytical nonlinear bending-torsion model and want to verify that with ANSYS results hence I need to simulate the nonlinear FRF. Did that answer your question?
I cannot open the file as it says the file was saved with a future version of the product. (downloading the 19.1 student version now) I am not very familiar with ANSYS/FEA software so the point regarding multiple layers through-thickness direction is something I had been searching for, so that is a big plus. Thanks.
August 7, 2018 at 1:15 ampeteroznewmanSubscriber
I added a Modal Superposition method to go alongside the Full Transient solution. There is a big difference in solution times. Modal = 4 seconds, MSUP Transient = 59 seconds, so total is 63 seconds. Full Transient solution = 1976 seconds, or 31 times longer.
I confirmed that for the Acceleration load, Base Excitation is only available for Modal Superposition method. The curious thing is that there is a setting called Absolute Result that can be Yes or No. I don't fully understand what that means, so I solved it twice. The No produced useful results, the Yes did not.
However, I did see the expected difference in the magnitude of the response between:
- Linear Mode Superposition = +/- 1.597 mm
- Nonlinear Large Deflection = +/- 0.41 mm
So I guess that is a good reason for the Full Transient!
Attached updated file ANSYS 19.1
P.S. I can't easily tell what version of ANSYS model you sent me unless you tell me.
August 7, 2018 at 2:32 amPunnag ChatterjeeSubscriber
I was using ANSYS Workbench 18.1. However, now I have downloaded 19.1 student version and was able to view/explore all the files you attached.
I went through both the attached files sent by you. All the suggestions were excellent. SOLSH190 link was something, which I never knew, very useful. I would still like to know how to create multiple elements through the thickness in future.
I have played with the setting: Absolute result (Yes/No). What I have observed is, when the Absolute result (yes) is selected it shows the deformation of the entire object along with rigid body deflection of the fixed ends too. With the Absolute result (no) selected it shows the relative deformation with respect to the fixed edges (relevant for my purpose).
If you could throw some light regarding the automation i.e. changing the frequency in a range instead of using a fixed value of 9.44 Hz and automatically finding the RMS ratio of output probe / input signal, it would be amazing.
August 7, 2018 at 12:29 pmpeteroznewmanSubscriber
Thanks for your observations on Absolute result Yes/No.
Creating more elements through the thickness will need a special work around for the Manual Thin Src/Trg Selection in the Sweep mesh control since the interface seems to assume you would only ever want one element. I don't immediately know how to do that.
I posted a new discussion to find out how to create the frequency as a parameter to a design study to sweep through a range of frequencies.
July 2, 2019 at 3:26 ammasud407Subscriber
Is there any way to linearize a system in ANSYS so that frequency response can be done?
I have considered a simple geometry and performed the harmonic response. However, Now I am considering a nonlinear system. For nonlinear system, will it be correct if I start with the harmonic response?
- 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.