

June 13, 2018 at 4:41 pmItalicBikeSubscriber
Hi everybody,
I've to model an experimental modal analysis, so i create an harmonic response analysis. I need to apply a "impulse". This impulse is not ideal, so i have to model the frequency spectrum of that, but i don't know how to do that.
I learn that only force can be applied tabular with frequency, but i can't select mesh node as geometry selection or named selection. Opposite, nodal force can be applied to mesh node named selection but i can't write it like a load vs. frequency.
I hope my problem it's clear.
Thanks for any help
Regards.

June 13, 2018 at 5:47 pmpeteroznewmanSubscriber
Hi ItalicBike,
It would be easier to visualize your problem if you would provide a sketch of the structure and how it is supported. Maybe you could create an archive of your Workbench Project that just has the Modal analysis and attach it to your post above using the Attach button.
Experimental Modal Analysis uses a hammer to tap at one location on a structure and an accelerometer to measure the response at another location on the structure. The Frequency Response Function (FRF) shows how the impulse from the hammer, which contains a broad spectrum of frequency content, appears at the accelerometer location after being transformed by the natural mode shapes of the structure. During the experiment, it is possible to collect FRFs at multiple locations around the structure. Sophisticated software can take all those FRFs and create a stickfigure representation of the structure and animate all the natural modes that were exposed by the analysis of the FRFs. Discovering the natural mode shapes and frequencies of the structure is the most important output of Experimental Modal Analysis.
ANSYS Modal Analysis computes the natural mode shapes and frequencies without having to hit the structure with a hammer.
You can simulate striking the structure with a hammer and you can plot the response of a point on the structure where you might mount an accelerometer. You can do that for the academic exercise of reproducing what you did experimentally, but it is not necessary to determine the natural frequency and mode shape. It is useful if you want to know how far one point on the structure will move when another part is hit with a particular force. Is this what you are trying to simulate?
The simulation of striking a structure with an impulsive force is done in a Transient Structural system. You could literally have a hammer head of mass m, strike the structure with velocity v, at time t=0 and watch the structure deform and the hammer head bounce off. That is one way to simulate the hammer strike. Another way is to take the forcetime data from the force transducer behind the hammer tip and apply that to one point on the structure.

June 14, 2018 at 8:06 amItalicBikeSubscriber
Hi peteroznewman,
as you said, i exactly need to reproduce the modal analysis. The goal is to carry out the analysis firstly without and secondly with a polymer and demonstrate if the frequency response in some points change.
I got the experimental analysis to validate the model without polymer, but if i apply a ideal impulse the results are very different.
Could you help me? Is it the right way to got the goal?
Thanks

June 14, 2018 at 11:01 ampeteroznewmanSubscriber
Hi ItalicBike,
Yes I can help. It would be easier to help you if you create an archive of your Workbench Project and attach it using the Attach button.
Do you have the forcetime data from the force transducer built into the modal hammer used in the experiment? Do you have the accelerationtime data from the accelerometer from the same hit that the forcetime data came from? Put those data in a zip file and attach the zip file along with your project archive .wbpz file.
What version of ANSYS are you using?
Peter

June 14, 2018 at 11:44 amItalicBikeSubscriber
Hi peteroznewman,
I'm using ANSYS 18.2.
The load it's applied in named selection "Excitation Point", and the responses it's measured in "Point 1".
Thanks for any help.

June 15, 2018 at 10:47 ampeteroznewmanSubscriber
Hi ItalicBike,
I changed your Geometry and sliced it up to make a vertex at the Evaluation Point. I changed the BCs to be on geometry instead of nodes. I don't have the sall BC quite the same, you can make 4 planes and 4 slices to make faces where you want to bond to a wall.
I changed your model to be a Modal Superposition method to calculate the Harmonic Response. That is done by linking the Modal Solution cell to the Harmonic Response Setup cell.
That required that I turned off the Damped solver in Modal.
I requested modes up to 750 Hz, which is 1.5 times higher than 500 Hz.
Here are the natural frequencies below 750 Hz:
In Harmonic Response, the Analysis Settings request frequencies between 100 and 500 Hz with 400 data points. You can see five peaks that correspond with the five modes found above. You can see that mode 5 has a bigger response at the evaluation point than mode 4.
If you click on the Solution Information folder for Harmonic Response, the Solution Output text will display. Scroll down till you find the PARTICIPATION FACTOR CALCULATION and look at the Y direction table. The RATIO column shows that mode 1 has the biggest contribution and mode 5 the second biggest to the response at the evaluation point. This is not what the graph above shows because the size of the peaks on the graph strongly depend on the spacing of points along the frequency axis. If you rerun the analysis and put 100 points between 150 and 170 Hz, the height of the maximum in the graph will jump up. The peaks are even more strongly dependent on damping, which is the whole point of your experiment, right?
Another analysis that can be added to this model is a Transient Structural.
This is where the forcetime plot you showed in the attachment can be applied to the vertex in the center.
Reply with the data from the graph in a text file or spreadhsheet if you want me to help with that.
The accelerationtime plot at the evaluation point can be made. This would simulate the data an accelerometer would record at that point when the force is briefly applied at the center. You can take that data, transform it to dB, compute the frequency content and plot the Power Spectral Density or FFT magnitude vs. Frequency. However dB is a ratio relative to a reference value. What is the reference value that you would divide the acceleration by to compute dB?

June 18, 2018 at 3:39 pmItalicBikeSubscriber
Thanks for help me peteroznewman.
So, if I've well understood, I can perform my analysis without the modal and harmonic response block, right?
Best Regards.

June 18, 2018 at 5:41 pmpeteroznewmanSubscriber
Yes, you can use just a Transient Structural with no other systems and it will solve the response to the forcetime history applied to the center point.

June 20, 2018 at 8:55 amItalicBikeSubscriber
Thank you peteroznewman,
the last one question: what if I transform with a FFT the load from time domain to frequency domain and I apply it in an harmonic response analysis? Do I obtain the same results?
Regards.

June 20, 2018 at 10:05 ampeteroznewmanSubscriber
Harmonic Response lets you assign the amplitude of a load to a steady state sine wave with adjustable frequencies and solve the steady state sine wave response at each frequency. Harmonic response is a Linear System analysis, so if you double the load amplitude, you double the response.
You could scale the response at each frequency according to the FFT magnitude of the load. I don't know if that gives the same result as applying a transient load and taking the FFT of the response. Why don't you try it and see if you get the same result. Maybe try it on a simple model. One reason the results could be different is if you allow the transient to include any nonlinearity, for example if large deflection is on.
You have a loadtime history that is not harmonic, and you have the ability to compute the transient response to that loadtime history. You can output the accelerationtime history at Response Point 1, then perform an FFT on that signal. The graph you showed is Acceleration [dB], however dB is a ratio relative to a reference value. What is the reference value that you would divide the acceleration by to compute dB?

September 17, 2018 at 9:25 amItalicBikeSubscriber
1 mm s^2

September 17, 2018 at 11:47 pmsk_cheahSubscriber
I've to model an experimental modal analysis, so i create an harmonic response analysis. I need to apply a "impulse".
I would advice against doing the analysis in the time domain. Better to first correlate your damping, natural frequency and mode shapes to your modal test before doing it in the time domain.
To replicate the FRF of your test, apply a unit harmonic load at where the impact hammer was applied. The analytical response at the location of your accelerometer would be your FRF.
Kind regards,
Jason

 The topic ‘Force Spectrum in Harmonic Response Analysis’ 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.
Ansys Blog
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 do the frequency response of the nonlinear vibration of a flexible PCB?
 Importing Line and Solid Bodies from SpaceClaim to Mechanical
 how to open SendCommand in Ansys
 problems facing during solution
 Still facing the same issue
 Failed to move file from solver directory to scratch directory: file.rst
 Adaptive Sizing
 Stiffness factor
 Import DAT file
 Import pressure data (coordinates and value) to ansys workbench through excel

8808

4658

3153

1680

1470
© 2023 Copyright ANSYS, Inc. All rights reserved.