## General Mechanical

Topics relate to Mechanical Enterprise, Motion, Additive Print and more

#### Harmonic Analysis – how to accurately collect directional frequency response

• Theodore Jenkins
Subscriber

Hi, i am trying to determine the frequency response in the Y- direction for three surfaces/points.
1 at the contact between the two small accelerometers (left and right), and the top of this 'dual rail magnet', where another accelerometer sits (point mass A).

this setup is trying to replicate what I have in a lab, where a vibration exciter is exciting the bottom of the 'rod' in the global Y-axis.

It manages to read some resonance points for some mode shapes, but there are other mode shapes (such as 'total deformation 8') that the harmonic analysis frequency repsonse does not pick up.
The two small accelerometers would be experiencing signifcant resonance at this 8th natural frequency, as would the acceleromter mounted upon the large dual rail magnet, but this is not reflected at all in the hamonic response frequency plot.

it is my belief that there should be a y-axis resonance here, but it appears not.

i tried selecting different geometry, such as a node on the edge of the dual rail magnet cylinder, and set some to use "maximum" instead of average but no luck. in the simulation inside the modal analysis, i can see that the node i selected in moving in the Y- direction, as well as moving side to side in the x direction...

I am not using MSUP due to the desire to model a damped system.

the purpose of all of this is to try predict the response of various mounting methods upon curved sufaces, so this is my approximation of a magnet attached to the curved surface. another challenge i am having is that i can only model linear contacts using this analysis, but i do not have the computer power or patience to run through multiple different models with different mounting methods and a range of 10kHz all using transient analysis, so I am willing to take the loss on that front, i will report my challenges and essentially say "this was the best i could do".

I would appreciate any help anyone can provide. attached is my workbench file and the STEP file in this link

Thank you,

Theo

• peteroznewman
Subscriber

Hello Theo,

Please describe more fully the support of the Test_Specimen. You show a rod bonded to the bottom. The bottom of the rod has a Harmonic Pressure load which acts along the Y axis and the bottom of the rod also has an elastic support and a Displacement that holds X and Z at 0 and leaves Y Free. In your model, I wonder if the displacement and elastic support on the bottom of the rod accurately represent the setup you have in the lab.

The setup in the lab uses a vibration exciter to excite the bottom of the rod in the Y direction. What is the setting on that vibration exciter?  Is that exciter set to provide a Force, Displacement, Velocity or Acceleration amplitude?

My experience is with harmonic testing on a shaker table where the test article is bolted to a fixture which is bolted to the table. The fixture has its first mode far above the highest mode of interest on the test article.  Does your test article bolt to another structure?

I have also read about harmonic testing of structures that don't bolt to anything, for example a satellite.  Ground testing of satellites might hang the structure from a few springs. A vibration exciter applies a harmonic load at one point on the structure in a single direction using a slender rod called a stinger. Accelerometers pick up the response of the structure at other points.

You were expecting to see a resonance of Mode 8 in the Harmonic Response. Not all modes resonate in the Harmonic Response. Consider a cantilever beam. The first few modes are bending around the low thickness direction, then there is a twisting mode, and later there will be a bending mode around the high thickness direction. If the harmonic load is only normal to the thin direction of the beam, then you will only see the first few bending modes show up. You won't see the twisting mode because there was no load to excite that.  If you use two harmonic loads, one on each corner of the tip and they were 180 degrees out of phase, that would excite the twisting mode.  In your model, the geometry is symmetric and the load is centered and aligned to the Y axis, so there is nothing to excite Mode 8.

• Theodore Jenkins
Subscriber

Hi Peter,

I have been reading your responses to other people for months now and i am always astounded by your knowledge and clarity of response. Thank you very much.

1 - the test-specimen is affixed to the moving part of the vibration exciter via a double ended stud bolt (See photo 1), and I beleive that this connection is not stiff enough ie the first mode is lower than the highest mode of interest. I beleive the setup is flawed, but i just need to be able to model it as best i can with FEA, i will address the concerns in the discussion of my thesis.
The elastic support was my attempt at creating "weak springs" to restrict the rigid body motion of the part. i did not want to model the exciter as i do not know enough about it to model it with any certainty.

2 - I really should know that, thank you for bringing it up. i will find out ASAP. Currently, we generate a sine wave or a particular frequency and convert it to analogue signal, which is then passed into the exciter.

3 - i dont know much about exciter tables. the vibration exciter sits on a heavy steel plank which rests on a table. photo 2 shows this.

4 - i have seen something similar in my vibrations class, however, we are trying to replicate the vibration of a pipe/pipeline. we are more just interested in the range of frequencies for which the accelerometer response is reliable before the mounting method reaches resonance. i.e., connecting a flat magnet on the curved surface would likely have some wobble (my theory) that would mean reduced accuracy. we are testing 0-10kHz.

5 - This makes so much sense, wow! thank you, i totally see what you mean. in the real experiment though, i assume there will be some of that motion, making the magnet wobble... this is just my assumption. experimental data shows a real spike (dB) at around 8kHz, therefore i believe this is what is happening. should I try to add some small excitation in another direction/point to try simulate this?

Also, experimental data I am using is from this vibration exciter orientated in the vertical direction, so the centre of gravity is acting through the centre of the exciter i.e. no moment due to gravity on the test specimen/accelerometer/magnet etc.

kind regards,

Theo

• peteroznewman
Subscriber

Hi Theo,

Thank you for the photos, that really helps to explain what you are trying to model. I agree that the single stud is going to create a cantilever beam support to your test specimen.

It is often the case in simulation where perfect geometry and perfectly aligned loads don't create a result that matches an experimental result. An example is a column under a compressive load in a nonlinear static structural analysis. The column just compresses, but experimentally, it buckles. In order to simulate reality, imperfection in the geometry is introduced and/or the load is applied off-center. You may need to introduce some small amount of imperfection to see Mode 8 appear in the harmonic response results.

The vibration exciter appears to be an electrodynamic shaker and when you put in a sine wave, it will vibrate at that frequency. It's good that you are using it in the vertical orientation. You don't need to include the exciter in your model.

You said you are not using MSUP because you want to model a damped system.  MSUP Harmonic Response analysis is always used with damping. The damping controls are in the same place under the analysis settings. The limitation is you can't use Structural Damping and simply provide one input like you did with the full Harmonic Response, but you can insert damping as two values for Mass and Stiffness damping, or a table of values versus frequency.

I recommend you switch to MSUP Harmonic Response, because then you can make the face of the rod a Fixed Support and use Base Excitation as the Harmonic Load. This will more accurately represent the connection of the stud to the shaker.

Best regards,

Peter

• Theodore Jenkins
Subscriber

Hi Peter,

Wow, of course! I have shifted the centre of mass of the accelerometer off centre a little bit, which accounts for the non-zero effect of the wires attached to each accelerometer. It is now showing something in the region i expected, but of a lower magnitude than i thought. I will see what else I can do by playing with the geometry and shifting the point mass around... might not be large enough to have a significant impact.

Ok, that is great to know RE MSUP, I will implement that asap and see the results. I am not sure about how i can determine the mass and stiffness damping of my real system as a single value or as a function/table of frequency... but addmittedly I was guessing the structural damping so i might play with it until the damping matches my experimental values. I will watch one of the ANSYS damping videos.

Once again you have come to the rescue, I really appreciate your help with this, and I am sure there are people reading this and other posts in the future that appreciate your responses.
Are you an employee of Ansys? or are you just a whizz at this stuff and want to help out?

anyway thank you, you have been a great help!

• peteroznewman
Subscriber

Hi Theo,

No, I'm not an employee of Ansys, I spend time helping students for my own enjoyment of teaching.

Regards,

Peter