MECHANICA: How do I simulate a sine sweep? 2

[Flask]

How do I simulate a sine sweep in Mechanica? I'm trying to identify resonant frequencies in a test fixture and the acceleration at each freq.

I've set up a Dynamic Freq analysis. I've created an acceleration measure. How should define the input? How do I interpret results?

Thanks!

 

[Twoballcane]

Why? Just do a modal analysis. This will find all of the resonant in either defining the band width you want or the number of resonate. Typically you would only want to find the first three. The first resonant is the Fn.

What is your application?


Tobalcane
"If you avoid failure, you also avoid success."
“Luck is where preparation meets opportunity”

 

[Flask]

Thanks Twoballcane.

Will a modal analysis tell me the response at each resonant freq? How do I know what the response is compared to the input?

 

[Twoballcane]

What do you mean response? You mean the G load at each resonant? Not until you have vibration or a shock (or any dynamic) event will you see a load.

Are you doing shock or vib?

For test fixtures, you would want to find the Fn and make sure it is one or two octave away from anything your are testing, preferably above the Fn of the UUT so that you don't couple and amplify the UUT. You don’t want the fixture to be a forcing function. If you are doing any kind of random vibration, you would like the Fn of the fixture to above the bandwidth you are testing too. The first three modes are the ones you should be concerned if you are doing any shock so that you would know how the fixture would move when exposed to the shock event.


Tobalcane
"If you avoid failure, you also avoid success."
“Luck is where preparation meets opportunity”

 

[Flask]

I'm doing vibe. And yep, I understand (1) the fixture Fn shouldn't be close to the UUT Fn and (2)the fixture Fn should be outside of a random vibe freq range.

So when I characterize the fixture I should know: where the resonant frequencies are and also amplification at each resonance, right? i.e. If I put a 1G load in do I get a 1.5G response or a 6G response.

Or let's say I'm designing a circuit card assembly (CCA) that goes on an airplane. I'd want to make sure that the CCA Fn doesn't coincide with an airplane input. So I'd want to know what the resonant frequencies are, but also the amplification at each resonant freq, right?

many thanks.

 

[Twoballcane]

“So when I characterize the fixture I should know: where the resonant frequencies are and also amplification at each resonance, right?”

Yes. You will want to look into the transmissibility (Q) of your input to your output on your fixture (and then into your UUT).

If you have a random vib profile (G^2/Hz), you can put that into ProM.

“Or let's say I'm designing a circuit card assembly (CCA) that goes on an airplane. I'd want to make sure that the CCA Fn doesn't coincide with an airplane input.”

Yes this is correct

So I'd want to know what the resonant frequencies are, but also the amplification at each resonant freq, right?”

Yes. But, what will you do with this information? Are you looking into the stress the CCA will see? If this is right, than once you know the G load at Fn and calc the deflection, than you can calc the stress.

Please keep asking questions, but a great book to read would be Vibration Analysis for Electronic Equipment by Dave Steinburg.



Tobalcane
"If you avoid failure, you also avoid success."
“Luck is where preparation meets opportunity”

 

[Flask]

Great suggestion on Steinberg- I've got the book... and have used his approach for fatigue predictions.

In the past, someone else was telling me the Fn, now I'm doing some of the structural FEA.

So I still want to run a sine sweep, identify the resonance frequencies and the acceleration at each resonance. A more general example might be some kind of mounting arm attached to a wall (simple cantilever type situation). I've set up the modal analysis, and set up the dynamic frequency analysis. My question remains:

(1) How do I set up the frequency input? Do I just use the default Mechanica "uniform" field?
(2) How do I view the results? I've created an acceleration measure- is that the way to do it?
(3) How do I view transmissibility in Mechanica?

thanks

 

[seymours2571]

Flask,

For last year's PTC User conference I created a presentation that covers exactly what you are trying to do. You can find the presentation on my site at the following link:

http://www.seymourecg.com/downloads/ptcuser2010/ptcuser2010_design_eng_with_promech.zip

Or

Got to my website and click on the link "Design Engineering with Pro/Mechanica"

The zip file contains both the presentation and the associated videos. Sorry...last years presentation did not have audio....this year's presentation will. The video shows you step by step how to force vibrate the part using a dynamic frequency analysis, create acceleration measures, plot the response in G, and subsequently extract the displacement and stress results at specified frequencies.

Let us know if you still have questions. If you will be at the PTC Conference this year in Las Vegas then bring your stuff with you and I can walk you through everything directly.

Good luck,

Steve



Stephen Seymour, PE
Seymour Engineering & Consulting Group

http://www.seymourecg.com

 

[Flask]

Wow Steve, thanks. Those videos were incredibly helpful. Got me a long ways farther. Thanks.

I've got a couple follow-on questions if that's okay:

(1) freq direction/vector: in the video you took the transform from one csys to another because you wanted the force applied in a direction that was not directly along one of the axes of the world csys, right? So if I just want to, say, go directly along the z axis of the world csys, I'd just enter a "1" next to Z and a "0" for X and Y, right?

(2) You created a frequency function that was equal to the acceleration of gravity (387 in/s^2). I could just use the default "uniform" function, and then when viewing the results, an acceleration of 2.0 would be the same as 2Gs, right?

(3) You used a damping coeff (%) of 3%. I've seen 4% used in PTC documentation. Is this just a good ballpark number, or should I be using tailoring this number more?

(4) Mass Participation Factor (MPF). You checked this box in your analysis definition. My crude understanding of MPF is that it's a measure of how much of the part/assembly is participating in the response. That number should usually be >80%, right? And if it's low, I should increase the number of modes in the modal analysis, right?

Thanks again- it was really a huge help. We may be in Las Vegas; I'll be sure to look you up if we're there.

 

[seymours2571]

Flask,

(1) That is correct. For the particular application and simulation the desire was to have the force vibrate in a specific direction that did not lie on any of the WCS axes. If you wanted to vibrate along any one of the axes just do as you stated by applying a 1 in the desired direction and 0 in the others.

(2)Hmmm. Interesting question. I don't think it would work that way. I have never tried. You might have to do some trial and error to see if this would work. My gut says no. However, it appears that the unit of "g" is not available in WF5 as a unit selection for graphing results.

(3) The part I was simulating was steel. Steel has a damping % somewhere in the neighborhood of 2-3% depending on the alloy. This will have to be obtained via testing or via literature like a book or a scientific paper.

(4) Your crude understanding is correct. Most analyst try to include enough modes such that the cumulative MPF is greater than 80%, however some situations may dictate a higher level like 90%. This is really done so that you don’t just simulate the default first four modes and call it done. If 80% or more of your MPF are in the first four modes then fine...your are done. Yet, some guys will run the first four by default, have a cumulative MPF of 20%, and miss the fact that mode 6 (which was not included) has a MPF of 70%. This means they would have missed a huge mode, that if its resonant frequency is at or near the operating or excitation frequency there could be big problems in the near future.

I will be giving two presentations at the conference. This one you have now will be given with a few updates to it. So if you go to the conference just catch me after the presentation and we can discuss.


Steve

Stephen Seymour, PE
Seymour Engineering & Consulting Group

http://www.seymourecg.com

 

[Twoballcane]

Some great insight there seymours. And, if you two meet, that is some cool networking in action!

Tobalcane
"If you avoid failure, you also avoid success."
“Luck is where preparation meets opportunity”

 

[Flask]

Thanks for the answers Steve.

I've got one more question guys. If I use the above approach, can I compare the results to test data from a sine sweep?

Here's why I ask: on a shaker table, the energy is applied to the part by the table and up through the mounting structure on the part. Is "base excitation" in Mechanica a similar loading scenario? ... Or would I need to somehow use loading functions to simulate the way the load is applied by a table?

My feel is that base excitation is the way to go, but I'm not 100% on that.

many thanks.

 

[seymours2571]

Base excitation is the typical approach for me. Mechanica's help files and PTC's KB will shead a little more light on this, but selecting either force funcitons or base excitation will change the reference point from where displacements are measured.

Base excitation will apply the forced vibration at the constraints.

Steve


Stephen Seymour, PE
Seymour Engineering & Consulting Group

http://www.seymourecg.com

 

[reyes163]

Hi Steve, when I have tried to do the vibe analysis, actually my base excitation is not available, meanwhile, I have used user-defined step and can't click the full result tab, it is gray and unavailable for clicking. so I can't get the Von-Mises at 1st resonse refrequency, and I can just get the stress at X, Y, Z direction.