cancel
Showing results for 
Search instead for 
Did you mean: 
cancel
Showing results for 
Search instead for 
Did you mean: 

Vibration is not an option

Highlighted
Participant

Vibration is not an option

Okay, bad choice of words, but lingo or terminology is exactly the point of this message. After hours pouring over the Help files, Verification models, etc., I'm no closer to being comfortable with the Dynamic Analysis (Structure) interface. This seems like a simple problem:
A large structure (vibratory conveyor) is vibrating due to an eccentric driver mounted on a motor (these things are fairly common on vibratory feeders). I am going to be bolting my device to the structure and want to check out the response...look for weaknesses.
Speed: 900 RPM so Frequency is 15 Hz
Amplitude: +/-.125" at 15 degrees from vertical

This seems like a Base Excitation loading, but the UI baffles me. It may be that there is more than one way to skin this cat, but if you know of one I'd love to hear about it. I'd like to be able to run the 15 Hz against several iterations to determine response, as well as graph the system response to speeds ranging from 10 to 20 Hz.

Thanks,

Gavin B. Rumble PE
Solid Engineering
6 REPLIES 6

RE: Vibration is not an option

Suggestions were to run a Dyn Tme study. But it is the loading UI that is
confusing. What are the units of the results of a custom function you would
enter for Dyn Time Base Excitation for example? "Help" says that Base
Excitation acts thru the constraints. So surely the units cannot be lbs
(force)...a force acting at a constraint is always a no-no, or at least
ignored. Same question for Dyn Freq Base Excitation...what are the units?

I did place a Support call. The nice young man pointed us to the Help files
and said he couldn't do any consulting...which is understandable IF THE HELP
FILES ARE COMPLETE AND UNDERSTANDABLE. He did say Mechanica DOES NOT
support Enforced Dynamic Displacement. This sounds like the problem I want
to run...should I hire an ANSYS guy?

Thanks in advance,

Gavin B. Rumble, PE
Solid Engineering
336-224-2312



Original Replies:
---
David - Maybe you can run a Dynamic Time analysis that will show you the
transient response. After a while it will settle down into a steady state
response. No point in taking it further than that.

Or if you have varying frequency then you're looking at a Dynamic Frequency
analysis.

The key is getting your measures set up right. Getting your input right is
(as you're discovering) quite hard too.

Run your first analysis just looking at measures (I prefer 'relative to
supports') then run again, requesting 'full results' at specific points of
interest - i.e. peaks of measures on graphs etc.
---
Jeff - One of the types of analyses (not Dynamic Random....maybe it's
Dynamic Frequency?) allows you to input a repeating function as the
vibration input.

You need to first run a static analysis (if there are static loads), then
run a modal analysis, then run the final Dynamic Frequency(?) analysis. Log
a call to Tech support; perhaps they'll fill in some more information for
you.
---

Original Question:

Okay, bad choice of words, but lingo or terminology is exactly the point of
this message. After hours pouring over the Help files, Verification models,
etc., I'm no closer to being comfortable with the Dynamic Analysis
(Structure) interface. This seems like a simple problem:
A large structure (vibratory conveyor) is vibrating due to an eccentric
driver mounted on a motor (these things are fairly common on vibratory
feeders). I am going to be bolting my device to the structure and want to
check out the response...look for weaknesses.
Speed: 900 RPM so Frequency is 15 Hz
Amplitude: +/-.125" at 15 degrees from vertical

This seems like a Base Excitation loading, but the UI baffles me. It may be
that there is more than one way to skin this cat, but if you know of one I'd
love to hear about it. I'd like to be able to run the 15 Hz against several
iterations to determine response, as well as graph the system response to
speeds ranging from 10 to 20 Hz.

RE: Vibration is not an option

Gavin,

1. It looks like you should run Frequency response -- range from 10Hz to 20Hz, just make sure you have 15Hz (0.5 interval between 10 and 20Hz) requested in Output tab. Then you'll have 2 rabbits shot with 1 bullet (as a Russian saying goes...) -- get full results at 15Hz, as well as get the system's response from 10 to 20Hz.

2. Base excitation in Pro/M is defined as acceleration, so you should calculate the acceleration amplitude of the 'base' (pretty trivial task since you know the displacement amplitude and frequency) in whatever units you use for your model (e.g. m/s2, or in/s2, etc) -- given your desciption of the system, it looks like you should end up with a 'parabolic' acceleration amplitude function (i.e. acceleration proportional to frequency squared) -- then enter this function in the analysis definition form.

Hope it'll be of some help, and -- good luck.

Yuri, Ph.D,P.Eng.

RE: Vibration is not an option

P.S. While I remember... Since you'll be running base excitation, use mass participation factors to ensure the accuracy of your analysis. The total should be 0.8 or greater (0.9 or greater, I believe, is required by US Navy in their shock analysis requirements...), otherwise you'll need to use more modes (determined in the Modal analysis used for the Dynamics).

Yuri

RE: Vibration is not an option

Thank you all for the comments...this is starting to make some sense (in
other words, I'm just realizing more that I don't yet understand...is that
progress?). I'll post a summary sooner or later, but first I may pose a few
more questions.

I think when the "No Dynamic Enforced Displacement" limitation of
Pro/Mechanica finally sinks into my feeble brain we will start to get closer
to the solution...we were trying so hard to make THAT work! I think we are
starting to get our arms around the idea of an accel input instead of a
displacement input...it is, after all, just the 2nd derivative of
displacement (as a function of time). Part of the problem is they (the PTC
developers) left off the Acceleration label in the function UI for Base
Excitation Frequency studies...a person has no idea what quantity the
function is calculating!

Regards,

Gavin


Original Question:

Okay, bad choice of words, but lingo or terminology is exactly the point of
this message. After hours pouring over the Help files, Verification models,
etc., I'm no closer to being comfortable with the Dynamic Analysis
(Structure) interface. This seems like a simple problem:
A large structure (vibratory conveyor) is vibrating due to an eccentric
driver mounted on a motor (these things are fairly common on vibratory
feeders). I am going to be bolting my device to the structure and want to
check out the response...look for weaknesses.
Speed: 900 RPM so Frequency is 15 Hz
Amplitude: +/-.125" at 15 degrees from vertical

This seems like a Base Excitation loading, but the UI baffles me. It may be
that there is more than one way to skin this cat, but if you know of one I'd
love to hear about it. I'd like to be able to run the 15 Hz against several
iterations to determine response, as well as graph the system response to
speeds ranging from 10 to 20 Hz.

RE: Vibration is not an option

Several great suggestions were mentioned (summarized below) but this simple
problem is wupping us. Neither the Stiff Spring method of Enforced
Displacement or the Base Excitation method are returning expected results.
Either we are expecting the wrong thing, doing it all wrong, or Mechanica is
broke and needs fixing.

See this webpage for a description of the problem with screen shots.
http://www.solidpe.com/BaseExcitation.htm

First, using the Stiff Spring method recommended by Mr. Holst we were
getting enforced displacements of 0.0025 inches with 125 lbf acting at a
1000 lb/in spring...way short of the 1/8" that that force should have
produced. Besides, the harmonic (16.xx Hz) of the ruler itself was showing
up in the (spring mounted) base even though the spring is way stiffer than
the ruler.

Second, the Base excitation is returning screwy Base Displacements (see
webpage above).

As Bill O'Reilly says, "Where am I going wrong...?"

SUMMARY:
=== Yuri ===
1. It looks like you should run Frequency response -- range from 10Hz to
20Hz, just make sure you have 15Hz (0.5 interval between 10 and 20Hz)
requested in Output tab. Then you'll have 2 rabbits shot with 1 bullet (as a
Russian saying goes...) -- get full results at 15Hz, as well as get the
system's response from 10 to 20Hz.

2. Base excitation in Pro/M is defined as acceleration, so you should
calculate the acceleration amplitude of the 'base' (pretty trivial task
since you know the displacement amplitude and frequency) in whatever units
you use for your model (e.g. m/s2, or in/s2, etc) -- given your desciption
of the system, it looks like you should end up with a 'parabolic'
acceleration amplitude function (i.e. acceleration proportional to frequency
squared) -- then enter this function in the analysis definition form.

3. Since you'll be running base excitation, use mass participation factors
to ensure the accuracy of your analysis. The total should be 0.8 or greater
(0.9 or greater, I believe, is required by US Navy in their shock analysis
requirements...), otherwise you'll need to use more modes (determined in the
Modal analysis used for the Dynamics).

=== Jim ===
I don't know if it helps or if useful, but I show a method for doing
Enforced Dynamic Displacements in the Tips&Tricks section of my web site.
www.TSDengineering.com

=== David ===
1. Base Excitation is precisely putting your acceleration inputs at the
constraints. And as we all know Force and acceleration are related when
mass is involved. Think of it like being an earthquake. Normally you
constrain the base and it's rock solid, but then that solid base itself gets
wiggled. Your option is either to do base excitation (vibrating the
constraints) or to oscillate an applied load. So you can'y apply an
enforced displacement and oscillate that (Not to my knowledge at least).

=== Rami ===
I'm not entirely sure that you need to use vibration analysis in mechanica.
According to your description, at least as I understood it, you better use
MDX (mechanism analysis). The beauty of it is that after you have calculated
what you need/want in MDX you can transfer it directly into mechanica
(structural).
The vibration analysis in mechanica is great for detecting small deflection
inside the model or an assembly, however I found that MDX is better & easier
for the rest. Now since you know your input I don't think you will have any
difficulties.

END OF SUMMARY

Regards,

Gavin

RE: Vibration is not an option

Dear Gavin,

Looks like Mechanica's working OK to me from the info on your web-page.

disp = a sin(wt)
velo = aw cos(wt)
accel = -aw^2sin(wt)

So if a = 0.125", then the peak velocity will be 11.78 inch/sec, and peak
acceleration 1110.3 inch/sec^2 at 15 Hz. You haven't multiplied w^2 by the
displacement, so your acceleration input is 8 times too high.

You will notice that the velocity is a cosine function, thus there is an
initial velocity of 11.78 inch/sec. For your Mechanica input the initial
velocity would be 94.24 inch/sec, or 37.7 inch in 0.4 seconds. This is
what your second graph shows, hence Mechanica is doing the calculations
correctly.

What you need to do to get the 'correct' results is to select 'relative to
supports' in the dynamic time analysis dialog box, then you will get the
results that you expect.

If you're ever in the UK, you could consider taking our Advanced Mechanica
Vibration course!

Regards,

Rod Giles
Mechanica User since 1990


--
Rod Giles
Technical Director
Elite Consulting Ltd.
www.elite-consulting.com

> Several great suggestions were mentioned (summarized below) but this
> simple
> problem is wupping us. Neither the Stiff Spring method of Enforced
> Displacement or the Base Excitation method are returning expected results.
> Either we are expecting the wrong thing, doing it all wrong, or Mechanica
> is
> broke and needs fixing.
>
> See this webpage for a description of the problem with screen shots.
> http://www.solidpe.com/BaseExcitation.htm
>
> First, using the Stiff Spring method recommended by Mr. Holst we were
> getting enforced displacements of 0.0025 inches with 125 lbf acting at a
> 1000 lb/in spring...way short of the 1/8" that that force should have
> produced. Besides, the harmonic (16.xx Hz) of the ruler itself was
> showing
> up in the (spring mounted) base even though the spring is way stiffer than
> the ruler.
>
> Second, the Base excitation is returning screwy Base Displacements (see
> webpage above).
>