Turn on suggestions

Auto-suggest helps you quickly narrow down your search results by suggesting possible matches as you type.

Showing results for

Auto-suggest helps you quickly narrow down your search results by suggesting possible matches as you type.

Showing results for

** Community Tip** - Did you know you can set a signature that will be added to all your posts? Set it here!
X

- Community
- Creo (Previous to May 2018)
- Creo Modeling Questions
- Vibration is not an option

Options

- Subscribe to RSS Feed
- Mark Topic as New
- Mark Topic as Read
- Float this Topic for Current User
- Bookmark
- Subscribe
- Mute
- Printer Friendly Page

Jun 05, 2006
09:57 PM

- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Notify Moderator

Jun 05, 2006
09:57 PM

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

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

Jun 06, 2006
02:15 PM

- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Notify Moderator

Jun 06, 2006
02:15 PM

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.

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.

Jun 06, 2006
10:37 PM

- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Notify Moderator

Jun 06, 2006
10:37 PM

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.

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.

Jun 06, 2006
11:01 PM

- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Notify Moderator

Jun 06, 2006
11:01 PM

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

Yuri

Jun 07, 2006
06:23 PM

- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Notify Moderator

Jun 07, 2006
06:23 PM

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.

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.

Jun 13, 2006
11:45 AM

- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Notify Moderator

Jun 13, 2006
11:45 AM

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

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

Jun 13, 2006
12:34 PM

- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Notify Moderator

Jun 13, 2006
12:34 PM

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).

>

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).

>