XANSYS Forum Index
    Register    

FAQ    Search    Memberlist    Usergroups    SmartFeedSmartFeed    Profile    Log in
[STRUC]pendulum to minimize displacements in the main struct
 
This forum is locked: you cannot post, reply to, or edit topics.   This topic is locked: you cannot edit posts or make replies.    XANSYS Forum Index -> XANSYS
Author Message
catarina.sousa
User


Joined: 22 Jul 2013
Posts: 13

PostPosted: Tue Jul 23, 2013 9:06 am  Reply with quote

Hello everyone,

I'm a student in Portugal in Faculty of Engineering of University of Oporto, and my master thesis is about using pendulums as tuned mass dampers.

I'm starting by modelling a very simple example of a structure in ansys to test results

The main structure is a simple frame with the mass of : 160,5 kg and lateral stiffness in the x direction of 4050 which gives the natural frequency of 0,79995 confirmed by a modal analysis, after that I've applied a transient analyses with a horizontal sinusoidal force of 100*sin(pi/4*time) and obtain a maximum displacement of 0,028. (this is without the pendulum to have something to compare to)

What I'm struggling with, is the pendulum, i have model it with link180 and mass 21 (with 32.1 of mass) like in the picture of the link below, (i have done a coupled DOF to simulate a pin joint) and applied the same sinusoidal force and the results stay the same, the don't decrease as I expected (I've tried different lengths and mass for the pendulum and nothing changes)

https://dl.dropboxusercontent.com/u/90559128/nao_estou_a_conseguir_resultados.png

and I know it is possible to model a pendulum on ansys like in this example

http://www.esss.com.br/events/ansys2013/brazil/pdf/24_4_1510.pdf

but I have been trying and trying and keep failing, so I really need some guidance and help because I don't no what else to do.

Thanks in advance for the attention.
Back to top
View user's profile Send private message
chris.masterson
User


Joined: 10 Jan 2012
Posts: 41

PostPosted: Tue Jul 23, 2013 10:05 am  Reply with quote

Have you applied gravitational acceleration to the model (or some other relevant acceleration field)?  Pendulums are meaningless without an acceleration to act on the mass.

Chris Masterson
LightSail Energy



On Tue, Jul 23, 2013 at 9:06 AM, catarina.sousa <ec08215@fe.up.pt (ec08215@fe.up.pt)> wrote:
Quote:
Hello everyone,

I'm a student in Portugal in Faculty of Engineering of University of Oporto, and my master thesis is about using pendulums as tuned mass dampers.

I'm starting by modelling a very simple example of a structure in ansys to test results

The main structure is a simple frame with the mass of : 160,5 kg and lateral stiffness in the x direction of 4050 which gives the natural frequency of 0,79995 confirmed by a modal analysis, after that I've applied a transient analyses with a horizontal sinusoidal force of 100*sin(pi/4*time) and obtain a maximum displacement of 0,028. (this is without the pendulum to have something to compare to)

What I'm struggling with, is the pendulum, i have model it with link180 and mass 21 (with 32.1 of mass)  like in the picture of the link below, (i have done a coupled DOF to simulate a pin joint) and applied the same sinusoidal force and the results stay the same, the don't decrease as I expected (I've tried different lengths and mass for the pendulum and nothing changes)

https://dl.dropboxusercontent.com/u/90559128/nao_estou_a_conseguir_resultados.png

and I know it is possible to model a pendulum on ansys like in this example

http://www.esss.com.br/events/ansys2013/brazil/pdf/24_4_1510.pdf

but I have been trying and trying and keep failing, so I really need some guidance and help because I don't no what else to do.

Thanks in advance for the attention.






+-------------------------------------------------------------+
|            XANSYS web - www.xansys.org/forum                |
| The Online Community for users of ANSYS, Inc. Software      |
|            Hosted by PADT - www.padtinc.com                 |
| Send administrative requests to xansys-mod@tynecomp.co.uk (xansys-mod@tynecomp.co.uk)   |
+-------------------------------------------------------------+





--
Chris Masterson
Design Manager
LightSail Energy, Inc|www.lightsailenergy.com
Phone: (510) 981-8088 Ext 108
Fax: (510) 981-8286
Email: cmasterson@lightsailenergy.com

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
catarina.sousa
User


Joined: 22 Jul 2013
Posts: 13

PostPosted: Tue Jul 23, 2013 11:37 am  Reply with quote

Thanks for the reply Chris Masterson,

Yes I have considered aceleration in the model with the folowing command:

ACEL,,9.81

But the results with and without the aceleration don't change ...

Catarina Mendes Alves e Sousa,
Student
Faculty of Engineering of Porto
Back to top
View user's profile Send private message
Martin Liddle
User


Joined: 15 Aug 2008
Posts: 1274
Location: Chesterfield, UK

PostPosted: Tue Jul 23, 2013 1:12 pm  Reply with quote

On 23/07/2013 17:06, catarina.sousa wrote:

Quote:

What I'm struggling with, is the pendulum, i have model it with link180 and mass 21 (with 32.1 of mass) like in the picture of the link below, (i have done a coupled DOF to simulate a pin joint) and applied the same sinusoidal force and the results stay the same, the don't decrease as I expected (I've tried different lengths and mass for the pendulum and nothing changes)

Have you looked at an animation of the transient? Is the pendulum moving?

--
Martin Liddle, Tynemouth Computer Services,
Chesterfield, Derbyshire, UK.
www.tynecomp.co.uk

Post generated using Mail2Forum (http://www.mail2forum.com)
_________________
Martin Liddle, Tynemouth Computer Services,
Chesterfield, UK.
Back to top
View user's profile Send private message Visit poster's website
karl.volkmann
User


Joined: 27 Jun 2013
Posts: 31

PostPosted: Tue Jul 23, 2013 1:16 pm  Reply with quote

I could be wrong here but as far as I know, modal analysis simply returns the frequencies from the eigenvalues/eigenvectors of the homogenous stiffness/damping/mass system. And therefore gravity and other accelerations won't come into play. I believe you need to be doing an harmonic analysis with forcing on the main structure and a global 1G acel (be careful with your signs and coords). Your answer makes sense. You simply asked it for natural frequencies, and it gave you natural frequencies.

Karl Volkmann
Kionix, Inc.

-----Original Message-----
From: xansys-bounces@xansys.org [mailto:xansys-bounces@xansys.org] On Behalf Of catarina.sousa
Sent: Tuesday, July 23, 2013 2:37 PM
To: xansys@xansys.org
Subject: Re: [Xansys] [STRUC]pendulum to minimize displacements in the main struct

Thanks for the reply Chris Masterson,

Yes I have considered aceleration in the modal with the folowing command:

ACEL,,9.81

But the results with and without the aceleration don't change ...

Catarina Mendes Alves e Sousa,
Faculty of Engineering of Porto






+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
catarina.sousa
User


Joined: 22 Jul 2013
Posts: 13

PostPosted: Tue Jul 23, 2013 1:32 pm  Reply with quote

I have checked the animation before and checked again just to be sure and the pendulum is moving.

My concern in this case is not really the natural frequencies, is more the fact that I'm doing a transient analysis with a sinusoidal force in the two cases (with and without the pendulum) and maximum displacements don't change, but I'm really thankful for the advise and I am gonna try the 1G tip

Catarina Mendes Alves e Sousa
Student,
Faculty of Engineering of Porto
Back to top
View user's profile Send private message
Martin Liddle
User


Joined: 15 Aug 2008
Posts: 1274
Location: Chesterfield, UK

PostPosted: Tue Jul 23, 2013 2:16 pm  Reply with quote

On 23/07/2013 21:16, Karl Volkmann wrote:
Quote:
I believe you need to be doing an harmonic analysis with forcing on the main structure and a global 1G acel (be careful with your signs and coords). Your answer makes sense. You simply asked it for natural frequencies, and it gave you natural frequencies.

I thought if you do a harmonic analysis with a gravitational load then
the gravitational load will become harmonic?

--
Martin Liddle, Tynemouth Computer Services,
Chesterfield, Derbyshire, UK.
www.tynecomp.co.uk

Post generated using Mail2Forum (http://www.mail2forum.com)
_________________
Martin Liddle, Tynemouth Computer Services,
Chesterfield, UK.
Back to top
View user's profile Send private message Visit poster's website
Martin Liddle
User


Joined: 15 Aug 2008
Posts: 1274
Location: Chesterfield, UK

PostPosted: Tue Jul 23, 2013 2:18 pm  Reply with quote

On 23/07/2013 21:33, catarina.sousa wrote:
Quote:

My concern in this case is not really the natural frequencies, is more the fact that I'm doing a transient analysis with a sinusoidal force in the two cases (with and without the pendulum) and maximum displacements don't change, but I'm really thankful for the advise and I am gonna try the 1G tip

How many cycles of the transient are you solving for?

--
Martin Liddle, Tynemouth Computer Services,
Chesterfield, Derbyshire, UK.
www.tynecomp.co.uk

Post generated using Mail2Forum (http://www.mail2forum.com)
_________________
Martin Liddle, Tynemouth Computer Services,
Chesterfield, UK.
Back to top
View user's profile Send private message Visit poster's website
karl.volkmann
User


Joined: 27 Jun 2013
Posts: 31

PostPosted: Tue Jul 23, 2013 2:29 pm  Reply with quote

You are probably right, disregard my comment, I thought I read somewhere that she was doing a modal analysis.

Karl Volkmann
Kionix, Inc.

-----Original Message-----
From: xansys-bounces@xansys.org [mailto:xansys-bounces@xansys.org] On Behalf Of Martin Liddle
Sent: Tuesday, July 23, 2013 5:16 PM
To: xansys@xansys.org
Subject: Re: [Xansys] [STRUC]pendulum to minimize displacements in the main struct

On 23/07/2013 21:16, Karl Volkmann wrote:
Quote:
I believe you need to be doing an harmonic analysis with forcing on the main structure and a global 1G acel (be careful with your signs and coords). Your answer makes sense. You simply asked it for natural frequencies, and it gave you natural frequencies.

I thought if you do a harmonic analysis with a gravitational load then the gravitational load will become harmonic?

--
Martin Liddle, Tynemouth Computer Services, Chesterfield, Derbyshire, UK.
www.tynecomp.co.uk

+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
chris.masterson
User


Joined: 10 Jan 2012
Posts: 41

PostPosted: Tue Jul 23, 2013 2:42 pm  Reply with quote

I don't think the pendulum will have any significant impact on displacements if you aren't exciting the structure at the resonant frequency which with a f=0.8Hz would imply a forcing function of 100*sin(2*pi()*0.8*time) I believe?  Your pendulum also would need to be properly tuned to the same frequency.

Chris Masterson
LightSail Energy


On Tue, Jul 23, 2013 at 9:06 AM, catarina.sousa <ec08215@fe.up.pt (ec08215@fe.up.pt)> wrote:
Quote:

The main structure is a simple frame with the mass of : 160,5 kg and lateral stiffness in the x direction of 4050 which gives the natural frequency of 0,79995 confirmed by a modal analysis, after that I've applied a transient analyses with a horizontal sinusoidal force of 100*sin(pi/4*time) and obtain a maximum displacement of 0,028. (this is without the pendulum to have something to compare to)

What I'm struggling with, is the pendulum, i have model it with link180 and mass 21 (with 32.1 of mass)  like in the picture of the link below, (i have done a coupled DOF to simulate a pin joint) and applied the same sinusoidal force and the results stay the same, the don't decrease as I expected (I've tried different lengths and mass for the pendulum and nothing changes)






--
Chris Masterson
Design Manager
LightSail Energy, Inc|www.lightsailenergy.com
Phone: (510) 981-8088 Ext 108
Fax: (510) 981-8286
Email: cmasterson@lightsailenergy.com

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
catarina.sousa
User


Joined: 22 Jul 2013
Posts: 13

PostPosted: Tue Jul 23, 2013 5:42 pm  Reply with quote

So I guess I was making a very basic mistake, because I was tuning the pendulum to is natural frequency but to the one in rad/s w=0.8*2*pi=5,02

I was doing this:

w=(g/l)^1/2
5,02=(9.8/L)^1/2 (finding the lenght of the pendulum this way)

Catarina Mendes Alves e Sousa
Student,
Faculty of Engineering of Porto
Back to top
View user's profile Send private message
catarina.sousa
User


Joined: 22 Jul 2013
Posts: 13

PostPosted: Wed Jul 24, 2013 12:45 pm  Reply with quote

I realised I was tuning the pedulum to the right frequency, that was the 5,02 rad/s

I did exited the structure, this time, to the 100*sin(0.8*2*PI*TIME) load with and without the pendulum and the results of the maximum displacement dont change

I dont know what else to do, I saw the animation again and it seems that the all pendulum was moving (the link) with the main structure, but the free end (where the mass is) almost or didn't move at all, but it makes no sense because there are no constraints in that node.

Catarina Mendes Alves e Sousa,
Student,
Faculty of Engineering of Porto
Back to top
View user's profile Send private message
chris.masterson
User


Joined: 10 Jan 2012
Posts: 41

PostPosted: Wed Jul 24, 2013 1:50 pm  Reply with quote

Did the magnitude of the structural displacement increase due to resonance when the forcing function was tuned properly relative to the improperly tuned forcing function?  And Martin's question still remains - how many cycles of the transient forcing function are you solving?  It takes a few cycles for the resonance to build.

Chris Masterson
LightSail Energy


On Wed, Jul 24, 2013 at 12:45 PM, catarina.sousa <ec08215@fe.up.pt (ec08215@fe.up.pt)> wrote:
Quote:
I realised I was tuning the pedulum to the right frequency, that was the 5,02 rad/s

I did exited the structure, this time, to the 100*sin(0.8*2*PI*TIME) load with and without the pendulum and the results of the maximum displacement dont change

I dont know what else to do, I saw the animation again and it seems that the all pendulum was moving (the link) with the main structure, but the free end (where the mass is) almost or didn't move at all, but it makes no sense because there are no constraints in that node.

Catarina Mendes Alves e Sousa,

Student,
Faculty of Engineering of Porto














--
Chris Masterson
Design Manager
LightSail Energy, Inc|www.lightsailenergy.com
Phone: (510) 981-8088 Ext 108
Fax: (510) 981-8286
Email: cmasterson@lightsailenergy.com

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
catarina.sousa
User


Joined: 22 Jul 2013
Posts: 13

PostPosted: Wed Jul 24, 2013 2:24 pm  Reply with quote

sorry not to have responded immediately to Martins question,
the maximum displacement increase from 0,028 to 0,03182 and in both transient analysis I chose :

"time at end of loadstep->200"
"time increment->1"
"Rampped"

I thought it would be enough..

I was thinking maybe the connection of the pendulum to the horizontal beam188 is poorly made and its causing problems, but I dont very well how to do it other way than Coupled DOFs, a teacher from brasil that I contacted via mail suggested CERIG but I dont know nothing about that, I will have to try to learn by myself.

Catarina Mendes Alves e Sousa,
Student,
Faculty of Engineering of Porto
Back to top
View user's profile Send private message
Martin Liddle
User


Joined: 15 Aug 2008
Posts: 1274
Location: Chesterfield, UK

PostPosted: Wed Jul 24, 2013 3:15 pm  Reply with quote

On 24/07/2013 22:24, catarina.sousa wrote:
Quote:

I was thinking maybe the connection of the pendulum to the horizontal beam188 is poorly made and its causing problems, but I dont very well how to do it other way than Coupled DOFs, a teacher from brasil that I contacted via mail suggested CERIG but I dont know nothing about that, I will have to try to learn by myself.

So tell us exactly how the pendulum is currently connected to the beam.


--
Martin Liddle, Tynemouth Computer Services,
Chesterfield, Derbyshire, UK.
www.tynecomp.co.uk

Post generated using Mail2Forum (http://www.mail2forum.com)
_________________
Martin Liddle, Tynemouth Computer Services,
Chesterfield, UK.
Back to top
View user's profile Send private message Visit poster's website
catarina.sousa
User


Joined: 22 Jul 2013
Posts: 13

PostPosted: Wed Jul 24, 2013 7:26 pm  Reply with quote

What I did was, I selected the coincident nodes, the one from the beginning of the link of the pendulum and one node of the middle of the beam188 and coupled the UX and UY degrees of freedom, and left the rotations uncoupled, i tough that was how the pin joint was simulated.

Catarina Alves e Sousa
Student,
Faculty of Engineering of Porto
Back to top
View user's profile Send private message
Martin Liddle
User


Joined: 15 Aug 2008
Posts: 1274
Location: Chesterfield, UK

PostPosted: Thu Jul 25, 2013 7:08 am  Reply with quote

On 25/07/2013 03:26, catarina.sousa wrote:
Quote:
What I did was, I selected the coincident nodes, the one from the beginning of the link of the pendulum and one node of the middle of the beam188 and coupled the UX and UY degrees of freedom, and left the rotations uncoupled, i tough that was how the pin joint was simulated.

OK sounds reasonable to me. One thought that has occurred to me; do you
have large deflection effects turned on (NLGEOM,ON)? I think this may
be necessary for the pendulum.


--
Martin Liddle, Tynemouth Computer Services,
Chesterfield, Derbyshire, UK.
www.tynecomp.co.uk

Post generated using Mail2Forum (http://www.mail2forum.com)
_________________
Martin Liddle, Tynemouth Computer Services,
Chesterfield, UK.
Back to top
View user's profile Send private message Visit poster's website
frank.exius
User


Joined: 21 Oct 2008
Posts: 50

PostPosted: Thu Jul 25, 2013 7:53 am  Reply with quote

Hello,

some suggestions.

- please, check unit consistency (lenght units , density, E) incl. cross
section and other dimensions
- BEAM188 has only two structural nodes, the third node is a
(crossection)orientation node. Which shouldn't really be used for hooking a
LINK element on to. Make the 2x BEAM's and pin at the node were these met
- reduce time increment to DELTIM,0.8/20 to resolve the exitation frequency,
with 20 points per cycle
- two hundred secs of oscillation at 0.8Hz is 250 cycles. You might want to
cut down end time, e.g. TIME,50: still more then 50x cyles

If the pinned pendulum doesn't provide the desired damping, for the given
design: probably so, as long as there isn't a torsional stiffness & damper
placed at the pinpoint, check
http://www.esss.com.br/events/ansys2013/brazil/pdf/24_4_1510.pdf page 16, Kp
Cp.

Anyway, what percentage of displacement reduction would satisfy the design
target?


Greetings,
Frank Exius

IFE Deutschland
Am Hellenberg 31
53489 Sinzig bei BONN
GERMANY

www.ife-ansys.de
Tel. +49-(0)2642-980409
Geschaeftszeiten Mo-Fr 9:00-18:00 Uhr
Alljaehrliche Betriebsferien im August

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
frank.exius
User


Joined: 21 Oct 2008
Posts: 50

PostPosted: Thu Jul 25, 2013 8:08 am  Reply with quote

sorry:

read "Make the 2x BEAM's" as "Make that 2x BEAM's"

incorrect: two hundred secs of oscillation at 0.8Hz is 250 cycles. You might
want to cut down end time, e.g. TIME,50: still more then 50x cyles
corrected: two hundred secs of oscillation at 0.8Hz is 160 cycles. You might
want to cut down end time, e.g. TIME,50: still 40x cyles

-----Messaggio originale-----
Da: xansys-bounces@xansys.org [mailto:xansys-bounces@xansys.org] Per conto
di xansys
Inviato: giovedė 25 luglio 2013 16.54
A: 'ANSYS User Discussion List'
Oggetto: [Xansys] R: [STRUC]pendulum to minimize displacements in
themainstruct

Hello,

some suggestions.

- please, check unit consistency (lenght units , density, E) incl. cross
section and other dimensions
- BEAM188 has only two structural nodes, the third node is a
(crossection)orientation node. Which shouldn't really be used for hooking a
LINK element on to. Make the 2x BEAM's and pin at the node were these met
- reduce time increment to DELTIM,0.8/20 to resolve the exitation frequency,
with 20 points per cycle
- two hundred secs of oscillation at 0.8Hz is 250 cycles. You might want to
cut down end time, e.g. TIME,50: still more then 50x cyles

If the pinned pendulum doesn't provide the desired damping, for the given
design: probably so, as long as there isn't a torsional stiffness & damper
placed at the pinpoint, check
http://www.esss.com.br/events/ansys2013/brazil/pdf/24_4_1510.pdf page 16, Kp
Cp.

Anyway, what percentage of displacement reduction would satisfy the design
target?


Greetings,
Frank Exius

IFE Deutschland
Am Hellenberg 31
53489 Sinzig bei BONN
GERMANY

www.ife-ansys.de
Tel. +49-(0)2642-980409
Geschaeftszeiten Mo-Fr 9:00-18:00 Uhr
Alljaehrliche Betriebsferien im August

+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
catarina.sousa
User


Joined: 22 Jul 2013
Posts: 13

PostPosted: Thu Jul 25, 2013 7:34 pm  Reply with quote

First of all I want to thank you all for the time spend on this,

Richard,

I took your advice to simply use a node from the meshed beam and conected it to another node to form the link element
I did only use one link element ( I was already doing that, but was good to know that was the right thing to do)

Martin Liddle,

I can not do a large deflection analysis, because all my thesis is based on small angles where sin(a) = a and cos (a)=1

There is no way the pendulum will work on small deflection? (that would really really bad news for me, and I will be in trouble)

Frank,
Actually first of all, all i want to see is some results in deacrising displacements, that would be a really good start

And I did a 0,04 time increment and 60 time of end this time (graphs became much more elucidatory)

Here is my code, it has everything but the force bacause i used the "read from file " option but the force is 100*sin(0.8*PI*TIME) in the top of beam188 (line 1), I still can't make it work....

/PREP7
ET,4,BEAM188
MP,EX,4,20E9
MP,DENS,4,2500
MP,EX,5,200E9
MP,DENS,5,7800

K,1,0,0,, ! keypoints and lines for the frame
K,2,0,2,,
K,3,2,2,,
K,4,2,0,,
L,1,2
L,2,3
L,3,4

SECTYPE,4,BEAM,RECT,BEAM,,
SECDATA,0.03,0.03
SECTYPE,5,BEAM,RECT,BEAM2,,
SECDATA,0.1,0.1

lsel,s,line,,1 ! meching atributtes of lines
LATT,4,,4,,,,4
lsel,s,line,,2
LATT,5,,4,,,,5
lsel,s,line,,3
LATT,4,,4,,,,4
lsel,s,line,,1,3

ESIZE,,10 !meching the main structure
LMESH,ALL

DK,1,UX,0,,UY,UZ,ROTX,ROTY,ROTZ ! here I constrained all dof's to define the suports

DK,4,UX,0,,UY,UZ,ROTX,ROTY,ROTZ

DL,1,,UZ,0,,
DL,2,,UZ,0,, ! here I constrained UZ in all frame to sim a 2D analysis
DL,3,,UZ,0,,
DL,2,,ROTZ,0,, ! here I constrained the rotations to sim a rigid beam
DL,2,,ROTX,0,,

ET,1,LINK180
ET,2,MASS21,,,2

SECTYPE,1,LINK
SECDATA,0.1
R,2,40
MP,EX,1,3E7
N,100,1,1.4,,
E,17,100 ! NODE 17 is the one from the middle of the beam
TYPE,2
REAL,2
E,NODE(1,1.4,,)
SAVE
FINISH


Catarina Mendes Alves e Sousa,
Student,
Faculty of Engineering of Porto
Back to top
View user's profile Send private message
christopher.wright
User


Joined: 17 Jun 2009
Posts: 927

PostPosted: Thu Jul 25, 2013 10:19 pm  Reply with quote

On Jul 25, 2013, at 9:34 PM, catarina.sousa wrote:

Quote:
There is no way the pendulum will work on small deflection? (that
would really really bad news for me, and I will be in trouble)
I've been following this, sort of, since I've done a fair amount of
seismic analysis and some miscellaneous dynamic work over the past 20
years. I really can't figure out what you're trying to do, starting
with the basic physics of what ever it is. What is the pendulum
supposed to do? What does resonance have to do with anything? The
nature of seismic excitation doesn't cause resonance, since there are
relatively few cycles at any one frequency. Is the pendulum you're
trying to model intended to oppose the seismic motion of the
cantilever and reduce the deformation? Can you provide a physical
description of the behavior you're trying to model?

Your explanation and the input file you've attached are very
confusing. To begin with, I don't think you have either the mesh or
the boundary conditions you think you have. You might want to start
with a simple static analysis which you can check manually to make
sure your model is correct. Use 2D beam elements to begin with
instead of 3D elements constrained to planar motion. It looks to me
like you need a lot of practice before you start with transient
analysis. When you do get to transient analysis, skip the pendulum
and apply a forcing function to mimic the motion and frequency of the
pendulum. You can also mimic pendulum with a simple spring mass
system before you try doing an actual free-swinging mass. try taking
small bites out of your problem and teaching yourself as you go.


Christopher Wright P.E. |"They couldn't hit an elephant at
chrisw@skypoint.com | this distance" (last words of Gen.
.......................................| John Sedgwick, Spotsylvania
1864)
http://www.skypoint.com/members/chrisw/

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
catarina.sousa
User


Joined: 22 Jul 2013
Posts: 13

PostPosted: Fri Jul 26, 2013 7:58 am  Reply with quote

What is the pendulum supposed to do? What does resonance have to do with anything? The nature of seismic excitation doesn't cause resonance, since there are relatively few cycles at any one frequency.


I'm sorry but I never said anything about seismic excitation, pendulums are used to prevent large displacements when the frequency of wind causes resonance, because when buildings are very tall a lot of times their frequency is about 0,1 hz and there is a large possibility that the wind will match that frequency and cause resonance. So a pendulum is put on the top of the building.


Your explanation and the input file you've attached are very
confusing. To begin with, I don't think you have either the mesh or
the boundary conditions you think you have. You might want to start
with a simple static analysis which you can check manually to make
sure your model is correct. Use 2D beam elements to begin with
instead of 3D elements constrained to planar motion. It looks to me
like you need a lot of practice before you start with transient
analysis. When you do get to transient analysis, skip the pendulum
and apply a forcing function to mimic the motion and frequency of the
pendulum. You can also mimic pendulum with a simple spring mass
system before you try doing an actual free-swinging mass. try taking
small bites out of your problem and teaching yourself as you go.




I agree the input file is very confusing, and i tried to use 2D elements but for example for the beam BEAM3 (Beam 2D elastic) , but it is no longer supported, and I'm trying to learn how to incorporate a rotational spring, but it isn't easy, and I running againts time. But I'll keep trying

(sorry for my bad english, and for not knowing how to properly quote...) Anyway thank you very much for the reply any help is a help for me right now because I know it takes time to think and write an answer

Catarina Mendes Alves e Sousa,
Student,
Faculty of Engineering of Porto
Back to top
View user's profile Send private message
catarina.sousa
User


Joined: 22 Jul 2013
Posts: 13

PostPosted: Fri Jul 26, 2013 8:19 am  Reply with quote

christopher.wright wrote:
On Jul 25, 2013, at 9:34 PM,

You can also mimic pendulum with a simple spring mass
system before you try doing an actual free-swinging mass. try taking
small bites out of your problem and teaching yourself as you go.


And thanks a lot for this advice, a spring mass system to mimic the pendulum is a great idea, I will try to do a system like that, don't know how yet, but I will try to figure out

Catarina Mendes Alves e Sousa,
Student,
Faculty of Engineering of Porto
Back to top
View user's profile Send private message
karl.volkmann
User


Joined: 27 Jun 2013
Posts: 31

PostPosted: Fri Jul 26, 2013 8:49 am  Reply with quote

Make a really really thin beam with a tiny Young's Mod (so it has almost zero stiffness) and put a brick of stuff at the end of it. It should be trivial to design the beam to be the right stiffness. (or the brick of mass)

Karl Volkmann
Kionix, Inc.

-----Original Message-----
From: xansys-bounces@xansys.org [mailto:xansys-bounces@xansys.org] On Behalf Of catarina.sousa
Sent: Friday, July 26, 2013 11:19 AM
To: xansys@xansys.org
Subject: Re: [Xansys] [STRUC]pendulum to minimize displacements in the main struct


christopher.wright wrote:
Quote:
On Jul 25, 2013, at 9:34 PM,

You can also mimic pendulum with a simple spring mass system before
you try doing an actual free-swinging mass. try taking small bites out
of your problem and teaching yourself as you go.



And thanks a lot for this advice, a spring mass system to mimic the pendulum is a great idea, I will try to do a system like that, don't know how yet, but I will try to figure out

Catarina Mendes Alves e Sousa,
Student,
Faculty of Engineering of Porto






+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
chris.masterson
User


Joined: 10 Jan 2012
Posts: 41

PostPosted: Fri Jul 26, 2013 10:19 am  Reply with quote

Quote:

I can not do a large deflection analysis, because all my thesis is based on small angles where sin(a) = a and cos (a)=1



Turning on large deflection analysis does not imply that your pendulum assumptions are invalid.  A 15 degree swing of your pendulum is a large deflection for the FEA but still meets the pendulum assumptions.


Chris Masterson
LightSail Energy 

--
Chris Masterson
Design Manager
LightSail Energy, Inc|www.lightsailenergy.com
Phone: (510) 981-8088 Ext 108
Fax: (510) 981-8286
Email: cmasterson@lightsailenergy.com

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
christopher.wright
User


Joined: 17 Jun 2009
Posts: 927

PostPosted: Fri Jul 26, 2013 10:42 am  Reply with quote

On Jul 26, 2013, at 9:58 AM, catarina.sousa wrote:

Quote:
I'm sorry but I never said anything about seismic excitation,
pendulums are used to prevent large displacements when the
frequency of wind causes resonance, because when buildings are very
tall a lot of times their frequency is about 0,1 hz and there is a
large possibility that the wind will match that frequency and cause
resonance. So a pendulum is put on the top of the building.

OK--an explanation of the problem is a good start. Sounds like you're
talking about a vortex shedding problem like the one that brought
down the Tacoma Narrows bridge. Or maybe something to do with gust
loading.

First question--
Is the motion of the pendulum intended to impose inertia forces that
counter the periodic loading generated by the wind? I think the
answer is 'yes,' but tell us just to be sure. BTW--don't worry about
using the 2d BEAM3 element. It will make your problem a lot less
complicated and it won't hurt anything.

three more questions--
Is the pendulum just something like a free mass suspended by your
rigid link or is it driven by an actuator or something?
Is the pendulum supposed to go into resonance with the building
frequency?
Am I right in guessing that you're considering the wind load as a
distributed load which varies sinusoidally with time? (You realize
that there's a start-up transient motion and another transient motion
when the wind load dies out--right?)

You're going to have a tough time modeling a suspended mass because
there will be an unrestrained rotational degree of freedom that
allows rigid body motion. I suggest that you model such a thing as a
lumped spring mass system with the mass (MASS21) taken equal to the
suspended mass and the spring (LINK element) taken to provide the
frequency of the pendulum. Put the mass at a generated node
coincident with the node at the end of your cantilever. Connect the
mass to the cantilever with the spring for the horizontal DOF and
couple the remaining DOFs.

Don't do a time history analysis until you're ready for all the
convergence and damping and time step selection issues you'll
encounter. This problem can't be done statically and since it
involves resonance, you should start with a harmonic analysis. You'll
have to read up carefully on the process which requires you do an
eigensolution then apply a harmonic loading corresponding to the
force generated by vortex shedding or whatever your wind loading
might be. The ANSYS docs will show you how to set up a modal analysis
and use the extracted modes to get displacement results. You can also
do the problem where the pendulum is driven into resonance and also
check to see whether a difference in phase between the pendulum
motion and the wind load might make.

After you get comfortable with basic dynamics you can do the problem
in the time domain--just make sure that you give the system enough
time (10-15 times the period of the highest significant frequency) to
get into resonance, and to use enough time steps to capture motion at
the frequencies of interest--say 1/50 of the lowest period of
significant modes. There will be a lot of differences with the time-
history analysis, starting with the starting and stopping transients
I mentioned above. There's also damping and convergence criteria to
check out along with time step size and number of steps. But keep it
simple at first.

It isn't obvious from your posts that you can handle the dynamics
without some practice, so take this in easy steps. I have a favorite
text _Structural Dynamics for the Practising Engineer_ by H. M.
Irvine which you should review before you start anything. There are
some simple examples in this area which you should run through until
you understand them. After you understand the results, try coding
them up with ANSYS to see how the results compare. When you're
comfortable with doing the solved examples and know how to trouble
shoot your mistakes, you can start on your building problem with some
confidence that you can think your way through it.

I can't resist a final comment: It sounds like you've fallen into the
common trap of believing the marketing hype (My Brasilian daughter-in-
law knows just the right word in Portuguese for what I mean) that
ANSYS will do your thinking for you. It won't. ANSYS isn't simple; it
isn't friendly; it isn't intuitive and it won't keep you from making
mistakes. It's a tool, like a chain saw. You can use it on anything
and do great good or great harm. The saw doesn't recognize the
difference between your firewood and your ankle--it cuts right
through both without making value judgments. Like the saw, success
with ANSYS requires practice, judgment and some basic skills. If you
take things slowly, assume nothing, check everything and use each
problem as a learning device, it'll probably start to make sense.


Christopher Wright P.E. |"They couldn't hit an elephant at
chrisw@skypoint.com | this distance" (last words of Gen.
.......................................| John Sedgwick, Spotsylvania
1864)
http://www.skypoint.com/members/chrisw/

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
karl.volkmann
User


Joined: 27 Jun 2013
Posts: 31

PostPosted: Fri Jul 26, 2013 11:48 am  Reply with quote

Quoted for truth:
"I can't resist a final comment: It sounds like you've fallen into the common trap of believing the marketing hype (My Brasilian daughter-in- law knows just the right word in Portuguese for what I mean) that ANSYS will do your thinking for you. It won't. ANSYS isn't simple; it isn't friendly; it isn't intuitive and it won't keep you from making mistakes. It's a tool, like a chain saw. You can use it on anything and do great good or great harm. The saw doesn't recognize the difference between your firewood and your ankle--it cuts right through both without making value judgments. Like the saw, success with ANSYS requires practice, judgment and some basic skills. If you take things slowly, assume nothing, check everything and use each problem as a learning device, it'll probably start to make sense."

One of my profs used to say, "Garbage in, garbage out." It actually shouldn't be too hard to set up a very simplified version of this system, do your FBD's, get some equations, do a Laplace or two and get a back of the envelope solution. (Might need a short Matlab script or Mathematica). A dynamics text I always go to is _System Dynamics (4th ed)_ by Ogata. He's got a pretty good chapter/section on vibration isolation, absorption and damping.

Karl Volkmann
Kionix, Inc.

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
frank.exius
User


Joined: 21 Oct 2008
Posts: 50

PostPosted: Sat Jul 27, 2013 5:59 am  Reply with quote

Hello,

adjust the input:

remove ROTZ at the horizontal beams, so the frame can deflect

set MP,EX,1 & MP,EX,4 to something like 0.8E11 and set MP,DENS,1 & MP,DENS,4
to something like 2700kg if aluminium

for LINK180 define a realistic cross section, as is it defaults to an area
of 1x square meter

the 2x base nodes of the frame do not get a UY constraint, please add


Check that your cyclic force load is introduced as intendet


Adjust the pendulum to the physics of the given design:

tailor your pendulum length such, that it's frequency coincides w the 1st
bending mode of the frame. Such the damping effect will maximize, i.e the
horizontal displaxements UX will get minimized.


Greetings,
Frank Exius

IFE Deutschland
Am Hellenberg 31
53489 Sinzig bei BONN
GERMANY

www.ife-ansys.de
Tel. +49-(0)2642-980409
Geschaeftszeiten Mo-Fr 9:00-18:00 Uhr
Alljaehrliche Betriebsferien im August

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
frank.exius
User


Joined: 21 Oct 2008
Posts: 50

PostPosted: Sat Jul 27, 2013 9:22 am  Reply with quote

Hello+,

are actual deflections large, visible? If yes, set NLGEOM,on as Martin
Liddle suggested. It depends on the load amplitude and resulting
deflections. Which depend on the actual design, dimensions and material
properties.

Talk with your supervisor: is the actual design nonlinear be design. Does it
undergo large deflections in the real world? Then, eventual nonlinear terms
in analytic calcs need be covered. Is the design supposed to behave linear?
Might necessitate increased stiffeness. And impede efficient damping (small
deflections, small pendulum motions, small damping effect).

Greetings,
Frank Exius

IFE Deutschland
Am Hellenberg 31
53489 Sinzig bei BONN
GERMANY

www.ife-ansys.de
Tel. +49-(0)2642-980409
Geschaeftszeiten Mo-Fr 9:00-18:00 Uhr
Alljaehrliche Betriebsferien im August

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
catarina.sousa
User


Joined: 22 Jul 2013
Posts: 13

PostPosted: Sat Jul 27, 2013 12:26 pm  Reply with quote

Well thanks again for the time, the advices and the references of good theoretical texts.

christopher.wright

I don't think I can use the BEAM3, the new versions of ansys don't allow it ( at least I couldn't make it work)

The pendulum is a free mass suspended and it is suppose to have the optimum parameters that is :

a=W(from pendulum)/W(structure)
a=1/(1+u)

u being the relation between the mass of the pendulum and the mass of structure

(don't know if my explanation is clear enough)

Frank.exius

Thanks a lot for the carefull look at my code!

I actually want the frame to be a shear frame, so the horizontal beams behave like rigid and dont deflect

My work is based on the approximation sin(z)=z and cos(z)=1, linear behavior

what I dont know is if the NLGEOM, ON invalidates those assumptions above
chris.masterson said that it doesn't invalidates, if its is like chris says it would be good because with NLGeom on I get some results in the decreasing I want

Another question, that might be very stupid, is can the NLGEOM be considered just for the pendulum and not for the frame? i guees not...

Catarina Mendes Alves e Sousa
Student,
Faculty of Egineering of Porto
Back to top
View user's profile Send private message
jose.galan
User


Joined: 21 Oct 2008
Posts: 140

PostPosted: Sun Jul 28, 2013 2:34 pm  Reply with quote

By the way, have you activated Pstres,on? Link elements do not have bending stiffness unless they are prestressed (tractioned). I suggest that you solve the simple problem of your pendulum alone, hanging from a fixed point, and calculate its natural frequencies. You will not obtain omega=sqrt(g/L), as you would expect, unless you previously solve a static problem with gravity loading and pstres,on, and Then solve a prestressed modal analysis, with pstres,on. There is a nice post in xansys by Thomas A. Wall (from 15 nov 2007) that Explains this quite well and includes an example code. Here I include a copy of Mr. Wall's post; I think that Mr. Wall would not mind. Best regards, Jose M. Galan Assistant Professor Dept. Engineering Construction Universidad de Sevilla OK now that everyone has chimed in to tell you that you can't do it with a modal analysis, here's how to do it. If you do a pre-stressed modal analysis, you can get the natural frequency of a pendulum. Try the follow commands and see for yourself. This gives three modes (well, really only two since one is repeated at 90 degrees): two for the pendulum swinging and the other for stretching of the "string". You can effectively eliminate the string stretching mode by using a very large stiffness (like 1E20), or you can add other string modes if you increase its mass. !----------------------------------------------------------------------- !----------------------------------------------------------------------- finish /clear,start !----------------------------------------------------------------------- /TITLE, Pre-stressed Modal analysis pendulum /PREP7 ET,1,link10 R,1,1.00e-3 MP,EX,1,10 MP,DENS,1,1E-9 ET,2,MASS21 KEYOPT,2,3,2 R,2,1.2583 K,1,0,0,0 K,2,0,-30,0 L,1,2 LATT,1,1,1 ESIZE,,10 LMESH,ALL TYPE,2 REAL,2 E,NODE(0,-30,0) DK,1,UX,,,,UY,UZ ACEL,,9.81 !----------------------------------------------------------------------- /SOLU ANTYPE,STATIC PSTRES,ON /STATUS,SOLU SOLVE FINISH /SOLU ANTYPE,MODAL MODOPT,LANB,5 MXPAND,5 LUMPM,0 PSTRES,1 SOLVE FINISH !----------------------------------------------------------------------- !----------------------------------------------------------------------- PS. I didn't actually write this code myself, but I do know how to search the internet which is where I found this. __________________ Thomas A. Wall Rock Solutions Group -----Original Message----- From: --email address suppressed-- [mailto:--email address suppressed--] On Behalf Of Balasubramanian Ram Sent: Thursday, November 15, 2007 2:41 PM To: --email address suppressed-- Subject: [XANSYS][STRU] Natural frequency of a simple pendulum Dear Experts, I've a question, which is more academic but of vital practical importance too. I'm trying to find the natural frequency of a simple pendulum in ANSYS. I have modeled the pendulum with BEAM3 and MASS21 . I've arrested the translational dofs at one end of the beam. I'm performing a modal analysis to extract the frequency. But in this regard, I've some doubts, As we know, the natural frequency of a simple pendulum is only a function of its length and gravity. So, it is independant of the cross-section of the link, mass , material etc., how to exactly simulate this in ANSYS?. Do I need to explicitly specify "g"? ( which is not feasible in modal analysis) Can anybody throw some light on this. Kindly excuse me , if this question is very fundamental for FEA. Thanks & Regards, Ram Balasubramanian Senior Engineer - CAE, Chennai, India. -- Well thanks again for the time, the advices and the references of good theoretical texts. christopher.wright I don't think I can use the BEAM3, the new versions of ansys don't allow it ( at least I couldn't make it work) The pendulum is a free mass suspended and it is suppose to have the optimum parameters that is : a=W(from pendulum)/W(structure) a=1/(1+u) u being the relation between the mass of the pendulum and the mass of structure (don't know if my explanation is clear enough) Frank.exius Thanks a lot for the carefull look at my code! I actually want the frame to be a shear frame, so the horizontal beams behave like rigid and dont deflect My work is based on the approximation sin(z)=z and cos(z)=1, linear behavior what I dont know is if the NLGEOM, ON invalidates those assumptions above chris.masterson said that it doesn't invalidates, if its is like chris says it would be good because with NLGeom on I get some results in the decreasing I want Another question, that might be very stupid, is can the NLGEOM be considered just for the pendulum and not for the frame? i guees not... Catarina Mendes Alves e Sousa Student, Faculty of Egineering of Porto

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
carl.mally
User


Joined: 21 Oct 2008
Posts: 120

PostPosted: Mon Jul 29, 2013 6:48 am  Reply with quote

Quote:
Quote:
Another question, that might be very stupid, is can the NLGEOM be considered just for the pendulum and not for the frame? i guees not...<<

If turning on large deflection affects the results noticeably then your small deflection assumption is not right anyway. If the physics of your problem are large deflection then assuming it is small deflection does not make the real world behave that way. The small deflection assumption only works if the actual deflections are small and the out of plane effects are insignificant. If the deflections really are small then the large deflection case will match the small deflection case anyway.


Carl Mally
Product Development Engineer
Centro Inc.
950 North Bend Drive
North Liberty, IA 52317

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
jose.galan
User


Joined: 21 Oct 2008
Posts: 140

PostPosted: Tue Jul 30, 2013 3:13 am  Reply with quote

Dear all,
I am sorry for the terrible typesetting of my previous post; I was writing from my cell phone.
Here I send you the link to the old xansys discussion about calculating the natural frequency of a pendulum with ansys ([XANSYS][STRU] Natural frequency of a simple pendulum). Please, read Thomas A. Wall's post (it is 9th in the list). It was the one that I included in my previous message, but the bad typesetting made it almost unreadable.
http://xansys.org/forum/viewtopic.php?p=67319&sid=80971a89f369f0514af83138a13ae363
Best regards,
Jose M. GalanAssistant Professor Dept. Engineering Construction Universidad de Sevilla Spain

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
jose.galan
User


Joined: 21 Oct 2008
Posts: 140

PostPosted: Tue Jul 30, 2013 12:09 pm  Reply with quote

I agree with Mr. Mally.

However, the stress-stiffening (or geometric stiffening) effect can be
included
in both linear and nonlinear analysis. You can include the geometric
stiffness
matrix in your ansys calculations by performing a prestressed analysis.
In the
ansys manual you can find the procedure for several types of
prestressed
analysis: prestressed modal analysis, prestressed harmonic response
analysis
and prestressed transient analysis.


In the case of a truss (LINK8) element, the linear stiffness matrix has
the
following components (using matlab syntax):

K2=E*A/L*[1 0 0;0 0 0;0 0 0];

Klin=[K2 -K2;-K2 K2];

This linear matrix only has stiffness in the axial direction of the
truss. This
element does not provide any stiffness in any direction perpendicular
to the
line element ("out-of-plane" stiffness).

The stress stiffness matrix (or geometric stiffness matrix) of the
truss
element under small rotations has the following components (using
matlab syntax):

K1=F/L*[0 0 0; 0 1 0; 0 0 1];

Kgeom= [K1 -K1;-K1 K1];

where F is the tractional force in the element, due to a prestressing
static
loading, and L is the element length. You can find the derivation of
this
matrix in Przemieniecki, J. S., Theory of Matrix Structural Analysis,
McGraw-
Hill, New York (1968), or in its Dover reprint. As you can see, when
the link
element is under traction, it offers an "out-of-plane" stiffness
proportional
to F/L in both directions perpendicular to the link element.

The total stiffness matrix is the sum of both matrices.

K=Klin+Kgeom


You can make a pendulum with a vertical massless LINK8 element of
length L,
fixed in its top end, with a point mass m in the bottom end (MASS21
without
rotary inertia, keyopt(2)=2). This model has only 3 degrees of freedom
(d.o.f),
i.e. the 3 displacements of the mass (Ux, Uy, Uz). This is similar to
what
Catarina did in her model (except that she connected the top node to
the structure).
The (3x3) mass matrix M is diagonal, and has the following expression
(using matlab notation):

M=m*eye(3);

The (3x3) stiffness matrix is also a diagonal matrix, with the
following expression:

K=K2+K1= [F/L 0 0; 0 F/L 0; 0 0 E*A/L];

The differential equation that governs the free vibration of the system
is:

(K- w^2 M)*d*exp(i*w*t)=0

where d is the (3x1) vector containing the (ux,uy,uz) displacements of
the mass.
The 3 equations are uncoupled, and this problem can be solved easily.
The natural frequencies are the solution of det(K-w^2 M)=0, which in
this case
have very simple expressions:

* One natural frequency corresponding to a vertical vibration of the
mass:
w_vert=sqrt(E*A/(L*m)), in rad/s.

* Two coincident natural frequencies, corresponding to horizontal
vibration of
the mass: w_horiz=sqrt((F/L)/m)=sqrt(m* g/(L*m))=sqrt(g/L). This is the
classical solution for the the natural frequency of a pendulum under
small
amplitude vibrations. However, to obtain this result you need to
include the
geometric stiffness matrix. In ansys, this is done by following the
procedure
described in presstressed modal analysis, which requires two solution
steps
with PSTRES,ON: first, perform a static analysis under gravity loading
with
PSTRES,ON; second, perform a modal analysis using PSTRES,ON to include
the
geometric stiffness matrix.


If you perform a modal analysis without the geometric stiffness matrix
(which
is the default option in ansys), then F=0, and the stiffness matrix of
the
pendulum will have two zero elements in the diagonal (corresponding to
stiffnesses against horizontal displacements). When calculating the
natural
modes, you will obtain two rigid body modes (corresponding to the mass
moving
in both horizontal directions, where there is zero stiffness), and the
same
vertical mode with the same natural frequency. w_vert=sqrt(E*A/(L*M)).
You do
not obtain the natural frequency of oscillation of the pendulum that
you are
trying to model, omega_pend=sqrt(g/L). What is missing here? The stress
stiffness matrix.




Catarina, I think that your problem is that your numerical model does
not
reproduce the real behaviour of your system.

You said in a previous post that you were not interested in calculating
the
natural frequencies of your system, that you only wanted to obtain its
transient dynamic response. However, unless the natural frequencies are
well
represented, your model will not reproduce the real dynamic response of
your
system. Therefore, you should first determine the natural frequencis to
make
sure that they are correct.

I think that you should calculate the natural frequencies of the
structure
withouth pendulum, of the pendulum alone, and of the structure with the
pendulum attached. Since you are using the pendulum as a tuned mass
damper, you
have to make sure that the natural frequency of the pendulum alone is
equal to
one of the natural frequencies of the structure alone.


Best regards,

Jose M. Galan
Assistant Professor
Dept. Engineering Construction
Universidad de Sevilla
Spain

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
jose.galan
User


Joined: 21 Oct 2008
Posts: 140

PostPosted: Tue Jul 30, 2013 12:13 pm  Reply with quote

Regarding my previous post, you can check the following sections of the manual:
Theory Reference | Chapter 3. Structures with Geometric Nonlinearities | 3.4. Stress StiffeningStructural Guide | Chapter 8. Nonlinear Structural Analysis | 8.3.2. Stress Stiffening Structural Guide | Chapter 5. Transient Dynamic Analysis | 5.8. Performing a Prestressed Transient Dynamic AnalysisStructural Guide | Chapter 3. Modal Analysis | 3.10. Prestressed Modal Analysis
Best regards, Jose M. Galan Assistant Professor Dept. Engineering Construction Universidad de Sevilla Spain

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
catarina.sousa
User


Joined: 22 Jul 2013
Posts: 13

PostPosted: Tue Jul 30, 2013 12:29 pm  Reply with quote

Thank you very very mush Professor Jose M. Galan!!

I will read all this carefully!
Actually I had already tried to use the prestressed code from the other topic forum, I but never had the ideia to use it to confirm the frequency! It's an excelent ideia to know if I have the pendulum I think I have!

I will read everyting again with carefull but I wanted to thank you in advance!

Catarina Mendes Alves e Sousa
Student,
Faculty of Engineering of Porto
Back to top
View user's profile Send private message
catarina.sousa
User


Joined: 22 Jul 2013
Posts: 13

PostPosted: Thu Aug 01, 2013 3:36 pm  Reply with quote

christopher.wright wrote:
On Jul 26, 2013, at 9:58 AM, catarina.sousa wrote:

Put the mass at a generated node
coincident with the node at the end of your cantilever. Connect the
mass to the cantilever with the spring for the horizontal DOF and
couple the remaining DOFs.



I was reading everything carefully and
I'm sorry but I didn't understand this part, could you explain better?

Thank you in advance

Catarina Sousa,
Student,
Faculty of Engineering of Porto
Back to top
View user's profile Send private message
christopher.wright
User


Joined: 17 Jun 2009
Posts: 927

PostPosted: Thu Aug 01, 2013 9:03 pm  Reply with quote

On Aug 1, 2013, at 5:36 PM, catarina.sousa wrote:

Quote:
I was reading everything carefully and
I'm sorry but I didn't understand this part, could you explain better?

What you need is another node to define the mass of the pendulum. So
you generate the node and use it to define a lumped mass with the
MASS21 element type. Then you need to attach that node to the end of
the cantilever with a spring. You can use COMBIN7 or COMBIN14, I
think--check the docs

Make the mass element coincident with the end of the beam: use the
NGEN command with all the geometric offsets equal to zero, Define the
spring rate with the proper degree of freedom (UX, UY or UZ) to
correspond with the pendulum movement you want. Then couple (CP,...)
the mass and the end of the cantilever in all the remaining degrees
of freedom.

That's about the best I can do.


Christopher Wright P.E. |"They couldn't hit an elephant at
chrisw@skypoint.com | this distance" (last words of Gen.
.......................................| John Sedgwick, Spotsylvania
1864)
http://www.skypoint.com/members/chrisw/

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
Display posts from previous:   
This forum is locked: you cannot post, reply to, or edit topics.   This topic is locked: you cannot edit posts or make replies.    XANSYS Forum Index -> XANSYS
All times are GMT - 7 Hours
Page 1 of 1

 
Jump to:  
You cannot post new topics in this forum
You cannot reply to topics in this forum
You cannot edit your posts in this forum
You cannot delete your posts in this forum
You cannot vote in polls in this forum
You cannot attach files in this forum
You cannot download files in this forum


Powered by phpBB © 2001, 2005 phpBB Group

sleek template created by Andrew Charron