XANSYS Forum Index
    Register    

FAQ    Search    Memberlist    Usergroups    SmartFeedSmartFeed    Profile    Log in
[Xansys] [STRUC] Displacement in Modal analysis
 
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
paris.altidis
User


Joined: 21 Oct 2008
Posts: 398
Location: Melrose Park, IL

PostPosted: Wed Apr 01, 2009 12:15 pm  Reply with quote

Try,
/dsca,,1 ! Reset plot/animation scale

and replot


Paris Altidis
BELCAN Engineering Group
Adv. Engineering & Technology Division
630-786-0008






-----Original Message-----
From: --email address suppressed-- [mailto:--email address suppressed--] On
Behalf Of Tong, Fung
Sent: Wednesday, April 01, 2009 11:02 AM
To: --email address suppressed--
Subject: [Xansys] [STRUC] Displacement in Modal analysis

Hi Ansys users,

I am conducting a modal analysis on a Double-walled Carbon Nanotube
(DWCNT) consisting of two coaxial circular cyclinder of different radii,
as you can imagine, one overlapping the other.There's a gap between the
inner and outer cylinder walls which consist of the van der Waals
interaction (characterised by linear spring elements) between the walls.
After solving the analysis, the deformation plot of the vibration mode
shows that the inner wall penetrates the outer wall. This is impossible
because as the inner and outer walls gets closer together, the van der
Waals forces becomes infinitely large.

So, I recalled from...Post: [XANSYS] [STRUC] Critical linear buckling
strain; Date: 13th May 2008 (replies from J. Galan and C. Wright)...that
in a linear eigenvalue buckling analysis, the displacement/strain is an
arbitriary value. I suppose that is the same with a modal analysis
(displacements/strains are also arbitriary)? If so, then I could simply
reduce the deformation scaling of the vibration mode (and avoiding the
use of contact analysis). Can someone shed a light or advice on this?
Thanks!

Note: assume that there's no critical issues relating the material
props, stiffness of spring element, geometry, mesh and solution options.
Even the frequencies captured agrees with the experiemental data.

Regards

Fung Tong
Graduate Engineer, Rail Solutions Western

ATKINS
3rd Floor, Longcross Court, 47 Newport Road, Cardiff, CF24 0AD

Tel: +44 (0) 2920 358193

Fax: +44 (0) 2920 48 5138

E-mail: --email address suppressed--

Web: www.atkinsglobal.com



This email and any attached files are confidential and copyright
protected. If you are not the addressee, any dissemination of this
communication is strictly prohibited. Unless otherwise expressly agreed
in writing, nothing stated in this communication shall be legally
binding.

The ultimate parent company of the Atkins Group is WS Atkins plc.
Registered in England No. 1885586. Registered Office Woodcote Grove,
Ashley Road, Epsom, Surrey KT18 5BW. A list of wholly owned Atkins Group
companies registered in the United Kingdom can be found at
http://www.atkinsglobal.com/terms_and_conditions/index.aspx

Consider the environment. Please don't print this e-mail unless you
really need to.
^----------------------------------------------------
| XANSYS web - www.xansys.org |
| XANSYS blog - xansys.blogspot.com |
| The Online Community for users |
| of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
^----------------------------------------------------


This e-mail transmission contains information that is confidential and may be
privileged. It is intended only for the addressee(s) named above. If you receive
this e-mail in error, please do not read, copy or disseminate it in any manner.
If you are not the intended recipient, any disclosure, copying, distribution or
use of the contents of this information is prohibited. Please reply to the
message immediately by informing the sender that the message was misdirected.
After replying, please erase it from your computer system. Your assistance in
correcting this error is appreciated.

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


Joined: 21 Oct 2008
Posts: 6
Location: Cardiff, UK

PostPosted: Wed Apr 01, 2009 2:43 pm  Reply with quote

Hi Paris, thanks for the input.

I've just tried that. It scales the deformation to 1.0 (true scale) and it results in EXTREMELY (unrealistic) deformed shape, which could suggest that the deformation in a modal analysis is arbitriary rather than real.

However, still need to be certain of this...

Regards
Fung Tong
Graduate Engineer, Rail Solutions Western

ATKINS
3rd Floor, Longcross Court, 47 Newport Road, Cardiff, CF24 0AD
Tel: +44 (0) 2920 358193
Fax: +44 (0) 2920 48 5138
E-mail: --email address suppressed--
Web: www.atkinsglobal.com

[quote="paris.altidis"]Try,
/dsca,,1 ! Reset plot/animation scale

and replot


Paris Altidis
BELCAN Engineering Group
Adv. Engineering & Technology Division
630-786-0008






-----Original Message-----
From: --email address suppressed-- [mailto:--email address suppressed--] On
Behalf Of Tong, Fung
Sent: Wednesday, April 01, 2009 11:02 AM
To: --email address suppressed--
Subject: [Xansys] [STRUC] Displacement in Modal analysis

Hi Ansys users,

I am conducting a modal analysis on a Double-walled Carbon Nanotube
(DWCNT) consisting of two coaxial circular cyclinder of different radii,
as you can imagine, one overlapping the other.There's a gap between the
inner and outer cylinder walls which consist of the van der Waals
interaction (characterised by linear spring elements) between the walls.
After solving the analysis, the deformation plot of the vibration mode
shows that the inner wall penetrates the outer wall. This is impossible
because as the inner and outer walls gets closer together, the van der
Waals forces becomes infinitely large.

So, I recalled from...Post: [XANSYS] [STRUC] Critical linear buckling
strain; Date: 13th May 2008 (replies from J. Galan and C. Wright)...that
in a linear eigenvalue buckling analysis, the displacement/strain is an
arbitriary value. I suppose that is the same with a modal analysis
(displacements/strains are also arbitriary)? If so, then I could simply
reduce the deformation scaling of the vibration mode (and avoiding the
use of contact analysis). Can someone shed a light or advice on this?
Thanks!

Note: assume that there's no critical issues relating the material
props, stiffness of spring element, geometry, mesh and solution options.
Even the frequencies captured agrees with the experiemental data.

Regards

Fung Tong
Graduate Engineer, Rail Solutions Western

ATKINS
3rd Floor, Longcross Court, 47 Newport Road, Cardiff, CF24 0AD

Tel: +44 (0) 2920 358193

Fax: +44 (0) 2920 48 5138

E-mail: --email address suppressed--

Web: www.atkinsglobal.com



This email and any attached files are confidential and copyright
protected. If you are not the addressee, any dissemination of this
communication is strictly prohibited. Unless otherwise expressly agreed
in writing, nothing stated in this communication shall be legally
binding.

The ultimate parent company of the Atkins Group is WS Atkins plc.
Registered in England No. 1885586. Registered Office Woodcote Grove,
Ashley Road, Epsom, Surrey KT18 5BW. A list of wholly owned Atkins Group
companies registered in the United Kingdom can be found at
http://www.atkinsglobal.com/terms_and_conditions/index.aspx

Consider the environment. Please don't print this e-mail unless you
really need to.
^----------------------------------------------------
| XANSYS web - www.xansys.org |
| XANSYS blog - xansys.blogspot.com |
| The Online Community for users |
| of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
^----------------------------------------------------


This e-mail transmission contains information that is confidential and may be
privileged. It is intended only for the addressee(s) named above. If you receive
this e-mail in error, please do not read, copy or disseminate it in any manner.
If you are not the intended recipient, any disclosure, copying, distribution or
use of the contents of this information is prohibited. Please reply to the
message immediately by informing the sender that the message was misdirected.
After replying, please erase it from your computer system. Your assistance in
correcting this error is appreciated.

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


Joined: 21 Oct 2008
Posts: 140

PostPosted: Thu Apr 02, 2009 1:49 am  Reply with quote

Dear Fung,

you have approximated the non-linear van der Waals forces by a linear spring. This linearization is only valid in a certain range of displacements, which is smaller than the gap between the cylinders. For small vibration amplitudes (smaller than the gap), your linear approximation will be a very good representation of the real behaviour. Therefore, the vibration modes that you have obtained are valid as long as the linear approximation is correct.

Ansys makes an automatic scaling of the vibration modes for visualization purposes. As you point out, the interpenetration that you observe is just a result of a large scale factor applied to modal displacements in the visualization. You can manually adjust this scale factor by using the command /DSCALE,,scale_factor

Best regards,

Jose M. Galan
Department of Construction Engineering
Escuela Tecnica Superior de Ingenieros
University of Sevilla
Spain



Date sent:              Wed, 01 Apr 2009 17:02:12 +0100
From:                     "Tong, Fung " <--email address suppressed-->
Subject:                 [Xansys] [STRUC] Displacement in Modal analysis
To:                         --email address suppressed--
Send reply to:        ANSYS User Discussion List <--email address suppressed-->

> Hi Ansys users,
>
> I am conducting a modal analysis on a Double-walled Carbon Nanotube
> (DWCNT) consisting of two coaxial circular cyclinder of different
> radii, as you can imagine, one overlapping the other.There's a gap
> between the inner and outer cylinder walls which consist of the van
> der Waals interaction (characterised by linear spring elements)
> between the walls. After solving the analysis, the deformation plot of
> the vibration mode shows that the inner wall penetrates the outer
> wall. This is impossible because as the inner and outer walls gets
> closer together, the van der Waals forces becomes infinitely large.
>
> So, I recalled from...Post: [XANSYS] [STRUC] Critical linear buckling
> strain; Date: 13th May 2008 (replies from J. Galan and C.
> Wright)...that in a linear eigenvalue buckling analysis, the
> displacement/strain is an arbitriary value. I suppose that is the same
> with a modal analysis (displacements/strains are also arbitriary)? If
> so, then I could simply reduce the deformation scaling of the
> vibration mode (and avoiding the use of contact analysis). Can someone
> shed a light or advice on this? Thanks!
>
> Note: assume that there's no critical issues relating the material
> props, stiffness of spring element, geometry, mesh and solution
> options. Even the frequencies captured agrees with the experiemental
> data.
>
> Regards
>
> Fung Tong
> Graduate Engineer, Rail Solutions Western
>
> ATKINS
> 3rd Floor, Longcross Court, 47 Newport Road, Cardiff, CF24 0AD
>
> Tel: +44 (0) 2920 358193
>
> Fax: +44 (0) 2920 48 5138
>
> E-mail: --email address suppressed--
>
> Web: www.atkinsglobal.com
>
>
>
> This email and any attached files are confidential and copyright
> protected. If you are not the addressee, any dissemination of this
> communication is strictly prohibited. Unless otherwise expressly
> agreed in writing, nothing stated in this communication shall be
> legally binding.
>
> The ultimate parent company of the Atkins Group is WS Atkins plc.
> Registered in England No. 1885586.  Registered Office Woodcote Grove,
> Ashley Road, Epsom, Surrey KT18 5BW. A list of wholly owned Atkins
> Group companies registered in the United Kingdom can be found at
> http://www.atkinsglobal.com/terms_and_conditions/index.aspx
>
> Consider the environment. Please don't print this e-mail unless you
> really need to. ^----------------------------------------------------
> |           XANSYS web - www.xansys.org             | |        XANSYS
> blog - xansys.blogspot.com          | |          The Online Community
> for users           | |            of ANSYS, Inc. Software           
>    | |         Hosted by PADT - www.padtinc.com          |
> ^----------------------------------------------------
>

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


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

PostPosted: Thu Apr 02, 2009 2:59 am  Reply with quote

In message <--email address suppressed-->, fung.tong
<--email address suppressed--> writes
>
>I've just tried that. It scales the deformation to 1.0 (true scale) and
>it results in EXTREMELY (unrealistic) deformed shape, which could
>suggest that the deformation in a modal analysis is arbitriary rather
>than real.
>
>However, still need to be certain of this...
>
Beyond all doubt the deformation from a modal analysis is arbitrary.
--
Martin Liddle, Tynemouth Computer Services, 3 Kentmere Way,
Staveley, Chesterfield, Derbyshire, S43 3TW.
Web site: <http://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
ravindra.bhide
User


Joined: 21 Oct 2008
Posts: 6
Location: Mumbai

PostPosted: Thu Apr 02, 2009 3:41 am  Reply with quote

Dear ANSYS Experts,

I am Ravindra Bhide, Senior Research Scholar from Indian Institute of
Technology Bombay, India. We are teaching Finite Element Methods
(applicable to EMAG) to undergraduate students, in which we want them to
develop their own programs in MATLAB and then validate their results in
ANSYS.

One simple problem given to students is "force computation between two
circular coils". It is an axi-symmetric, magneto-static problem, in which
applied loads are current densities assigned to cross-sections of both the
coils. There is no highly permeable material in the problem domain (i.e.,
MURX=1 for surrounding as well as for coil domain). The force is computed
by setting flag (FMAGBC) to cross-sections of the coils and it is matching
with the practical solution of 76.6 mN.

I have also computed (J cross B) for each coil cross-section using ETABLE.
X-component of force density (say, FXD) is computed by multiplying JTZ and
BY of every element, and Y-component of force density (say, FYD) is
computed by multiplying JTZ and BX. Finally, X and Y components of forces
are computed by multiplying VOLU to FXD and FYD, respectively. This will
give us forces on each element. To compute total force, I did the
summation of FX and FY terms in ETABLE.

The results obtained by FMAGSUM shows good agreement only to the summation
of FY in ETABLE (i.e., 76.6 mN). But, then, what is the significance of
the summation of FX in ETABLE. The value of this summation is much higher
than the desired value (i.e., 0.26 N).

Please guide me what I am missing in the analysis.
The APDL code is very small and hence pasted here with this mail.

----------------------------
finish
/clear,nostart
/prep7
et,1,plane53,,,1, !* axi-symmetric option
mp,murx,1,1
mp,murx,2,1
mp,murx,3,1
!*
rectng,0,0.2,0,0.46
rectng,0.05,0.06,0.20,0.21
rectng,0.05,0.06,0.25,0.26
alls
aovlap,all
aglue,all
numcmp,area,all
asel,s,area,,1,,,1,
aatt,1,1,1
asel,s,area,,2,,,1,
aatt,2,2,1
asel,s,area,,3,,,1,
aatt,3,3,1
alls
asel,s,area,,1,2,1,1,
aesize,all,1e-03
mshape,1,2d
amesh,all
asel,s,area,,3,,,1,
aesize,all,20e-03
mshape,1,2d
amesh,all
alls
/pnum,mat,1
/number,1
eplot
esel,s,mat,,1,,,1
cm,con_1,elem
bfe,all,js,1,,,3e06
esel,s,mat,,2,,,1
cm,con_2,elem
bfe,all,js,1,,,3e06
fmagbc,'con_1','con_2',
lsel,s,line,,1,4,1,1,
lplot
dl,all,,asym
/solu
alls
solve
save
finish
-----------------------------------------------

Thanks in advance!

Thanks and Regards,
--
Ravindra S. Bhide
Senior Research Scholar
Dept of Electrical Engineering
IIT Bombay
mob-98671 92404
off-02225764424

Post generated using Mail2Forum (http://www.mail2forum.com)
_________________
Ravindra S. Bhide
Research Scholar
Department of Electrical Engineering
Indian Institute of Technology Bombay,
Powai,Mumbai, India
Mob:- +(91)-9867192404
Off:- +(91)-(22)-25764424
Back to top
View user's profile Send private message Send e-mail Visit poster's website Yahoo Messenger
jose.galan
User


Joined: 21 Oct 2008
Posts: 140

PostPosted: Thu Apr 02, 2009 3:59 am  Reply with quote

Dear Fung,
I think that you should review the basics of vibration theory. You should be absolutely certain that a modal analysis gives you natural frequencies and mode shapes only. The eigenmode amplitudes are unknown and could be chosen arbitrarily. However, since modal analysis is usually performed prior to a Mode Superposition Harmonic Response Analysis, the eigenmode amplitudes are chosen in a way which facilitates that next step. This procedure is known as mode shape normalization.


With the MODOPT command you can choose between two altenative ways to normalize mode shapes (See the Manual: Theory Reference (theory_toc.html)  | Chapter 17. Analysis Procedures (thy_anproc.html)  | 17.3. Mode-Frequency Analysis): (a) by default, eigenmodes are normalized to the mass matrix, that is, transpose(phi_i)*M*phi_j=delta_ij, where phi_i is the ith eigenvector, M is the mass matrix, and delta_ij is the Kronecker delta function (1 if i=j, otherwise 0).

(b) eigenmodes can be normalized to unity, which means that "phi_i is normalized such that its largest component is 1.0 (unity)" (taken from the Ansys manual).
Let us assume that your modes are normalized to unity. If we also assume that you are using mm as the unit to input your distances in ansys, then your mode shapes have displacements between -1mm and 1mm. I do not know how large is the gap between the cylinders, let us assume that it is 0.1mm. In that case, if you plot your mode with a scale factor of 1, you will be likely to see interpenetration (depending on the mode shape). The solution is to apply a scale factor smaller that unity, with the following commands:
gap=0.1
scale_factor=0.8*gap /Dscale,,scale_factor

With these commands you will not see any interpenetration, as long as the modes are normalized to unity. If they were normalized to the mass matrix, you should adjust the scale factor manually to a value small enought to avoid seeing interpenetration.
Best regads,

Jose M. Galan
Department of Construction Engineering
Escuela Tecnica Superior de Ingenieros
University of Sevilla
Spain


Date sent:                 Wed, 01 Apr 2009 15:43:57 -0600
From:                       "fung.tong" <--email address suppressed-->
Subject:                    Re: [Xansys] [STRUC] Displacement in Modal analysis
To:                           --email address suppressed--
Send reply to:           ANSYS User Discussion List <--email address suppressed-->

> Hi Paris, thanks for the input.
>
> I've just tried that. It scales the deformation to 1.0 (true scale)
> and it results in EXTREMELY (unrealistic) deformed shape, which could
> suggest that the deformation in a modal analysis is arbitriary rather
> than real.
>
> However, still need to be certain of this...
>
> Regards
> Fung Tong
> Graduate Engineer, Rail Solutions Western
>
> ATKINS
> 3rd Floor, Longcross Court, 47 Newport Road, Cardiff, CF24 0AD
> Tel: +44 (0) 2920 358193
> Fax: +44 (0) 2920 48 5138
> E-mail: --email address suppressed--
> Web: www.atkinsglobal.com
>
>
paris.altidis wrote:
Try,
> /dsca,,1 ! Reset plot/animation scale
>
> and replot
>
>
> Paris Altidis
> BELCAN Engineering Group
> Adv. Engineering & Technology Division
> 630-786-0008
>
>
>
>
>
>
> -----Original Message-----
> From: --email address suppressed-- [mailto:--email address
> suppressed--] On Behalf Of Tong, Fung Sent: Wednesday, April 01, 2009
> 11:02 AM To: --email address suppressed-- Subject: [Xansys] [STRUC]
> Displacement in Modal analysis
>
> Hi Ansys users,
>
> I am conducting a modal analysis on a Double-walled Carbon Nanotube
> (DWCNT) consisting of two coaxial circular cyclinder of different
> radii, as you can imagine, one overlapping the other.There's a gap
> between the inner and outer cylinder walls which consist of the van
> der Waals interaction (characterised by linear spring elements)
> between the walls. After solving the analysis, the deformation plot of
> the vibration mode shows that the inner wall penetrates the outer
> wall. This is impossible because as the inner and outer walls gets
> closer together, the van der Waals forces becomes infinitely large.
>
> So, I recalled from...Post: [XANSYS] [STRUC] Critical linear buckling
> strain; Date: 13th May 2008 (replies from J. Galan and C.
> Wright)...that in a linear eigenvalue buckling analysis, the
> displacement/strain is an arbitriary value. I suppose that is the same
> with a modal analysis (displacements/strains are also arbitriary)? If
> so, then I could simply reduce the deformation scaling of the
> vibration mode (and avoiding the use of contact analysis). Can someone
> shed a light or advice on this? Thanks!
>
> Note: assume that there's no critical issues relating the material
> props, stiffness of spring element, geometry, mesh and solution
> options. Even the frequencies captured agrees with the experiemental
> data.
>
> Regards
>
> Fung Tong
> Graduate Engineer, Rail Solutions Western
>
> ATKINS
> 3rd Floor, Longcross Court, 47 Newport Road, Cardiff, CF24 0AD
>
> Tel: +44 (0) 2920 358193
>
> Fax: +44 (0) 2920 48 5138
>
> E-mail: --email address suppressed--
>
> Web: www.atkinsglobal.com
>
>
>
> This email and any attached files are confidential and copyright
> protected. If you are not the addressee, any dissemination of this
> communication is strictly prohibited. Unless otherwise expressly
> agreed in writing, nothing stated in this communication shall be
> legally binding.
>
> The ultimate parent company of the Atkins Group is WS Atkins plc.
> Registered in England No. 1885586.  Registered Office Woodcote Grove,
> Ashley Road, Epsom, Surrey KT18 5BW. A list of wholly owned Atkins
> Group companies registered in the United Kingdom can be found at
> http://www.atkinsglobal.com/terms_and_conditions/index.aspx
>
> Consider the environment. Please don't print this e-mail unless you
> really need to. ^----------------------------------------------------
> |           XANSYS web - www.xansys.org             | |        XANSYS
> blog - xansys.blogspot.com          | |          The Online Community
> for users           | |            of ANSYS, Inc. Software           
>    | |         Hosted by PADT - www.padtinc.com          |
> ^----------------------------------------------------
>
>
> This e-mail transmission contains information that is confidential and
> may be privileged. It is intended only for the addressee(s) named
> above. If you receive this e-mail in error, please do not read, copy
> or disseminate it in any manner. If you are not the intended
> recipient, any disclosure, copying, distribution or use of the
> contents of this information is prohibited. Please reply to the
> message immediately by informing the sender that the message was
> misdirected. After replying, please erase it from your computer
> system. Your assistance in correcting this error is appreciated.
>
>  Post generated using Mail2Forum (http://www.mail2forum.com)

>
>
>
>
>
>
> ^----------------------------------------------------
> |           XANSYS web - www.xansys.org             |
> |        XANSYS blog - xansys.blogspot.com          |
> |          The Online Community for users           |
> |            of ANSYS, Inc. Software                |
> |         Hosted by PADT - www.padtinc.com          |
> ^----------------------------------------------------
>

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


Joined: 21 Oct 2008
Posts: 6
Location: Cardiff, UK

PostPosted: Thu Apr 02, 2009 6:47 am  Reply with quote

Dear Jose,

I'm an idiot in theory. I shall get a good reference to read! Anyway, when the mode scale factor is 1, indeed, the model was deformed unrealistically (the transverse displacement is way greater than the longitudinal length!)

Thanks for the inputs! Now I'm more confident of the analysis. CHeers

Regards
Fung Tong
Graduate Engineer, Rail Solutions Western
ATKINS
3rd Floor, Longcross Court, 47 Newport Road, Cardiff, CF24 0AD
Tel: +44 (0) 2920 358193
Fax: +44 (0) 2920 48 5138


[quote="jose.galan"]Dear Fung,
I think that you should review the basics of vibration theory. You should be absolutely certain that a modal analysis gives you natural frequencies and mode shapes only. The eigenmode amplitudes are unknown and could be chosen arbitrarily. However, since modal analysis is usually performed prior to a Mode Superposition Harmonic Response Analysis, the eigenmode amplitudes are chosen in a way which facilitates that next step. This procedure is known as mode shape normalization.


With the MODOPT command you can choose between two altenative ways to normalize mode shapes (See the Manual: Theory Reference (theory_toc.html)  | Chapter 17. Analysis Procedures (thy_anproc.html)  | 17.3. Mode-Frequency Analysis): (a) by default, eigenmodes are normalized to the mass matrix, that is, transpose(phi_i)*M*phi_j=delta_ij, where phi_i is the ith eigenvector, M is the mass matrix, and delta_ij is the Kronecker delta function (1 if i=j, otherwise 0).

(b) eigenmodes can be normalized to unity, which means that "phi_i is normalized such that its largest component is 1.0 (unity)" (taken from the Ansys manual).
Let us assume that your modes are normalized to unity. If we also assume that you are using mm as the unit to input your distances in ansys, then your mode shapes have displacements between -1mm and 1mm. I do not know how large is the gap between the cylinders, let us assume that it is 0.1mm. In that case, if you plot your mode with a scale factor of 1, you will be likely to see interpenetration (depending on the mode shape). The solution is to apply a scale factor smaller that unity, with the following commands:
gap=0.1
scale_factor=0.8*gap /Dscale,,scale_factor

With these commands you will not see any interpenetration, as long as the modes are normalized to unity. If they were normalized to the mass matrix, you should adjust the scale factor manually to a value small enought to avoid seeing interpenetration.
Best regads,

Jose M. Galan
Department of Construction Engineering
Escuela Tecnica Superior de Ingenieros
University of Sevilla
Spain


> ^----------------------------------------------------
> |           XANSYS web - www.xansys.org             |
> |        XANSYS blog - xansys.blogspot.com          |
> |          The Online Community for users           |
> |            of ANSYS, Inc. Software                |
> |         Hosted by PADT - www.padtinc.com          |
> ^----------------------------------------------------
>

Post generated using Mail2Forum (http://www.mail2forum.com)[/quote]
Back to top
View user's profile Send private message MSN Messenger
Christopher Wright
Guest





PostPosted: Thu Apr 02, 2009 9:22 pm  Reply with quote

On Apr 2, 2009, at 8:48 AM, fung.tong wrote:

> I think that you should review the basics of vibration theory. You
> should be absolutely certain that a modal analysis gives you
> natural frequencies and mode shapes only. The eigenmode amplitudes
> are unknown and could be chosen arbitrarily.
You should have stopped at the word 'only.' Never treat eigenvectors
as displacements, because they are shape functions, not
displacements. The You will only know the amplitudes if you provide
some loading--harmonic force or displacements, response spectra or
time-varying loads or displacements.

It is a fiction to normalize all displacements to unity and pretend
you have accurate displacements, because all the modes have equal
amplitudes. Nor do you know that the actualy amplitude of any mode
will be unity unless you know what the loading is. You can expect
that the fundamental frequency will dominate the response with
smaller contributions from higher modes. It definitely wont be a
matter of each mode having an equal amplitude. That would provide a
squirrelly plot. Figure out the excitation and determine the
displacement the right way--don't try to fake it.

> With these commands you will not see any interpenetration, as long
> as the modes are normalized to unity. If they were normalized to
> the mass matrix, you should adjust the scale factor manually to a
> value small enought to avoid seeing interpenetration.
It penetration exists, you want to see it. You may or may not be able
to close the gap depending on the excitation. Put it in.

Christopher Wright P.E. |"They couldn't hit an elephant at
--email address suppressed-- | 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
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