Author 
Message 
christopher.wright User
Joined: 17 Jun 2009 Posts: 927

Posted: Thu Jan 26, 2012 10:34 am 


On Jan 26, 2012, at 1:27 AM, Luca Zanotti Fragonara wrote:
Quote:  What is nonlinear is not the behaviour of the beam
(except for geometric nonlinearity, but that doesn't affect linear
normal
modes) but the succession of the frequencies:
 Just so you'll knowbe careful throwing the therm 'nonlinear' around
when you post. Everyone else who saw your post was probably thinking
the same thing as Ithat the stretch of the cable isn't proportional
to the load.
Quote: 
Now, my problem is that I want to change the bending stiffness of my
element,
without changing its mass.
 Change the elastic modulus you input. If your cable is anything like
wire rope, the wire strands inside are twisted and tend to straighten
under load. Consequently an 'effective modulus' is used to model such
things.
Quote:  That is because I want to use the ASEC command, but, apparently,
it doesn't generate a mass matrix related to my element.
 You make the mass matrix by inputting a mass density (mass/volume).
You can do a quick inline calculation of the appropriate density as
mass/length divided by the cable crosssectional area. I makes for
neat readable input. Something like DENS,,(gamma/Ac) or DENS,,(gamma/
(k*Ac)) where gamma is mass/length and Ac is the input for the area of
the beam element definition. You'd use the k value to modify the
stress area to the area of all the cable material.
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/~chrisw/
Post generated using Mail2Forum (http://www.mail2forum.com) 

Back to top 


jose.galan User
Joined: 21 Oct 2008 Posts: 140

Posted: Fri Jan 27, 2012 7:05 am 


The problem seems to be that the command INISTATE,DEFI,,,,,4260000/(9271/1e6), which should introduce an initial stress of 459MPa, works properly when using a CSOLID section, but it does not introduce any initial stress when you use an ASEC cross section.
You can easily check this out by running a static analysis with the initial stress state only, without gravity, and looking at the values of the reactions in the general postprocessor (PRRSOL). When using the CSOLID section, you get horizontal reactions Fx equal to (459e6 Pa*pi*(0.058 m)^2=4.85e6 N=4.85 MN. However, for the ASEC section the horizontal reactions are zero, which shows that no initial tension has been introduced.
You can also notice the problem by comparing the static solutions including gravity. The displacements calculated with the CSOLID and ASEC sections are very different. The ASEC results are 10 times bigger, which means that the ASEC model is 10 times less stiff under gravity load, which is due to the lack of pretension.
I think that the strange behaviour happens because the INISTATE command applies the initial stresses at the integration points, but the ASEC section does not have any integration points because its integrated crosssection properties (area, inertia, etc) are supplied by the user (check the help on the sectype command).
There is an alternative to using INISTATE. You can introduce a prestress by applying a prescribed horizontal displacement at the right edge of your cable, keypoint 2, of value UX=(initial_sigma/E)*L=459e6 Pa/1.6298e11*45m=0.1267m. Simply replace the command DK,2,UX with DK,2,ux,0.1267 By doing so, the cable deflections (UY) under gravity in the ASEC model agree with those in the CSOLID section.
When you calculate the eigenfrequencies, the only load that you apply on your model comes from the initial stress with the command INISTATE. Since it does not work properly in the ASEC model, you really have a model of a cable with zero stress. That explains why the natural frequencies are zero!
I reccommend you to check the following chapter of the Ansys help:
Structural Guide  Chapter 3. Modal Analysis  3.11. Prestressed Modal Analysis of a LargeDeflection Solution
You will see how Ansys lets you do a prestressed modal analysis, based on a previous largedeflection static analysis. You will find the command UPGEOM specially useful, since it updates the geometry to the deformed solution, without storing the displacements as you were doing in your macro. The stresses from the previous static solution are automatically applied with the PSTRES,ON command.
You can simply add the following lines after calculating the static solution to obtain the modes:
!!! Prestressed Modal Analysis of a LargeDeflection Solution/SOLU!ANALISI MODALEANTYPE,MODALupcoord,1.0,on !update geometry to the largedeflection solutionpstres,on !uses prestresses obtained in the previous largedeflection static analysis
!ESTRAZIONE DEI PRIMI 20 MODI DI VIBRAREMODOPT,LANB,20MXPAND,20
PSOLVE,eiglanb !PSOLVE is used instead of solve to calculate eigenvaluesFINISH
/soluexpass,on !expand eigenvector solution (to review modes in the postprocessor)psolve,eigexp
/POST1SET,LIST !See list of natural frequenciesset,first !Review first mode/dscalePLDISP,2
Kind regards,
Jose M. Galan
Construction Engineering Dept.
University of Sevilla
Spain
On Thu, 26 Jan 2012 10:27:49 +0100 (CET), Luca Zanotti Fragonara wrote: Quote:  Quote:  Actually that was not the point of my email.
Using a Beam element with a circular section, I get results that are very
close to the reality. What is nonlinear is not the behaviour of the beam
(except for geometric nonlinearity, but that doesn't affect linear normal
modes) but the succession of the frequencies: cables and beams have succession
of frequencies in the form n*pi.greek*(constant). If you consider bending
stiffness, this series of frequencies is not linear anymore (n is squared or
something like this).
Now, my problem is that I want to change the bending stiffness of my element,
without changing its mass. This is because I know with good accuracy the mass
per unit of length of my steel cable, but it is very hard to know the bending
stiffness of my steel cable. One thing its sure: bending stiffness of a cable
is NOT the bending stiffness of a beam with the same circular section, it will
be much lower. That is because I want to use the ASEC command, but, apparently,
it doesn't generate a mass matrix related to my element.
I can solve the problem in another way: using a circular section "reduced" and
increasing the density of my element, in order to keep constant my mass per
unit of length... But this is not the way I like to solve a problem like
this...
Thank you in advance,
LucaMessaggio originale Da: chrisw@skypoint.com (chrisw@skypoint.com) Data: 26/01/2012 4.06 A: "ANSYS User Discussion List"<xansys@xansys.org (xansys@xansys.org)> Ogg: Re: [Xansys] Problem with cable modelled with beam elements On Jan 25, 2012, at 9:28 AM, Luca Zanotti Fragonara wrote: Quote:  My final purpose is to perform a modal analysis and comparing the results of frequencies with experimental determined frequencies.  If you really mean 'nonlinear' and not 'stress stiffened' you're going to have problems since modal analysis is basically a linear process. You can try doing modal analysis with stress stiffening or you can run the problem with whatever nonlinearity you have in mind and restart it as a modal analysis. In the latter case the analysis will run a linear mode extraction with stiffness and mass matrices as they exist under load. The eigensolution will represent a small displacement to either side of the equilibrium point. You might also give some thought to the possibility that your non linearities have a small effect on the solution and that the non linearities have a small effect, so you would get good rather than perfect resultsmaybe within the experimental error. Christopher Wright P.E. "They couldn't hit an elephant at chrisw@skypoint.com (chrisw@skypoint.com)  this distance" (last words of Gen. ....................................... John Sedgwick, Spotsylvania 1864) xansysmod@tynecomp.co.uk (xansysmod@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 xansysmod@tynecomp.co.uk (xansysmod@tynecomp.co.uk) 
++
 
Post generated using Mail2Forum (http://www.mail2forum.com) 

Back to top 




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

