element type for glass in ansys 1

[mohamm21]

i need to create a glass for windshield.
im using fluid30 as an acoustic element
whats the element type for glass and whether i can use it with fluid30 for coupled acoustic analysis

hope u can help me out.

thank you
Quadris.
Automotive Engineering,

 

[Drej]

You must choose the element based on its constitutive behaviour NOT by the element type, although there is a link between the two. Glass varies depending on something called the "glass transition temperature". There are three main stages (solid, rubber, liquid) that glass goes through wrt this temperature - so you must develop your model based on the thermally active conditions. Glass can be viscoelastic (if thermally activated) and this can be modelled easily using the 18x family of elements - see TB,PRONY TB,HYPER and TB,SHIFT also. Just check the "Special Features" in the element help file. Search for "glass" or "amorphous" in the help search to find more information.

 

[mohamm21]

thank you drej for your reply.

I chose shell181 element type and used TB shift, tool narayanswamy tool to define the viscoelastic properties for glass. I am performing a modal analysis and when i run the solve command it gives an error saying nlgeom must be on when tb,sma is used.. But nlgeom can be only activated for static or a full transient analysis. if i run tha analysis without defining the viscoelastic properties using tb command then it solves perfectly.

do u know how i can solve this problem.

thank you for your help.

quadris
automotive engineering.

 

[Drej]

I'm not totally sure what you've done, or what you're trying to do (you said initially you were doing coupled acoustic, now you're doing modal analysis?) but for modal analysis you cannot include any model non-linearities. You have specified a set of non-linear material properties - and maybe other non-linearities - which may explain why you are getting the above errors. Remove the non-linear material properties for the glass (run them as linear using the MP command) and re-run the analysis. Remove any other non-linearity you have as well as ANSYS will either ignore them or take their initial conditions (as in the case of contact)for the run depending on what you're modelling - so remove them as you'll have more control. Remember also that you cannot have large displacement analysis turned on (NLGEOM,ON) as this introduces a form of non-linearity into your modal analysis (and NLGEOM is only relevant for static/transient structural analyses - not modal).

-- drej --

 

[mohamm21]

i am performing coupled structural-acoustic analysis of a vehicle cabin. i chose fluid30 as fluid30 as acoustic element and then had fluid structure interface at the boundary. then i ran modal analysis to obtain the structural, acoustic modes and structural-acoustic modes and frequencies.

i was trying to model the windshield of the vehicle cabin with glass and with non linear properties. i used tb/hyper command with nlgeom ,on.ansys solved it but as u said there were no changes in the results. i think ansys ignored teh non linear properties.


please tell me whether doing modal analysis is correct for this problem and also how to select exterior nodes of an area. we use nsla,s,1 to select interior nodes .

thank you for all your help.

quadris
automotive engineering.

 

[Drej]

For the selection of external nodes on an area try:

asel,s,area,,(area number)
lsla
nsll

I'm not an expert in acoustic analysis, however it appears that you will probably have to perform a harmonic analysis (ANTYP,HARMIC), which, as you say will require a frequency-based analysis to be performed. Remember that Harmonic Response analysis is a LINEAR analysis. Any nonlinearities, such as plasticity and contact (gap) elements, will be ignored, even if they are defined. You can, however, have unsymmetric system matrices such as those encountered in a fluid-structure interaction problem (see Acoustics in the ANSYS Coupled-Field Analysis Guide). Another, relatively expensive method is to do a transient dynamic analysis with the harmonic loads specified as time-history loading functions; see Transient Dynamic Analysis in the help for details.

-- drej --