Equiv. approach to model sandwich panel

[aubrey7978]

hi to all experts,

wondering if anyone had experience in modeling a composite material using equivalent approach, which means converting the composite to non-composite. can this approach model all behaviours, i.e. bending, axial behaviours etc, accurately?

thank you very much

 

[tstanley]

It is doubtful whether a composite material can have an accurate equivalent model, for several reasons.

1. An unsymetric lamination has bending and extension coupling.
2. The equivalent model would also have to take into account the properties of the individual plies, as well as the failure index that you would choose.

I personally have found it difficult to use micro mechanics to accurately predict the properties of the individual plies let alone the entire lamination with core. A good book on composites is Mechanics of Composite Materials by Robert Jones.

 

[aubrey7978]

thanks very much tstanley,

actually mine is a linear system, so wondering if the axial and bending effects can be uncoupled. since young's modulus of axial and bending effects are different, so will use the respective E's to get axial and bending stress respectively.

will try to look for the book recommended. thanks v much

 

[vonlueke]

Modeling your sandwich panel with noncomposite shell elements won't give you the micro-mechanics, but might be an acceptable approach for the macro-mechanics. If sandwich is symmetric, I believe bending/membrane coupling doesn't matter and can be uncoupled.

Check out

http://femci.gsfc.nasa.gov/hcplate/

. Your software probably provides an obscure menu somewhere to allow you to fully control these described membrane and bending stiffness parameters yourself, to model the sandwich. E.g., see NASTRAN PSHELL link at bottom of above page.

I believe the above link is a recommended method described as "Method 2(b)" in the following excellent article. Modeling Sandwich,

http://groups.google.com/groups?selm=3scsf5$25u@news.engr.udayton.edu

. Note he claims the transverse shear factor should be, say, 0.08 or less (?). I don't believe you'll find the "MIL-HDBK-23A" (circa 1968) he references, on-line. It might be many MB, and might not be as good as modern text book references.

Also, here's another link, just in case it might help a little.

http://www.oneoceankayaks.com/Sandcore.htm

. Good luck.

 

[aubrey7978]

thanks so much vonlueke.

those sites are really wonderful.

just wondering if u have used SAP2000 to model sandwich panel before? i'm currently playing around with 2 methods, one is using the equivalent approach and the other one is to directly model the composite panel. Did this by constraining nodes on the 3 layers tog. using rigid body constraints. have u ever come across this method?

thanks so much for ur help once again and truly appreciate it.

 

[vonlueke]

No. I haven't used SAP2000. Also I'm still fuzzy on whether Brockman in second link I listed above is referring to nonlayered or only layered shell elements; whether or not his mention of transverse shear thickness factor applies only to core; and the exact differences between his Method 2 and the first link I listed above. Brockman doesn't delineate details; and NASA link is sketchy to not delineate advantages/disadvantages of its stated method. My main question is whether Brockman's Method 2 recommendation can include "equivalent" nonlayered elements, as the NASA link seems to claim.

I haven't tried your second method (I used a laminate element, so far). What about making all three layers coincident, which automatically connects them, then applying z' offsets to face sheet layer elements, if possible? I assume you're referring to offset face sheets in your second method; otherwise it probably would be far from the correct answer. If the strain (not stress) distribution is really as nonlinear as Brockman claims, then any of these plate methods, including the laminate element, of course might be somewhat inaccurate. For more study on the subject, a few more references were listed in thread507-14199. Good luck.

 

[vonlueke]

I forgot to say, in your second method, I'm not sure, but using rigid bars might induce grossly false Poissons effects (?), trying to hold back strong forces when the panel tries to undergo the required, slight expansion or contraction through its thickness during bending. An analogy might be, trying to hold back a sealed steel container of water when it freezes. The effect of impossible rigid constraints can sometimes be rather dramatic. These inaccuracies might slightly contribute to the cumulative result inaccuracies. Good luck to you.

 

[vonlueke]

By the way, the so-called "z offsets" I was referring to, earlier, are a mathematical parameter (not physical element translations), if your software provides this feature in some obscure menu (along with the stiffness, bending/membrane coupling parameters, etc.).  By the way, some packages disable buckling analysis if model contains z offsets.

 

[aubrey7978]

thanks once again vonlueke,

just to add on the comment u made on my 2nd method, i tried comparing my model with a calculated answer (formula gotten from J.M.Davis book on Lightweight Sandwich Construction). tried varying the mesh density and my results seemed to tell me that there is an 'optimum mesh density'. the more i meshed the stiffer the panel became till it became stiffer than the actual caluclated answer. probably this is what u are referring to as results being dramatic.

also, u mentioned z-offset, what does a z-offset do anyway? what i'm doing is just physically offsetting the individual layers.

thanks so much.....

 

[vonlueke]

"z offset" is a parameter in the menu of plate element definition parameters (probably in same menu where you'll find membrane stiffness, bending stiffness, and bending/membrane coupling, etc.). A nonzero "z offset" value mathematically moves the plate element in the z' direction while simultaneously maintaining continuous connectivity with the nodes you offset it from...without you having to physically move the element yourself followed by laboriously attempting to connect it back to the meshed nodes or member centerline nodes. The default value for "z offset" is zero. Check your program documentation index or Help for the word "offset" to see if your software might have this parameter, or maybe call Technical Support.

There is also an "offset" paramater for beam elements. A beam offset is same as above, except you can offset in y' and/or z' directions. Plate element z offsets don't show up on the screen, but they're in the mathematical definition during the solve, whereas most products do show beam offsets on the screen. Good luck.