Honeycomb aluminium sandwich

[dragonix]

Hi all,

I have to model a honeycomb aluminium sandwich made of 2 sheets bonded to an honeycomb structure with ansys

Now my problem is how to model it correctly. Reading around the web I found many techniques but the main are:

1) Model the sheets with shell elements and isotropic material. Honeycomb is modeled with solid elements but ortotropic equivalent properties are needed

2) Use shell elements to model sheets and honeycomb using isotropic material (i.e. model the real geometry of the material). This can cause an over extimation of E33 (normal young modulus) because of through thickness stiffness of shells

3) Use shell91 elements (composite) defining all layers.

I don't have the material properties but I just know that plates and honeycomb are made of aluminium so I wonder if option 2 is valid

Anyone can give me a suggestion?
Thanks in advance

 

[ESPcomposites]

There are even more methods. All can work, but you must define what your interest is first.

For example, is it deflection (stiffness), buckling, local failure modes, etc.? What you seek from the model will dictate your approach.

Brian

http://www.espcomposites.com

 

[rb1957]

and your FE code ... "shell91" ?

i'd've thought that the easiest way is to use laminate elements, plate elements with laminate properties.

you can model the core (as solid) and the faces (as shells), just sounds like needless duplication, and a hold-over from before laminate elements were common.

if you don't have the material properties, i wonder what you hope to accomplish. i guess you could use E, G of Al for the face sheets as 2D elements, and the core has very low in-plane properties and "large" out-of-plane.

most of that data should be online ... what are you using ?

 

[dragonix]

I am using ansys to model it.
Shell 91 is the 2d element with composite option.

A good way should be (as rb1957 told) use 2d shells for plates (material: isotropic aluminium) and model core with 3D solid elements using an equivalent ortotropic model (i.e. out of plane young modulus >> than in-plane young modulii).

But I want to be sure of material behaviour, so I thought to do like this:

model the real core (I mean model the true core cells geometry) using a isotropic material (aluminium), then do a second model with solid elements for core (which is easier to handle than the previous one) with ortotropic properties and compare both models.

What do you guys think?

 

[rb1957]

does "model the true core cells geometry" mean you're going to model the hex-cells ? ... that's a "novel" method for getting the out-of-plane G ... i suspect it'll work, but is sounds like a lot of work ? surely you're using a standard core 3 lb/ft3 ? surely the data's available on Hexcell's site ??

 

[dragonix]

does "model the true core cells geometry" mean you're going to model the hex-cells?

Yes, I would like to try.


i suspect it'll work, but is sounds like a lot of work ? Unfortunately yes.


surely the data's available on Hexcell's site ?? I will try to find it.

Anyway, to define material properties for solid core elements, I need in-plane young modulus, out of plane young modulus and poisson ration. Are these data available on manufacturer datasheets?

 

[rb1957]

i think that Hexcell, or wohever, has all the data you need on their site. if not, i'd use 1E4 for E11 and E22 for the core; that should be enough to keep the load in the faces.

 

[ESPcomposites]

You still have not stated what you want to get out of the model and what effects you are trying to capture.

For example, why do you want to model the core at all? Do you want to capture the effects of transverse shear deformation or capture the facesheet wrinkling mode (or perhaps even intracell buckling)?

Depending on your objective, the model can be as simple as a plane of shell elements or as complex as modeling in the hex array of the honeycomb.

That said, shells for the face and solids for the core is a common approach. But it will not cover all failure modes and may be overly complex for some problems. You should really have a better idea of what you want out of it before you model it.

Brian

http://www.espcomposites.com

 

[dragonix]

You still have not stated what you want to get out of the model and what effects you are trying to capture.

For example, why do you want to model the core at all? Do you want to capture the effects of transverse shear deformation or capture the facesheet wrinkling mode (or perhaps even intracell buckling)?

Depending on your objective, the model can be as simple as a plane of shell elements or as complex as modeling in the hex array of the honeycomb.

That said, shells for the face and solids for the core is a common approach. But it will not cover all failure modes and may be overly complex for some problems. You should really have a better idea of what you want out of it before you model it.


The panel is loaded by accelerations on x,y,z axes and I have to analise panel stresses and deformations (to see if any bucking occurs). For this reason I was thinking to model core and sheets.

Thank you to both of you