Honey comb modeling 8

[kotawsu]

Hello everyone, I am new to NE nastran and i want to analyse a honeycomb structure with aluminum facings and a honeycomb core. Could anyone guide me as to how to assign the material properties and is there any example which would be useful. I would really appreciate any kind of help. Thanks
Sakota

 

[SWComposites]

GBor, the isotropic formula for shear modulus DOES NOT APPLY to honeycomb core since the core is not a solid homogeneous material. Core shear moduli are usually available from the core material supplier.

 

[GBor]

I believe that for a SMALL CELL SIZE/LARGE GAGE, you can reasonably approximate through the isotropic equation. I agree that the manufacturer is the place to go for the information and would reference my very first post to this thread. Barring that as a posibility, if you have to make some assumption...

I understand that you have to understand "garbage in...garbage out".

With that, I quit arguing and agree with you...

 

[kotawsu]

ok, i dnt understand where i could have gone wrong, this is what i have done:
i have modeled the top face of the skin and have defined 2 materials. one for the facing and the other for the core. and in property i have used laminate and have defined isotropic for the facings and have defined laminate-2d orthotropic for the core. here i have given a small value for E1 and E2 to prevent numerical singularity while i have given the L direction and W direction shear modulus.I have simulated the simply supported beam problem which is there in the hexcel website. But the deflection from fem seem to be nowhere near the theoretical solution.like fem gives 0.0184m while theory gives 0.04m
could u please tell me where i have gone wrong.
the hexcel link for the problem is:

http://www.formulaschools.com/curriculum/7586+HexWeb+Sand+Design.pdf

 

[SWComposites]

The difference is probably due to a) boundary conditions, b) loads, c) mesh size. FE models are often too stiff. Please describe how you applied the boundary conditions and loads. Also, how many elements are in your model? Did you assign the L and W shear moduli to G1z and G2z?

 

[kotawsu]

i got it to work. i actually had overconstrained the model and i constrained it in the right way later. it matches well wth the theoretical result. Thanks. Is there an example of composite laminate modeling. if there is could u send me the link. Thanks.

 

[AdrianSonelly]

Dear SWComposites, Gbor (sorry don't know your names) and all who shared knowledge in this topic - thank you very much for your patience.
What you're discussed here was something I was looking for long time and could not find. My problem is that at my time I had no possibility to go to university so my math base is very poor if non existent. Also language limitations don’t help much. But enough of excuses (here we have a joke about bad dancer and balls that hinder him - it might well be international). How ever I'm determinant (i.e. persistent as a donkey) to learn.
So would someone rise to challenge and summarize what was discussed here? That would make an invaluable source for many IMHO.
So to model a sandwich structure in NASTRAN (it will apply for most other FEA solvers).
What is proper way to define material for lamina plies?
1)2D orthotropic
2)3D orthotropic
I was thinking that 3D orthotropic because in case of non unidirectional fabric we may have different Ex,Ey,Ez etc.
(Note that 3D properties data is rarely available from manufacturers. I guess that there's some way to calculate 3D data from 2D? If so than it will be nice to learn how.
What is the proper way to define material for core material?
1) Foam
2) honeycomb (alu, nomex)

What would be the best choice of elements for complex 3D sandwich structure? I'm very new to NASTRAN? In ANSYS one would simply choose shell91 (composite) with sandwich option and assign material_1 (carbon/epoxy) with appropriate orientation and thickness for face laminates and material_2 (core) for mid layer. My stupidity prevented me from being able to define core material properly as usually only compression modulus
Compression strength
G13
G23
And ANSYS requires full set(9) for E,G and Nu.

What would be best approach to model complex sandwich structure from geometric point?
Import it as surfaces and than mesh it with shell elements?
SWComposites, you mentioned "If you are using 3D solid elements (where the skins and core could be modeled with separate elements) then the full 3D set of properties is required."
Would you (please! please!) explain a bit more thoroughly how one should do it - from geometry till meshing and material.

I'm not asking about modeling hard points, bolted and adhesive joints etc. as this is out of topic or is it?

If there are some dumb mistakes in this post please excuse and correct me.

Kotawsu – would you please share how you finally modeled your case and it correlated well with theoretical results?

Thank you all so much!
Adrian

 

[kotawsu]

if i have the midsurface can i still use pcomp method to idelaise a sandwich panel or should i use pshell method.and if i have to use pshell method do i have to give only the facing thickness as the Taverage. thanks.

 

[tstanley]

Here is what Nastran has to say on the subject:

http://support.mscsoftware.com/kb/results_kb.cfm?S_ID=3031&requestTimeout=2000

This is more or less what SWComposites proposed.

Tom Stanley

 

[vorwald]

I have modeled Aramid honeycomb core with solid elements (CHEXA) using anisotropic material cards (MAT9). I specified appropriate values for G33 (Ezz), G55 (Gyz), and G66 (Gzx), and entered small values for G11 (Exx), G22 (Eyy), and G44 (Gxy). Please make sure that the material orientation is correct for the solids and plate elements, and the same for all the elements.

 

[AdrianSonelly]

Tstanley,
Thanks for the link!

 

[kotawsu]

how do we go about modeling a complicated honeycomb design using pcomp.suppose there are multiple parts connected to one another . do we have to assign local orientation to see that the face of each part falls on the x-y plane.

 

[vorwald]

Non planar surfaces are approximated as small planes. The important thing is to make sure the material direction is correct. In FEMAP, read the help section for "Modify, Update Elements, Material Angle." You can view the material angle using view/options; labels, entities and colors; element - orientation/shape. To see the material angle for 3-d elements, you have to turn off hidden line.

You can update the material angle for a group of elements using modify / update / material angle. I don't recall if this works for 3-d elements.

To get the x/y/z stresses/strains to come out in the right planes, you may have to modify the element orientation. Just remember to update the material angle after any modifications to the element orientation since the angle is relative to sides one/two of the element.