## Honey comb modeling

## Honey comb modeling

(OP)

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

Sakota

## RE: Honey comb modeling

You are trying to enter a "sandwich" composite. You will first want to define othotropic materials for your honeycomb and, although it is isotropic, it is easier to define an "orthrotropic aluminum". "orthotropic aluminum" has the same material properties in all directions, but it allows you to select it when defining your property. Honeycomb cores have known directional properties...you can get them from the manufacturer. Enter the two different materials (aluminum and honeycomb) so that you can select them when you are defining your thick (sandwich) composite property. This should get you started.

Garland

Garland E. Borowski, PE

## RE: Honey comb modeling

There are 2 ways you can do this:

1. Use a composite laminate property and define 3 layers. Layer 1 is the bottom facesheet, layer 2 the core, and layer 3 is the top face sheet. In the Reference Manual under PCOMP you will see some other settings field 9 (LAM) that allow you to specify the core type for facesheet stability index calculations. You would need to change these in the Editor. This step is optional.

2. Use a single PSHELL property and adjust the bending stiffness parameter, TS/T, etc. I recommend #1 above because it is easier to set up.

## RE: Honey comb modeling

Garland E. Borowski, PE

## RE: Honey comb modeling

Sakota

## RE: Honey comb modeling

## RE: Honey comb modeling

## RE: Honey comb modeling

3-D orthotropic properties are for orthrotropic brick elements, not quad elements, so that is why it is reducing the inputs to 2-dimensions. To have the 3-D properties, you would have an 8 to 20 node, 3-dimensional representation of the skin (including thickness) or core. As modeled, the thickness is handled by the laminated plate theory that is being used, or, if you are not using one of the composite material element types, then it is not concerned with your third dimension.

As for the Aluminum honeycomb, it still has material properties that should be available from the honeycomb core manufacturer. They are not 10e6psi and 0.33 like typical aluminum. Check the web for aluminum honeycomb.

Garland E. Borowski, PE

## RE: Honey comb modeling

A star for your patience

www.probasci.com -

Implantable FEA for medical device manufacturers

## RE: Honey comb modeling

Garland E. Borowski, PE

## RE: Honey comb modeling

## RE: Honey comb modeling

OK, time to "knock some cobwebs loose". You have to define your element type as "Laminate". You set up two different materials: one for your aluminum skins and one for your core. Your aluminum skins can be 2-D orthotropic, but your core would need to be 3-D orthotropic, not 2-D. When you define the layers in your laminate, select material 1 for the first skin, give it a thickness...you may even be able to use isotropic material properties for this...I haven't really tried it this way. For the second layer input into the laminate, select material 2, give it a thickness. Then for the third layer in your laminate, select material 1 again to provide for the other skin. My only concern is whether you can apply a 3-D orthotropic material to a 2-D representation. I have to admit that I'm not sure how the processor will handle this.

Garland E. Borowski, PE

## RE: Honey comb modeling

compression modulus

Compression strength

L direction shear modulus

W direction shear modulus

Any inputs??

## RE: Honey comb modeling

You have to tell us how you plan to model the structure and what type of elements you are using. If you are using 2D shell elements, then the thru-thickness E3 and strength properties are not used. However, NASTRAN does use the thru-thickenss transverse shear stiffnesses, G13 and G23. With 2D elements and compositeee/sandwich materials, you define properties for each layer as a Material, then combine the layers in a Property; the core is treated simply as a different layer. For in-plane properties of the core you enter some small dummy properties (I typically set E1=E2=100, G12=50, nu12=0.0).

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.

If you are using 2D elements, then read about the PSHELL, PCOMP, MAT2 and MAT8 cards in the manual; if you are using 3D elements read about the PSOLID and MAT cards in the manual.

## RE: Honey comb modeling

## RE: Honey comb modeling

Garland E. Borowski, PE

## RE: Honey comb modeling

## RE: Honey comb modeling

G=E/2(1+v)

But I'm not so sure that you can simply use your E3 to calculate the G-value for a honeycomb.

I would recommend that you look at the chapter on honeycomb plates in the FEMCI book:

http://femci.gsfc.nasa.gov/femcibook.html

Good Luck

Thomas

## RE: Honey comb modeling

Garland E. Borowski, PE

## RE: Honey comb modeling

Great Reference! A quick glance says the following:

"The shear modulus and the poisson's ratio is required on the MATERIAL card for MID3 and is obtained from the HEXEL manuals. You need to know the cell size and gage, or the desired nominal density."

I completely agree with this statement, but again say that an approximation, assuming a fairly small cell size and reasonable gage, is to use the isotropic equation.

Garland E. Borowski, PE

## RE: Honey comb modeling

## RE: Honey comb modeling

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

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

## RE: Honey comb modeling

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://w

## RE: Honey comb modeling

## RE: Honey comb modeling

## RE: Honey comb modeling

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

## RE: Honey comb modeling

## RE: Honey comb modeling

This is more or less what SWComposites proposed.

Tom Stanley

## RE: Honey comb modeling

## RE: Honey comb modeling

Thanks for the link!

## RE: Honey comb modeling

## RE: Honey comb modeling

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.