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

 

[GBor]

Sakota,

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

 

[fkmeyers]

Look in the NEiNastran User's Manual, Special Topics section. There is a sandwich example there.

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.

 

[GBor]

I would add that Frank's option #1 is likely to be more accurate than option #2. Laminated plate theory for a sandwich composite is a bit more complicated than just an alteration of the bending stiffness parameter, although bending is the largest impact. You need to be able to examine your core failure modes. For an uncored composite, you can use an orthotropic shell element if you know the "smeared" properties of your composite, which, personally, I prefer to calculate outside of the software as a check on how I entered the information.

Garland E. Borowski, PE

 

[kotawsu]

thanks everyone. i really appreciate your time and patience. Meyers,I have still not looked into the manual but would do so now.If i have any problems shall post the problem here..thanks once again.
Sakota

 

[kotawsu]

ok, i have a question. I am modeling my core using 3d orthotropic properies but whn i run it its converting the material properties to 2d orthotropic because of the quad elements used to model the shell. What i am concerned about is the how do i give the compressive modulus if i can define the 3rd direction properties.do i juss leave it?

 

[kotawsu]

ooopss one more question.. the core is aluminum honeycomb. so,it has no elastic modlus and poisson ratio. so how do i define the material property? i used orthotropic but then it needs a E and a possion ratio.Thanks

 

[GBor]

Let's try to answer your first question:

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

 

[ProbaSci]

GBor,
A star for your patience

http://www.probasci.com

-
Implantable FEA for medical device manufacturers

 

[GBor]

Much Thanks!

Garland E. Borowski, PE

 

[kotawsu]

GBor, Thanks for your reply..I have some properties for the core but the things is i am trying to figure out where to input it. i am using orthotropic 2d for the core and i have modeled the top face of the upper facing in the 1-2 plane.And from the properties i have a compression modulus which would be E3. But i dn't have option for E3, its only E1 and E2.. so do i have to define a local co-ordinate system to define the compression modulus and the L, W strength? Thanks once again

 

[GBor]

If I understand correctly, the problem is that you are trying to give 3-D properties to a 2-D element type. 2-D orthrotropic element types will not consider the out of plane compression and, therefore, is not concerned with E3.

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

 

[kotawsu]

Gbor, that is eactly how i modeled earlier. But it dsnt take 3d orthotropic properties since the core is a 2d representation and the thickness is given through section properties and not thru the nodes. So, i donno how to assign the material properties that i have for the core. the properties that i have are:
compression modulus
Compression strength
L direction shear modulus
W direction shear modulus
Any inputs??

 

[SWComposites]

Kotawsu,

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.

 

[kotawsu]

Thanks SW for your input. But for a honeycomb core E1 and E2 are zero and it has only compression modulus which is E3. But since i have modeled juss the upper facing of the skin and defined the thickness through section properties i am forced to used 2d elements which means that i dnt have an option of entering E3 which is the compression modulus. In order to avoid singularity am entering small values for E1 and E2 even though they are zero. So the compression modulus which is the out of plane modulus is what causing the difficulty here.

 

[GBor]

OK. I can't figure out how else to say this other than: You have to model your situation differently...or at least think of it differently. Cores generally exist for one purpose...to transfer load from the inner skin to the outer skin. It does this not by Young's modulus, but by the shear carrying capabilities...in other words: G13 and G23, as SWComposites has stated. In NENastran, these values show up in 2D orthotropic materials as G1z and G2z, respectively. If all you have is E3, but you know that you have aluminum and it is isotropic, estimate G1z and G2z as approximately equal and having a value of E/2(1-v^2) (I think that's the isotropic formula...someone please confirm or I'll look it up later), where v is poisson's ratio (about 0.27 for aluminum, I think).

Garland E. Borowski, PE

 

[kotawsu]

Gbor, thanks for the patience.. i solved the problem that i had using 2d orthotropic.

 

[ThomasH]

The isotropic formula GBor mentioned should probably be:

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

 

[GBor]

Thanks for the correction, Thomas, I should know better than to try and remember an equation...even one as simple as that! As for the calculation of G from E3, it's an approximation. Probably not precise, but shouldn't be too far off. He does still have an isotropic material even if it is in a honeycomb.

Garland E. Borowski, PE

 

[GBor]

Thomas,

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