Modelling honeycomb core panels 1

[gutboy17]

I a new NeiNastran user and also new to the FEA world and I might have a analysis job pending that would be dealing with phenolic honeycomb core, fiberglass skin panel sturcture contruction. I've done a search on the web and this site for honeycomb core topics on how to model (i.e. material properties, FEMAP construction, element properties, etc.) these types of panels. So I was wondering if anyone has any info or past experience with this type of modeling that I might be able to pick their brain on how to accomplish this task. Thanks.

gutboy17

 

[JakeLiv]

I assume you will be using PCOMP entries for modeling the composite.
The problem with honeycomb material properties is that using a linear elastic material for the honeycomb is problematic. you will need to use "virtual" attributes, since honeycomb doesn't act like the regular poission ratio.

a sample honeycomb material entry:
mat1,1,1.972+8,6.8+7,.45,50

sample carbon bidirectional prepreg:
mat8,2,7.1+10,7.1+10,.27,2.2+10,7.+9,7.+9,1650

I assume you can decipher the code

 

[SWComposites]

JakeLiv - what units are your properties in?? If they are psi, etc., then they are wrong, since h/c core doesn't have anywhere near 200Msi modulus! Further, you can't use a MAT1 card for core properties with a PCOMP card - you have to use a MAT8 card with
E1 ~ 100 psi
E2 ~ 100 psi
G12 ~ 50 psi
nu12 = 0
G1z = core shear stiffness in ribbon direction
G2x = core shear stiffness in transverse direction

gutboy17 - what are you specifically modelling, do you plan to use a shell or solid model, what is the loading, and what do you want to determine with the model (deflection, stresses, frequency, etc.)??

 

[fkmeyers]

I think you can use a MAT1 for the core properties, not that this would be the best choice for honeycomb. For foam it should work OK. Typically, we use the PCOMP method for sandwich materials and MAT8 entries for all layers. NE Nastran has stability indexes for the face sheets which can be useful. It should be explained in the reference manual under PCOMP. I think it is the LAM field that specifies this. You would need to use the Editor to specify it since FEMAP does not support all of the NE Nastran (or MSC or NX) PCOMP options.

 

[gutboy17]

SWComposite-

The project is closet partition that is being installed on a 757 cargo conversion. We are using fiberglass/phenolic honeycomb core panels for the partition walls. The enclosure will be secured in the same fashion as seen in airline enclosures. The enclosure will have shelving to hold the crews carry on luggage and a garment rod to hanging articles. I would have to say the loads are very minor compared to the construction and therefore I think the deflections are going to be small also.

There is a solidmodel of the enclosure, but the panels are modelled as a single intity, not as two skin panels with a honeycomb matrix core.

So the question I guess is what is the industry standard for analyzing panels in this type of application. Solidmodel the actual panel and then build in the appropriate surface contacts between the models or FEM a 3D surface with laminate properties that would model the acutal panel component properties? I've seen on the web, where a honeycomb core solidmodel was modeled in a CAD program and then FEA for stress results. Looked pretty, but looked like a lot of work in the modeling world.

 

[SWComposites]

A shell model is the appropriate way to go. A solid FE model of this type of h/c panel will be overly complicated and frankly ridiculous. You should be able to generate mid-surfaces from the CAD model in your FE preprocesor to use to define the shell elements on; if not just create the shell model geometry from scratch. Also, solid elements often have poor bending performance. The most important modelling issue is the boundary conditions at the attachments to the aircraft stucture, and you may need to consider the flexibility of the structure that the closet is attached to.

 

[pcompg]

Usual practice is to model core with hex solid elements (2 elements through thickness) and face skins with cquad shell elements. After creating hex mesh, Patran Utility creates shell eleemnts on free faces of hex elements.

 

[Stresser1]

I dont think i have any brain you can pick on.

gutboy17,

In FEMAP you have two choices with the property definition, either PSHELL (plate) or laminate. Laminate is much easier to input, material and distances/thickness. with PSHELL (plate) visit this NASA page

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

go to presentations section for Honeycomb PSHELL card. This gives you plate equivalents.

PSHELL:
Thickness, Tavg or T1 (total thickness of facesheets from both sides)

Stress recovery
top fiber = Core thickness/2,
bottom fiber = negative of core thickness/1bottom

Material = facesheet material

Bend Stiffness, 12I/T**3 = from website calc
TShear/Mem Thickness, tx/t = from website calc

Bending Material = facesheet material (again!)
Transverse Shear = Core shear material

The Above is for plate, as you can see laminate will be much faster and simpler to input.

let me knwo how it goes!

 

[40818]

I will add my half-pennys worth....

The face skins should be quads and the core should be solids (CHexa). The material card for the core should be a MAT9 card.

You can determine accurately the core material properties to use from data such as boeing BMS/BDM for example.

Be careful with your allowables (FSL, FSW) as they will change due to differing thickness of core, also the core properties will change due to temperature etc.

Also, last thing, be very careful with your ribbon directions for the material card data, and the core element alignment as this will cause you all sorts of problems.

Try doing some sanity checks using hand calcs before progressing down the FE route though, a simple box type enclosure should be easy to Freebody, then check the structure by hand. Only then will you know whether the values you obtain from FEM are realistic or junk.

 

[SWComposites]

For the OPs application it is not worth the bother to model the skins and core separately. Just use shell elements and PCOMP/MAT8 cards to represent the entire sandwich panel thickness. Much easier to generate the model.