Honeycomb panel - Modal analysis

[adampar]

Hi there!

I am using Femap v.11.1.2 with NX Nastran 9.0 and i am currently working on modelling a honeycomb panel consisting of aluminum core and Carbon Epoxy laminate faces. I have decided to proceed with modelling the faces qith QUAD4 elements along with PCOMP entry (laminates) and solid elements for the Core. Now, my first attempt was to model the hexagonal aluminum core as a uniform homogeneous mesh and input orthotropic material properties. The problem is, that the core has significant values only for the thickness direction (E3,G13,G23), whereas in the other directions i insert low values (also to be careful with singularities). This causes my modal analysis to produce many natural frequencies that should not be there (very local modes in the core), maybe because of the small values of E1,E2 and G12. Other modes are close enough to a similar model consisting of only one laminate (no solid elements). So, what am i missing? Is this not a good way to model a honeycomb panel for a dynamic analysis?

Thank you in advance

 

[nlgyro]

how many solid elements do you have across the thickness?

 

[adampar]

I have 4 rows of solid elements through the thickness (thickness=20 mm). The other dimensions for the panel are 283 and 581 mm respectively.

 

[nlgyro]

For your dimensions, you're better of modeling your panel using shell elements.

The pcomp card can be used to give the face-sheet and core properties.

Modal analysis needs mass and stiffness, for which the shell representation is more than adequate.

 

[adampar]

OK I was just trying to correlate the results from these two different approaches...I input some other 3D orthotropic properties that i found from literature and the results are pretty close. Thanks nlgyro.

 

[APav]

What you describe can actually be done 4 ways:

- full 2D + PSHELL: derive equivalent PSHELLs for your panel properties. In the end this is what NASTRAN does anyways (with an echo = PUNCH you can retrieve the equivalent PSHELLs)

- full 2D + PCOMP: your 1rst solution

- 3D + PCOMP for laminate skins: your 2nd solution, using orthotropic formulation of MAT9

- full 3D solid laminates: a little complicated at first, but it works well. Setting up the model in NX NASTRAN is easier than in MSC NASTRAN.


As to which is best, I would say that depends on your model/part and load cases. For a dynamic analysis, let's say you've got a panel with equipments on it, 2D mesh will be easiest and well representative if the equipments don't have outrageous inertias for example.

 

[stressebookllc]

All you need is a 2D orthotropic skin and core definition, use 1 or low values for everything on the core material except G1Z and G2Z, get these from HEXCEL documents, and you'll be good to go.

http://www.stressebook.com

Stressing Stresslessly!