Honeycomb Sandwich Close Outs Modeling

Engineering Software general discussion FEA (Finite Element Analysis)
#1

QUESTION
I am trying to model a honeycomb panel of a fuel tank subjected to internal pressure. We use tapered or ramp close outs for Honeycomb sandwiches and had a few questions regarding the same. I am using Patran/Nastran version 2010. To start with, I did represent the end doublers followed by ramp and panel section with max core thickness. When I did a simple 2D panel under the influence of uniform pressure with all sides simply supported, the results are way off from hand calculated values.

To provide some more info, I used 2D representation of Honeycomb Panel. The panel I am trying to model has Aluminum face sheets (2024) with Aluminum Core (5052). When I modeled the above without the closeouts in FEA, the results are matching very closely to hand calc values. So, is it acceptable to not include close outs in FEA model? If its necessary, any inputs on how better I can represent the same in FEA apart from the above procedure?

My employer is urging me to find out the best practices regarding the above. I am receiving very little help here.

REPLIES

KSshopper
I don’t think there is any industry best practice. I’ve worked for three separate companies and seen it done three different ways:

  1. Model the entire composite bondment with shell elements (PCOMPS). Model the core ramp area with average (1/2) height core. Use a hand analysis to calculate:
  • strain in the ramp ply,
  • flatwise tension and compression at the ramp transitions
  • shear at the height (thickest portion) of the core. Note that core shear is not checked at the bottom of the ramp near the laminate. Otherwise you would never show it good.

  1. Model the core with solid elements and the facesheets with shell elements. The core stresses and ply strains can be read directly from the model. NASTRAN is pretty good for this since the solid elements have features that avoid shear locking in thin solids. This method is great unless you need to make design changes that blows away the geometry on your carefully crafted FEM.

  2. Model with shell elements and ignore stresses and strains in the transition. If the core shears and laminate strains are acceptable at the boundaries of the transition, they will be acceptable in the ramp as long as you respect the design rules (ply drops, core ramp angles, etc).

I like item 3. Items 1 and 2 tend to show low margins at the ramps despite never seeing a panel fail like that. It’s a big paradigm shift for me since core ramps were big deals at the last place I worked.

SOURCE
https://www.eng-tips.com/viewthread.cfm?qid=389488
Above is a snippet.

#2

A point of view that may be worth adding:
It is fairly common practice to use FEA for bulk load distribution and evaluate details by hand-calc. Using FEA for the entirety of the analysis is of course possible, but requires much more experience using the FEA software to know the details that allow you to make the model that permits extraction of the results you need. I am personally much more comfortable with the combined method that the OP says that they started with, and actually consider that the “best practice” when it is done well.

A footnote that there may be some additional methods to be found in the Boeing Design Manual, if you have access to it. I don’t have a copy handy now, but IIRC this is a subject presented in some depth there.

1 Like