Skip to main content
  1. HyperX Support
  2. HyperX Solutions
  3. Stiffened Panels

Discretely Stiffened Panels

Add Context with collieraerospace.com

Stiffened panel segments are defined from attaching skins and stiffeners. Failure analyses such as cross section crippling require that the skin and stiffener are treated as a system. Read more in the context of the Analysis Workflow here.

To discretely model a Stiffened Panel is to represent stiffeners with finite elements. The primary advantage of discrete models is that unique stiffener buckling, crippling, strength, and local buckling margins of safety may be reported for each skin and stringer segment component. In HyperX, Panel Segments are used to correspond to these components during analysis.

Additionally, the discrete Techniques 2 and 3 will capture the effects of having non-uniformly spaced stiffeners and stiffener terminations.

Modeling

Discretely meshed models have several variations which utilize a combination of beam and shell elements - as shown below using Nastran terminology. For all discrete modeling techniques, the skins are represented using shell elements.

mtech_tech14.png

For proper loads processing assumptions, the shell element normal vectors should point "out" of the aeroshell (same as smeared panels).

implication-beam-orientations.png

The choice of technique will affect which cross-section variables can be optimized.

implication-frozn-var.png

Note

When the stiffener space or height value is needed for loads processing, HyperX will automatically calculate them based on element areas.

The Panel Segment dimensions (\(A_{seg,L}\), \(A_{seg,R}\), \(L_{seg}\), \(w_L\), \(w_R\)) are required to compute the Panel Segment forces, see below.

Methods and Equations - FEA Loads Stiffened Panels

The Segment dimensions are computed directly in HyperX based on the length and area of the prescribed FEM elements.

ss-tech2_skin_stiffener_FEM_dimensions.png

Computing the Spacing

The skin segment areas are calculated by summing the element area. Where the subscripts 'L' and 'R' denote the elements in the left skin and right skin segments respectively.

\(A_{seg,L}=\sum A_{e,L}\)

\(A_{seg,R}=\sum A_{e,R}\)

The segment length is the sum of the length of the stiffener segment elements.

\(L_{seg} = \sum L_e\)

The skin segment widths are calculated from the skin segment area and stringer segment length.

\(W_L=\frac{A_{seg,L}}{L_{seg}}\)

\(W_R=\frac{A_{seg,R}}{L_{seg}}\)

The spacing span for left and right skin are equivalent to the skin segment widths.

Computing Panel Height for Tech3 Segments

The panel height for discrete modeling Techniques 3 and 4 is calculated from the FEM grid spacing, skin and cap thickness defined for concept and the skin offset.

\(H_{panel} = B_H + T_{skin} + Z_{off} + (1/2)T_{cap}\)

This calculation does not account for Z offsets on the bottom flange.

Uniaxial Stiffened Panel Example

implication-height-uni_v7.png

\(H=1.57+0.14+0.04+0.05⁢= 1.8⁢in\)

Hat Stiffened Panel Example

implication-height-hat_v7.png

\(H=1.57+0.14+0.04+0.05⁢=1.8⁢in\)

Overwrite the Spacing and Height

The height and spacing calculations are overwritten if the following Advanced Settings option is set = No.

ss-panel_height_backdoor_option.png

The user may then manually define the stiffener height in the Design Property. The stiffener spacing (skin widths) is defined separately for each skin by setting the X and Y buckling spans on the skin segment component on the Panel Settings Form.

setarea.png

Discrete Object Assignment

Panel Segments are constructed by assigning shell and beam elements corresponding to the objects of the Stiffened Panel - skin, flange, web etc. The following tables show which objects are assigned for each modeling technique (per family, per concept).

HyperX Implications

The Panel Segment Analysis Entity allows HyperX to properly recognize discretely modeled skins and stiffeners as part of a collective system, rather than individual Zones. This allows Design Results and Margins of Safety to be calculated per object within the Segment (left skin, right skin, and stiffener).

panelSegmentOverview

In order to be combined into a Panel Segment, the Zones corresponding to the related panels and beams must be in the same Structure. As with traditional Zones, Panel Segments require Design, Load, and Analysis Properties in order to define the Sizing/Analysis. But, since a single Panel Segment consists of 3+ different entities (left skin, stiffener, right skin), that assignment process looks a little different. An example is shown below - taken from the Tech 2 Blade Sample Project.

image5.png

Note

Stiffener dimensions (\(T_{foot}\), \(T_{web}\), etc.) and margins (strength, crippling, etc.) are stored with the Stiffener Segment Zone. Skin dimensions (\(T_{skin}\)) and margins of safety (skin strength, skin local buckling) are stored with the Skin Segment Zone.

The loads processing for Panel Segments works a little differently as well - since the loads-sharing between skin and stiffener elements must be properly applied over the cross-section. The image below summarizes this process. Note the skin element orientations, as it is important to have those consistent with the stiffener axial direction.

panelSegmentLoadProcessing

Tip

For more information, see Panel Segment Loads Processing.

Recently Viewed

Didn’t find what you’re looking for?

Submit a Request

Didn’t find what you’re looking for?

Create a New Post