Skip to main content
  1. HyperX Support
  2. Interfacing With Your Tools
  3. HyperX and FEA

Discrete Stiffener 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).

Sizing Implications

Comparison to Smeared

The primary advantage of using smeared models is that the models are much easier to construct. There is less labor involved in meshing because the grids do not have to be aligned with the stiffener spacing as required by the discrete techniques. Discrete modeling technique 3 requires that stiffener grids be located in the correct Z axis depth to represent the web height.

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

Frozen Sizing Variables

Depending on the discrete modeling technique, certain Sizing variables are dependent on the mesh geometry. Therefore, these variables cannot be optimized (are frozen). Smeared modeling is valuable for preliminary design because all Sizing variables are available for optimization.

Frozen Sizing variables are automatically locked out so no values may be entered in the interface. The extracted value is returned from the FEM and reported on the Sizing form after analyzing.

implication-frozn-var.png

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