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

Shell Elements

Shell, or 2D, finite elements are used to make up HyperX Panel Zones.

Supported Elements

Nastran/Optistruct

CQUAD4, CQUAD8 (version 2024.2 and up), CQUADR (version 2024.2 and up), CTRIA3, CTRIA6 (version 2024.2 and up), CTRIAR (version 2024.2 and up), CSHEAR

Abaqus

STRI3, S3, S3R, STRI65, S4, S4R, S8R

Supported Sections

HyperX can import laminates and isotropic thicknesses directly from the FEM, if desired. See Import FEM Properties and Materials. In this workflow, HyperX supports:

Nastran/Optistruct

PCOMP (with MAT8), PCOMPG (with MAT8), and PSHELL (with MAT1)

Abaqus

Shell Sections and Shell General Sections.

Note

HyperX will read ply data if specified using the Composite option.

Orientation

Shells must be oriented properly with respect to the HyperX convention. The HyperX shell orientation convention is illustrated below.

signconvention.png

FEM-defined 2D element material orientation and normal vectors are used to determine this HyperX orientation.

Material Orientations

The HyperX x-axis is determined by the element material angle.

CQUADElementCoord.png

  • All element forces from the FEA are transformed according to the material orientation during loads import.

  • The material orientation - or HyperX x-axis - becomes the fiber direction for composites and the stiffener direction for stiffened panels.

Warning on Material Orientations

HyperX relies heavily on material orientations. Even if analyzing metallic structure, it is important for material orientations to be consistent within a Zone. Material orientations can be modified in HyperX (see Model tab of the Ribbon), but it is recommended to do so in a preprocessor, and then rerun the FEA.

Normal Vectors

Element normal directions are typically determined by default depending on the ordering of the nodes defining each element. This defines the HyperX z-axis of a given panel.

The HyperX normal vector determines the direction for all of the following:

Ply Stacking Direction

The element normal direction dictates the direction of ply stacking sequence, as shown in the figure below.

shell_implication-stacking_sequence.png

Stiffener Orientation

Smeared Stiffened Panels

Element normal vectors are assumed to point away from the stiffeners. As an example, in the image below, the element normals are pointed out, so the stiffeners are assumed to be on the inside of the aeroshell.

shell_model_intent_small.png

Discretely-Modeled Stiffened Panels

For discrete modeling techniques, the shell element normal vectors should point "out" of the aeroshell (same as smeared panels).

shell_implication-beam-orientations.png
shell_implication-shell-orientations.png

Pressure

The element normal vectors also dictate the direction for surface pressure loading. Pressure is defined as positive if it acts in the same direction as the element normal (shown as the positive z-direction below) and negative if it acts in the direction opposite to the element normal vector.

shell_pressure.png

Through-Thickness Thermal Gradient

The element normal vector also dictates the direction of the through-thickness temperature gradient. A positive through-thickness gradient is defined such that the temperature increases linearly (°F/inch) in the direction of the normal vector as shown below.

shell_temperature.png

Verify Element Orientations in the Viewport

Verify your shell element material orientation and element normals by turning on the corresponding Indicators on the View Tab of the Ribbon.

2DShells-VerifyOrientations.png

Reference Planes and Offsets

Reference Planes and Offsets

Reference Planes

The FEM Reference Plane is the plane FEA loads and stiffnesses are calculated with respect-to during the FEA solve. By default, the FEM reference plane is at the nodal plane. Any reference plane shifting from the nodal plane is implemented with respect to the element normal direction via offsets.

The HyperX Reference Plane - also considered the analysis reference plane - is the plane about which HyperX calculates Zone-level stiffnesses and loads during Sizing/Analysis. Each Zone has a reference plane (with corresponding offset, if applicable) defined as a Panel Setting.

PanelReferencePlane.png

Zone reference planes are both user and Design Property-concept-dependent - meaning they don't always align with the FEM reference plane or the natural load path of the panel.

  • When panels are placed into Structures, HyperX will automatically detect the FEM reference plane (and offset, if applicable) and apply that as the initial panel setting

  • The user is able to manually change the reference plane on the Panel Settings form for each panel - or in bulk using the Zone Settings Table. For more information, see Zone Settings.

  • For Unstiffened and Sandwich concepts, the HyperX reference plane follows the Panel Settings selection. But, for stiffened panels, the HyperX reference plane is always taken at the midplane of the top facesheet.

Be Mindful of Virtual Moments

When the HyperX reference plane defined on the Panel Settings form does not match the FEA reference plane, HyperX will automatically apply Virtual Moments to shift the FEM loads to the HyperX reference. It is recommended to iterate with FEA a couple of times to ensure the loads are in-sync with the panel reference plane.

Panel Reference Plane Options

  • Top Face Midplane - The shell offset is located at the midplane of the top facesheet or top stack.

    RefPlane-TopMid.png

  • Midplane - The shell offset is exported at the midplane of the entire stack.

    RefPlane-Midplane.png

  • Bottom Face Midplane - The shell offset is exported at the midplane of the bottom facesheet or bottom stack.

    RefPlane-BottomMid.png

  • Top - The shell offset is exported at the top of the entire stack. If element normal directions are pointed outward, this is equivalent to OML offset.

    RefPlane-Top.png

  • Bottom - The shell offset is exported at the bottom of the entire stack. If element normal directions are pointed outward, this is equivalent to IML offset.

    RefPlane-Bottom.png

Offsets

In many cases, reference plane offsets are defined in the FEM. This can be done either on the FEM element definitions or on the FEM property definitions. HyperX prefers property offsets, and therefore handles each case differently.

Element Offsets are used to define the reference plane offset directly on each element definition (think Zoff terms).

  • Import to HyperX - HyperX will not recognize element offsets on import.

  • Export from HyperX - Any FEM exported from HyperX will be updated to contain property offsets, rather than element offsets (element offsets will be cleared from the element definitions). These property offsets will take the original element offsets into account if applicable.

Property Offsets define the reference plane offset using the property definition (think Z0 definition for PCOMPs, or PSHELL with non-zero Bij and inflated Dij terms).

  • Import to HyperX - Offsets are recognized and directly translated to Panel Reference Plane on the Zone Settings form for each panel.

  • Export from HyperX - Any existing or updated offsets are applied to the exported FEM via property offset.

A user can also define Added Offsets in HyperX. This offset is the distance from a user-selected reference plane to the grid plane. The conversion between this offset (\(z_{HX}\)) and each of the solver offsets is shown below.

\(z_{Nastran}=-(z_{HX}+\frac{t}{2})\)

\(z_{Abaqus}=\frac{z_{HX}}{t}\)

Generalized Shell Export

Generalized shells (ABD) matrices are exported for the following cases:

  • Stiffened panels modeled using smeared panel Zones.

  • Unstiffened panel concepts (one stack, honeycomb sandwich etc) and discrete skin Zones with the PCOMP/PSHELL FEM Export set to PSHELL. See FEM Export Settings.

The shell offset is always zero. The assumption is that the shell in the FEM is meshed at the midplane of the top facesheet. See the figure in Shell Orientations.

Nastran, Optistruct

The ABD properties are exported to the FEM using PSHELL entries along with associated MAT2 entries for the 3x3 membrane (A), membrane-bending coupling (B), and bending (D) matrices. The MAT2 entries also contain the thermal coefficients.

The Nastran PSHELL ABD formulation factors out the shell thickness as a separate user input. This is different than the ABD terms found in classical lamination theory (CLT) where the shell thickness is modeled directly in the ABD terms. HyperX follows the CLT convention by setting the PSHELL thickness to 1 unit (see the 3rd field below). The PSHELL entry also contains a "bending moment of inertia ratio" field defined as \(12I/T^3\). In the same way as the shell thickness, the bending moment of inertia I is already modeled in the D matrix. Therefore, this field is always set to 12 units (\(T =1 \text{unit}\), \(I = 1 \text{unit}^4\)).

Listed below is a PSHELL entry for component 64 which points to three different MAT2 entries. The MAT2 entry 640 contains the 3x3 membrane stiffness matrix A as well as the membrane thermal expansion coefficients. The MAT2 entries 639 and 637 contain the bending D and bending-coupling B terms respectively. Also note that the PSHELL thickness is 1 and the bending moment of inertia ratio is 12 (these values hold for all unit systems).

$
$ Component 64
PSHELL        64     640      1.     639     12.                4.6804-4+
+
MAT2*                640  .216362035E+07  .348738516E+06 -.181898940E-10*
*         .131543634E+07  .367435860E-09  .410734503E+06                *
*         .316926664E-05  .748853548E-06 -.259254383E-21  .700000000E+02 
MAT2*                639  .602760870E+07  .635808845E+03  .231525114E+02*
*         .237766844E+04  .231525114E+02  .267053518E+06                *
*         .489963249E-05  .240954625E-05 -.578532834E-09  .700000000E+02 
MAT2*                637  .221413007E+07  .577538334E+04  .113686838E-11*
*         .186302688E+05  .113686838E-11  .121608701E+06                *
*         .490000000E-05  .490000000E-05 -.853752119E-22  .700000000E+02$

Notes:

  • The mass of the panel is modeled using the "Non-Structural Mass" (NSM) parameter (i.e. mass per unit area).

  • The thickness of the PSHELL entry is always one unit as in classical lamination theory.

  • Z1 and Z2 fiber distances for stress calculations are exported according to the outermost regions of the panel section.

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