The help system contains resources describing the supported element types, solution procedures, etc. for using FEA models in HyperX. This page is designed to serve as a quick reference guide for the best practices of FEA modeling. Although not exhaustive, this guide is a self-contained reference for most of the modeling techniques relevant to HyperX.
-
SHELLS: Prefer S4(R) and S3(R). Also support S8(R), STRI3, STRI65.
-
BEAMS: B31 or B32.
-
SOLIDS: Only supported as sandwich core. C3D8(I)(R), C3D6.
-
BOLTS: Only supported are CONN3D2 elements, used for fastener analysis.
-
SHELLS: Shell Sections and Shell General Sections are supported. Will read ply data if specified using the Composite option.
-
BARS: Beam Sections or Beam General Sections.
Note
See Shell Elements and Bar Elements for more information.
-
If HyperX does not “support” a FEM entity (such as coupling interactions, rigid attachments, higher-order elements, etc.), the model may still be used within HyperX without issue.
-
HyperX will only import entities it understands (shells, beams, solids, etc.), and ignore all others.
-
If a FEM update is executed with HyperX, all original FEM data that was not used by HyperX is copied over in its original state.
-
SHELLS: HyperX relies heavily on material orientations. These can be modified in HyperX, but it is strongly recommended to be set in the preprocessor.
-
Material orientations determine the fiber direction for composites, and the stiffener direction for stiffened panels.
-
Normal directions are also important. Element normals are assumed to point out of the aeroshell (in the opposite direction of the stiffeners for stiffened panels).
-
Normal directions also indicate the direction of stacking for laminates.
-
-
BARS: HyperX bar orientations must be set consistently throughout the model according to the HyperX convention.
-
SOLIDS: Z-axis is assumed to be the through-thickness direction for sandwiches, and x-axis is assumed to be the longitudinal (ribbon) direction.
Note
See Shell Orientation, and Bar Element Orientation, for more information.
-
SHELLS: Shell offsets (if applied) are automatically imported and used for sizing and analysis when transforming and localizing loads.
-
BARS: Bar offsets are not imported from the FEM but will be automatically computed and exported during the FEM update process.
Note
See Shell Offsets and Bar Element Offsets for more information.
-
When establishing mesh connectivity (such as the connection of a spar to a skin), the best practice is to have nodal connectivity between the stiffener and skin elements.
-
HyperX needs mesh connectivity to identify lines on which to split Zones if using the automated utilities to do so (such as splitting a large panel along a rib to allow for independent Sizing of the two new Zones).
-
-
Tie constraints, cohesive Zones, etc. may be used if desired, but Zone split-up (if required) will need to be done manually.
-
HyperX also needs to know mesh connectivity to associate stiffeners with skin sections for discretely stiffened models in order to accurately perform Panel Segment analysis.
-
Use of rigid constraints and connections for load introduction is acceptable, but often results in artificial load peaking. HyperX can use statistical load processing to reduce or eliminate the impact on Sizing results, but ideally load introduction should be realistic for best outcomes.
-
Whenever possible, material names should be used consistently throughout FEMs and HyperX. HyperX relies on names to match materials between the FEM files and Sizing / Analysis Materials.
-
This is necessary because HyperX requires much more information than is typically stored in FEA material definitions, such as laminate allowables, thermal properties, Correction Factors, etc.
-
-
HyperX supports the following common Abaqus solution sequences (both linear and non-linear):
-
*STATIC
-
*DYNAMIC
-
*BUCKLE
-
-
HyperX only requires element forces as an FEA output when performing strength and closed-form stability Sizing.
-
Grid displacements, eigenvalues and modeshapes for *BUCKLE, and solid element stresses may also be imported and used for deflection limits, sizing to FEA buckling results, and sizing to FEA stresses in sandwich cores, respectively.
-
Whenever feasible, steps should be generated to isolate load combinations that would be superimposed.
-
Example: fuselage pressure and wing up-gust should be included as two distinct steps, not combined.
-
-
HyperX will superimpose the loads as required internally, which may dramatically reduce runtimes for large numbers of steps.
-
Thermal steps should be run separately from mechanical steps, again to allow superposition.
-
HyperX will also allow cases to be “flagged” as thermal, and use help / hurt factors when combining with mechanical cases if desired.
-
-
Caveat: this strategy is invalid for nonlinear geometry or material properties. If using nonlinear FEA, combinations must be made before bringing into HyperX for accurate results.
-
It is recommended to apply pressures directly on the FEM (using DLOAD and DSLOAD entries), rather than using nodal forces, etc.
-
For curved plates, it is common practice to use FEA to compute membrane, bending, and transverse shear loads due to pressure.
-
For flat plates, it is desirable to compute the resulting moments and transverse shear loads due to pressure in a secondary process, as linear FEA is highly inaccurate for this.
-
In HyperX, use the “Zero Curvature” (prev. "Zero FEA Moment") option to ignore the bending moments FEA computed due to pressure, and enable the panel pressure analysis to compute these offline. See Zone Settings for more information.
-
HyperX reads pressure loads from Abaqus through the results file.
-