Skip to main content
  1. HyperX Support
  2. Training
  3. Training Module #3: Basic Building Blocks

Training Module #3: Building Blocks - FEM and FEA

Video

Overview

Unless you are working with Non-FEA zones and/or Non-FEA Loads, all HyperX Sizing and Analysis will be one on FEM geometry in response to element-by-element forces from the corresponding FEA. Some general guidelines to keep in mind:

  • Each HyperX Project is associated with a single Finite Element Model (FEM). That model can have multiple Run Decks with varying load cases and configurations, but there is always one model per Project.

  • HyperX Zones (areas of constant cross-section, which are Sized/Analyzed) are made up of FEM elements. When a FEM is imported, each existing FEM Property (or Section) will become a HyperX Zone. In the image below, each colored panel is a HyperX Zone, created from corresponding FEM property cards.

    zone-example.png

  • HyperX can directly import the material and property definitions from the FEM, which allows for a margin assessment on the as-modeled structure.

  • Element forces and grid displacements are imported from the FEA results file for all (desired) subcases. These are the loads that are used for Sizing and Analysis.

Supported FEM Entities

The supported element and property types are listed in the table below, organized by solver and dimension. See also Nastran Quick Reference and Abaqus Quick Reference, respectively.

Note

HyperX will ignore anything in your FEM that it does not support.

FEMSupportTable.png

Tip

As of Version 2024.2, released in October 2024, HyperX also supports: CTRIA6, CTRIAR, CQUAD8, CQUADR

Modelling Best Practices

2D Elements

  • 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.

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

    CQUADElementCoord.png

    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.

    shell_model_intent_small.png

  • Reference Planes and Offsets

    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

1D Elements

  • Orientation

    Bar elements must be oriented properly with respect to the HyperX convention. Failure to do so leads to invalid results. The figure below shows the beam orientation convention for HyperX, Nastran (and Optistruct), and Abaqus.

    beam_csys_comparison.png

    Grid A to Grid B direction and orientation vector both affect how a beam section will appear in HyperX.

    • Flipping Grid A and Grid B rotates a beam section lengthwise (green indicator below).

      • Ex. Z beam has cap and foot pointing the wrong directions.

    • Changing the orientation vector rotates the beam section about the long axis (orange indicator below).

    BarElement-GridAGridB.png

  • Offsets

    Bar offset vectors are defined by the distance from the centroid of the beam section to some reference point. Bar offsets are not imported from the FEM. If an offset is applied to a HyperX beam, that offset will be automatically computed and exported to the FEM during the FEM update process.

    HyperX offers three options for introducing offsets into beam sizing/analysis. These are set on a Zone-by-Zone basis on the Reference Plane section of the Beam Settings form. In this case, "Top" is in the direction of the HyperX Z-axis.

    beam_offsets.png

Connector Elements

To ensure the best results, it is important to understand the relationship between connector modeling techniques and HyperX Joint Load Extraction/Processing methods. Load extraction and processing differs based on whether the Joint is analyzed as an Edge Joint or Point Joint.

Note

Bolted Joints can be represented as Edge or Point Joints. However, when the connector elements are discretely modeled, they must be represented as Point Joints.

multiLapJointDiagram.png

To make the most of HyperX's Bolted Joint capabilities, reference the image above and make the following considerations when modeling connector elements:

  • CBUSH elements must be attached either directly or via RBE to different Zones on both ends. If they are not connected to different Zones, HyperX will create 0 or 1 member Joints which have limited functionality.

  • RBE may be RBE2 or RBE3. RBE3 is recommended.

  • The outer-most 'Grid A' represents the connection to 'Sheet 1'. For countersunk fasteners, this will be the countersunk skin.

  • It is important to align 'Grid A' and 'Grid B' directions for each spring in series. However, the local shear (y-z) planes do not have to be perfectly aligned between springs - HyperX will make the proper transformations, into-sheet coordinates defined by material vectors, and shear force vector sums to compute the sheet bearing for Sheet 2.

  • HyperX can handle zero-length CBUSH elements (where 'Grid A' and 'Grid B' are coincident) for single and multi-lap joints with the following considerations:

    • They require a reference coordinate system, and the X-axis direction of that reference CS becomes the axial direction in HyperX.

    • Zero-length CBUSH elements in multi-lapped joints must all reference the same or identical coordinate systems, or HyperX won’t recognize them as being part of the same joint.

    • You can create a multi-lap joint that is a mix of zero-length and non-zero length CBUSHs, as long as the zero-length CBUSHs have a CS X-axis that aligns with the Grid A to B direction of the non-zero length element.

HyperX and FEM Organization

INCLUDE Files

HyperX will maintain and understand your INLCUDE file structure. Recommended Include file structure is shown below.

IncludeFile_IdealStructure.png

If your model is organized by INCLUDE file, it can be useful to view the FEM Tree in terms of "Include View," indicated in the screenshot below. In this example, by clicking on the Aeroshell - Lower node, all of the elements from the Aeroshell - Lower INCLUDE file is selected. A Structure can now be quickly created by using the right-click menu.

TransFEM_IncludeFile_Example.png

HyperMesh Assemblies and Components

The HyperMesh preprocessor will export comments containing information on the Components and Assemblies belonging to a particular model. HyperX will recognize these entities as FEM Tree nodes and selectable items - allowing you to quickly isolate these entities and organize them in HyperX as needed.

TransFEM_HyperMeshEntities.png

Element SETS

HyperX will recognize element sets defined in the FEM - typically invoked with the Nastran ELSET command. Each element set corresponds to a node on the FEM Tree, which can then be selected/isolated/etc.

The FEM Tree

The FEM Tree, found on the left-hand side of the Viewport, facilitates the organization of all FEM entities - elements, properties, grids, materials, and coordinate systems. It can also show entities organized by INCLUDE Files and HyperMesh.

All FEM entities listed in the Tree can be hidden, shown, or selected using the right-click menu. Like all other Trees, any entity that is selected in the FEM Tree (and is currently 'shown' in the Viewport) will be highlighted. Also note that hovering the cursor over a single node will show the corresponding FEM definition, taken directly from the input file. Selected elements and properties can be placed into new Structures via the right click > Create Structure option.

FEMTree_Example.png
Structures

The Model Tab of the Ribbon

The Model tab contains operations related to import/export of FEM models, Project unit display, and import/export of CAD.

Ribbon-model.png

The function of each button is more explicitly explained below:

  • FEM Import – Import Finite Element Model with user-specified selections. See How To Import a FEM.

  • FEA Results Import – Import results of Finite Element Analysis.

  • Design Loads – View/modify reference temperature, limit/ultimate load factors, and multipliers defining case combinations for selected Design Load Cases.

  • Load Extraction Method (rise-up) – Create a Load Property with corresponding method (average, peak element, element based, etc.) for extraction of FEA loads within Zone/Joint boundaries.

  • Exclude Elements – Select elements to be excluded from force summation and analysis. See How to Exclude Elements from Sizing/Analysis.

  • FEA-Like Loads (rise-up) - Define user-defined stress resultants to be assessed during Sizing/Analysis. See Non-FEA Design Loads.

  • User-Defined Loads (rise-up) - Analysis-specific user-defined loads to be assessed during Sizing/Analysis. See Non-FEA Design Loads.

  • Project Units – Control of Project unit display in relation to units modeled in the FEM (English, SI, or custom).

  • Measuring Tool - Measure distances between CAD and HyperX entities. See Measuring Tool.

  • Change Material Direction - Project a vector to material coordinates for selected plate elements.

  • FEM Export – Export of finite-element model with design sizing results from HyperX.

  • Import CAD - Import CAD geometry (Points, Curves, Surfaces) into the current Project. See How To Import and Export CAD Entities.

  • Export CAD - Export CAD geometry (Points, Curves, Surfaces) to selected file type. See How To Import and Export CAD Entities.

  • Generate CAD Stiffeners - Generate 2D or 3D CAD stiffener entities from existing Sizing results.

  • Create CAD Entities (rise-up) - Options to create new CAD Points or Curves in the HyperX interface. See How To Create CAD Entities.

  • Modify CAD Entities (rise-up) - Options to edit existing CAD entities in the HyperX interface. See How to Modify CAD Entities.

  • Discrete Fields - Open the Library to create and manage custom tabular data. See Discrete Fields.

  • Discrete Field Modifiers (rise-up) - Map and project external Discrete Field tables to the FEM.

Structures

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