User Tools

Site Tools


This is an old revision of the document!

Structural Modeling

OpenVSP allows a user to model aerospace structures for a geometry and generate a finite element mesh model. This model can then be exported to an FEA post-processing tool for further analysis. To begin, a geometry must first be created or loaded. The FEA Mesh GUI is accessed by clicking “FEA Mesh…” in the Analysis pull down menu.

VSP Terminology


A structure is defined as a collection of FEA parts associated with a single geometry. A geometry is able to have multiple structures.

FEA Part

An FEA part is any structural entity that is used to define a structure. This includes full-depth, zero-depth, and key-point types of entities.


A structural entity that passes entirely through a geometry is considered full-depth. Triangular shell elements are used to define the surface of the full-depth entity. Examples of full-depth aerospace structures include ribs, spars, and floors.


A zero-depth structural entity is defined along a sub-surface edge or the intersection of two surfaces. A series of beam elements define the zero-depth feature. Stringers, longerons, and other stiffeners are represented as zero-depth entities.


A specific FEA node that is fixed in space is referred to as a key-point (used interchangeably with fixed point). Key-points can be used to provide connectivity to other FEA meshes. The can also be used to apply a point load or mass at a specific location.

FEA Element

A group of interconnected FEA nodes create an FEA element. All elements are assigned a single element property.

FEA Node

An FEA node is a 3D coordinate point used to build FEA elements. FEA nodes may be assigned to multiple elements. Key-points are FEA nodes that have been defined at a specific location.


Shells are full-depth FEA parts comprised of triangular FEA elements. In NASTRAN these elements are CTRIA6. In Abaqus and Calculix they are S6 elements.


A cap is a zero-depth FEA part made up of beam FEA elements. The beam elements are represented in NASTRAN as CBAR. In Abaqus and Calculix they are B32 elements.

FEA Mesh Screen

Visible on all tabs of the FEA Mesh GUI are the status window, currently selected structure output, and “Mesh and Export” button. The status window is mainly used to display the status of FEA mesh generation, which is run as a separate process. However, error messages and warning will also be displayed. The current structure output list which structure is selected in the structure browser on the Structure tab. This is the structure that willl be used to create the FEA mesh when “Mesh and Export” is selected.

Structure Tab

The main function of the Structures tab is the addition and removal of structures for the vehicle. At the top of the tab under “General”, there is a link to this wiki. Below, the unit system for the vehicle can be specified. All of the FEA export file formats are unitless, so the following options are available to ensure consist units:

  • Insert Unit System Chart

The structure browser lists all of the structures for the vehicle, along with their name, parent geometry, and surface index. Below the browser, all available geometries for which a structure may be added to are listed. The available surface indexes for each geometry are also listed. All geometry types, with the exception of Blank and Hinge, are available to add a structure to. In addition, more than one structure may be added to a geometry. The “Add Structure” button will create a new structure on the geometry and surface indicated in the above choices. “Delete Structure” will, as expected, delete the structure that is currently selected in the browser. The name of the currently selected structure may be edited below the add and delete buttons. When a structure is selected, the degenerate geometry preview can be displayed under “Orientation”. This feature is particularly useful for wing structural layups, where a top-down 2D view will be shown. The display options can also be changed in the Geom Browser under “Surface”.

Part Tab

The Part tab provides organization and control of FEA parts for the selected structure. The browser at the top of the tab lists all FEA parts for the structures, and includes their name, type, structural entity type, and property assignment. To the left of the browser are controls for reordering FEA parts. The ordering of parts in the browser is important in the case of overlap conflict, where priority is given to the part higher up in the browser. For example, if two FEA sub-surfaces overlap, the overlapping region is tagged according to the FEA part earlier in the list. Another feature of the browser is that multiple FEA parts can be selected at once. The options under “General” can then be set for the group of selected parts (this is also true for a single selection).

Material Tab

The Material tab contains a library of linear, temperature-independent, isotropic materials. In NASTRAN, these are defined by the MAT1 keyword. Materials in the library are available to all structures and are saved with the vehicle, i.e. there is no need to recreate materials for different structures. The browser at the top of the Materials tab lists all materials in the library. The default materials available are Aluminum 7075-T6, Aluminum 2024-T3, Titanium Ti-6AI-4V, and AISI 4130 Steel. To add a material, simply select “Add Material” and adjust the parameters for mass density, elastic modulus, Poisson's ratio, and thermal expansion coefficient to the desired values.

Property Tab

Similar to the Material tab, the Properties tab contains a library of FEA element properties which are available to all structures. Properties can either be shell properties or beam properties. The browser at the top of the Properties tab lists all of the properties available in the library. There must be a minimum of one shell and one beam property at all times. A default shell and beam property are provided, and can be edited as desired. To add a new property, simply specify the type and click the “Add Property” button. The selected property can be renamed or deleted (unless it is the last of its type). For shell properties, the only defining parameters are a material and thickness. Shell properties are written in Calculix and Abaqus export files with the SHELL SECTION keyword. In NASTRAN, PSHELL is used. Like shell properties, beam properties are also assigned a material. The cross section of the beam element defines the parameters needed for the beam property. The available cross sections are General, Circle, Pipe, I, Rectangle, and Box. In Calculix and Abaqus, the “Beam General Section” keyword is used if the cross section is general, and “Beam Section” is used for all other cross section types. Similarly, PBAR defines general cross sections in NASTRAN while PBARL defines all other cross section types. The “Show XSec” button next to the cross section type opens a new window with a dimensioned drawing of the cross section type. Once the FEA properties library has been built up, properties can be assigned to individual FEA parts. As would be expected, shell properties can only be assigned to triangular shell FEA elements and beam properties can only be assigned to beam FEA elements.

Mesh Tab

The Mesh tab is available for controlling aspects of the solver used during the generation of an FEA mesh. The options available here are similar to those seen on the Global tab to the CFD Mesh GUI. Further insight into these settings can be found here: CFD Mesh Wiki. Below the mesh control settings, the files exported during FEA mesh generation are listed. The first two, *.stl and *.msh, are general mesh formats that do not include any materials or properties. The mass output file below these is a *.txt file that lists the mass of each FEA part, divided between the shell and beam FEA elements. The remaining two export files are *.dat files written in NASTRAN and Calculix/Abaqus FEA mesh format. These files may be imported to an external FEA mesh program for further processing and analysis.

Display Tab

The Display tab is used to control visualization of the generated FEA mesh. Therefore, it has no functionality until the “Mesh and Export” button has been selected. At the top of the tab under “Display”, toggle buttons are available for controlling the display of all FEA elements selected in the set. “Draw Mesh” displays the borders of each triangular shell element. “Color Elements” is used to apply a different color to each element set. “Draw Nodes” provides visualization of the individual FEA nodes. “Draw Element Orientation Vector” draws the normal vector for beam elements and a vector pointing in increasing U direction on the surface of shell elements. Since the FEA mesh is unstructured, this orientation vector is important to know if laying out composite laminate layers for shell elements. Under “Display Element Sets”, FEA parts are grouped by their shell and beam elements. Their visibility is controlled by the check boxes next to each set or by using the “Show All” and “Hide All” buttons.

FEA Part Types


The one FEA part common to all structures is skin. Skin is defined as the outer mold line (OML) of the parent geometry of the structure. The skin is automatically added upon the creation of a new structure, and can not be removed. The skin is composed of shell FEA elements, which the property for can be specified. The only additional option available for skins in the FEA Part Edit GUI is to delete the skin triangles after the FEA mesh has been generated.


Slice is a 2D cutting plane that is used to intersect a skin. A slice can be full-depth, zero-depth, or both, specified by selection of “Shell”, “Cap”, or “Shell and Cap”, respectively. The cutting plane for a slice is defined by an orientation, center location, and rotation. Orientation is the plane in which the slice runs parallel to. This can be defined off of either the absolute axes or the body axes of the parent geometry. An option is available to specify distance as either relative or absolute. Relative specifies the center location of the slice as a fractin of the bounding box of the parent geometry. Absolute means a fixed location within the bounding box is used as the slice center.


Ribs are a derivation of slice made specifically for wing geometries. Ribs are defined from the leading edge to the trailing edge of the wing, parallel to the local XZ plane. In the FEA Part Edit GUI, “Edge Normal” is used to specify the rib as perpendicular to the wing's leading edge, trailing edge, or any spars that have been added to the structure.


Spars are another extension of slice made for wing geometries. They are defined from the root to tip of the wing, oriented vertically along the local XZ plane. An optional control is included to constrain a spar to a specific wing section, useful for a multi-section wing.


Dome is a semi-elliptical cutting surface, which can be used to model pressure bulkheads and similar aircraft structures. The parameters used to define a Dome are radius (A, B, C), location (X, Y, Z), and rotation. The center of the dome can be constrained to a location along the spine of the parent geometry. This allows the dome to react more parametrically to changes made to the parent geometry. It is important to note that domes must be oversized manually to correctly intersect the skin, due to the fact that the skin-dome intersections are not calculated until FEA mesh generation begins. Another item to note is that dome is not available for wing geometries.

Fixed Point

A fixed point, or key-point, is a forced FEA node at a specified surface location (UW coordinates). Fixed points can be placed on the parent skin surface or any available FEA part surface. A fixed point can also be turned into a mass element, defined as CONM2 in NASTRAN and MASS in Calculix and Abaqus, and assigned a mass value.

FEA Sub-Surface

Sub-surface modeling capabilities have been extended to structures with line, rectangle, ellipse, and control surface sub-surface types. All of the same options and parameters for “normal” sub-surfaces have been made available to FEA sub-surfaces. However, sub-surfaces defined for a geometry are not automatically transferred when a structure is created. FEA sub-surfaces can be used to assign properties to specific areas, define separate element sets, cut holes in a surface, and create beam elements. “Tag” is used to specify which triangular shell elements are identified as belonging to the FEA sub-surface. If “Cap (no-tris)” is indicated for an FEA sub-surface, all shell elements tagged for the sub-surface will be deleted and a hole will be left.


Arrays are groups of FEA parts defined by their start and end location, spacing, and direction. The three types of arrays are rib array, slice array, and line array. Many of the same options and features available to the individual FEA part type are available for the array as well. If a specific number of parts is desired for the array, “Relative” should be indicated for distance. “Absolute” ensures a fixed distance between parts in the array. All arrays have the option to be individualized, which turns the array into individual FEA parts. However, this action cannot be reversed.

API and Scripting

Best Practices

References and Further Reading

feamesh.1504912650.txt.gz · Last modified: 2018/04/01 14:40 (external edit)