Oasys GSA Documentation

# 2D Element Properties

There are two different classes of 2D elements. The basic 2D element is the normal finite elements used for structural applications included in-plane and/or out-of-plane behaviour. The load panel element is a non-structural element used to apply load to beam elements.

# Property Type

Name

The name is only used as a convenient way of identifying a 2D element property.

Color

Define the color of the elements that use this property when element coloring by property on graphic view

Element Type

The types of 2D properties available will depend on the structure type. For the 2D structure types (plane stress, plane strain and axisymmetric) only the type corresponding to the structure type is available. Likewise for non 2D structure types the plane strain and axisymmetric types are not available, although the plane stress option is. The types are:

  • Plane Stress – in plane effects only (no out of plane stress)
  • Plane Strain – plane effects only (no out of plane strain), it is only active/used when the Structure Type is "Plane strain"
  • Axisymmetric – in plane effects only (the out of plane direction is the hoop direction), it is only active/used when the Structure Type is "Axisymmetric"
  • Fabric – in plane effects only (no thickness associated with fabrics)
  • Flat Plate – out of plane effects only
  • Shell – in-plane and out-of-plane effects
  • Curved Shell – a general shell element which may be curved out of plane, Curved shell cannot be used in GSA analysis at present, it can be used to build a GSA model and export to other software to do the analysis
  • Load Panel – an element which is used only for the distribution of loads. It has no stiffness, so does not need material or thickness parameters. For more information see 2D Loads on Load Panels

Axis

Users may assign an axis to be used to define the orientation of 2D elements. If the axis is set to “Topological” the orientation of the element will be determined by the first two nodes of the elements and the orientation angle. If an axis (global or user defined) is assigned here then that axis will be projected on to the element plane to determine its orientation.

Material

The material definition breaks into three parts. The first part is the material type. it is one of:

  • Steel
  • Concrete - if it is concrete, then concrete slab property can be set for RC slab design
  • FRP
  • Aluminium
  • Timber
  • Glass
  • Fabric
  • <undefined> – not associated with any grade

The second part is material grade index that this 2D property refers to. The material grade with actual material design properties is defined in material grade table. If material type is assigned and material grade is defined, analysis can use this material grade as the analysis material when "from Grade" is used in "Analysis" column.

The third part is the Analysis material index that this 2D property refers to. The analysis material property can be defined in Analysis Material table. If analysis material is set to "from Grade", then the material properties defined by the material grade will be used in the analysis.

Concrete Slab Property

The Concrete slab property is used in concrete slab reinforcement.area calculations

Profile/Thickness

In the simplest case this defines the thickness of the 2D elements. No thickness definition is needed if material type is fabric, and a unit thickness is assumed for plane strain and axisymmetric structure types. For a shell element there are four options for defining the property

  • Solid – just the thickness
  • Decking slab – a composite concrete slab based on steel decking and is defined on the next page of the dialog
  • Hollow – a hollow core concrete slab and is defined on the next page of the dialog
  • Layered composite – a layered shell that needs to be exported to LS DYNA for analysis and is defined on the next page of the dialog

Reference Surface

The reference surface is a virtual plane that the in-plane forces are assumed to act in a 2D element. If the reference surface is the top or bottom surface, in-plane loads will also generate a bending moment. The reference surface setting is only used by shell elements. There are two parameters to define the reference surface, "Surface" defines top, middle or bottom of the 2D elements as the reference surface, "Offset" defines an extra offset from the selected top, middle or bottom surface. If offset is zero, then the selected top, middle or bottom surface will be the final reference surface.

Property Modifiers

There are four factors, three for stiffness modifications and one for volume modification. The three stiffness modifiers are for in-plane stiffness, bending stiffness and through thickness shear stiffness, the volume modifier is for modifying the volume that is used to calculate the mass and self-weight of the elements. By using the property modifiers, the 2D element properties can be different from those calculated by the given thickness which may be useful to deal with situations such as cracked concrete slabs (reduced bending stiffness due to cracking) or hollow slabs where the stiffness of the slab in bending and in-plane will be less than that for a solid slab.

The modifiers can be an absolute values or a percentage of the calculated values from the given thickness. For Plane Strain, Axisymmetric or Fabric elements, these modifications are not relevant so they are not enabled.

The stresses in 2D elements are calculated using unmodified thickness.

Additional Mass

Normally the gravity loads on a 2D element are calculated from the density and thickness or modified volume. Fabric elements have no thickness but it may still be desirable to assign a mass, or where a slab is modelled which has a non-structural screed that adds mass. Both of these situations are provided for by the additional mass per unit area. This mass is in addition to the mass implied by the thickness and density.

Support pattern & reference edge

The support pattern and reference edge are applicable only to load panel elements. The support pattern defines the number of edges to which the load is transferred and the reference edge sets the selection of the free/loaded edges. For more information see 2D Loads on Load Panels