2D Member Element Types & Behaviours

This chapter describes the theoretical background for the available types and behaviours of 2D members in SCIA Engineer.

Important note

At this time, SCIA Engineer offers two types of very similar objects:

Load panels are a long known feature of SCIA Engineer. Their behaviour and features remain unchanged.

2D members with element type = Load panel offer the same basic functionality as load panels, plus some extensions:

• the type and behaviour of a 2D member maybe be modified at any time; for instance, a 2D member, initially defined a standard FEM plate, may be converted into a load panel - more accurately, a 2D member with element type = Load panel
• 2D members with element type = Load panel support a few types of loads that are not supported by load panels

For more details, read the following text. However, please keep in mind, that the two types of objects mentioned above are distinct and must not be confused.

2D element types

In SCIA Engineer, a 2D member can have one of the following types:

Standard	Standard 2D member, used for the analysis of generic plates, walls, shells. Its properties are typically defined by a thickness (uniform or variable) and a material.
Metal deck	2D member with settings dedicated for the analysis of metal decks, i.e. deck made of a profiled steel sheeting. The type of sheeting is obtained from a library and its orthotropic properties are calculated from the geometry of the sheeting. This type is supported only for 2D members with a plane geometry.
Composite deck	2D member with settings dedicated for the analysis of composite decks, i.e. deck made of a profiled steel sheeting with a concrete topping. The type of sheeting is obtained from a library. The orthotropic properties of the deck are calculated from the geometry of the sheeting. This type is supported only for 2D members with a plane geometry.
Load panel	Virtual surface for the application of loads. Its purpose is to transmit loads to the structure, without introducing any additional stiffness into the model. See the chapter related to load panels for more information. This type is supported only for 2D members with a plane geometry.

The Load panel element type is available only in the 64-bit version of SCIA Engineer. To use a load panel in the 32-bit version, create a load panel directly from the dedicated options in the structure service tree.

2D element behaviours

A 2D member can have one of the following behaviours:

Diaphragm element behaviours are available only for element types Composite deck and Metal deck

Standard FEM	The 2D member is taken into account in the analysis model as a finite element plate
Flexible diaphragm	The 2D member has no in-plane shear stiffness nor shear stiffness in the analysis model. The loads applied to it, as well as its self-weight, are transmitted to the supporting members in the same way as for a load panel; in-plane loading is transferred only axially, without transverse diffusion.
Rigid diaphragm	The 2D member has no bending stiffness and infinite in-plane stiffness in the analysis model. The loads applied to it, as well as its self-weight, are transmitted to the supporting members in the same way as for a load panel.
Semi-rigid diaphragm	The 2D member has no bending stiffness. Its in-plane stiffness is taken into account in the analysis model by means of a finite element mesh. The loads applied to it, as well as its self-weight, are transmitted to the supporting members in the same way as for a load panel.

See a comparison of the in-plane behaviour of various diaphragm types in Composite Analysis Model: Diaphragm Types.

The following table summarizes the features of the various element behaviours. The load panel element type is added at the bottom of the table, as it also has its own special behaviour.

Behaviour	Bending stiffness	In-plane stiffness	Load transfer	Self-weight
Standard FEM	FEM	FEM	FEM	yes
Rigid diaphragm	none	infinite	load panel	yes
Semi-rigid diaphragm	none*	FEM	load panel	yes
Flexible diaphragm	none*	FEM (no shear)	load panel	yes
Load panel	none	none	load panel	no

* unlike for rigid diaphragms, the bending stiffness of flexible and semi-rigid diaphragms is actually not zero. Such diaphragms are taken into account in the analysis model as a Standard FEM 2D member with a reduced bending stiffness (default = 1/1000 of nominal bending stiffness). Additionally, for flexible diaphragms, the in-plane shear and Poisson's components are set to zero (d₁₂ and d₃₃ components of the 2D orthotropy matrix).

Standard FEM 2D member

• has both bending and in-plane stiffness, depending on its geometry and material properties; various options are available for altering the behaviour (property modifiers, nonlinear behaviours, etc...)
• is analyzed in the FEM model using standard finite element mesh
• loads applied to the 2D member are directly sent to the solver and applied to the finite element mesh

Load panel & Load panel 2D member

• has no stiffness, no mechanical properties
• is not taken into account in the FEM model
• loads applied to the load panel are distributed to the beams (or other structural entities) underlying the load panel; only the generated loads are sent to the solver and applied to the corresponding finite elements

Diaphragm 2D member

• is a hybrid entity, between Standard FEM and Load panel
• has in-plane stiffness
• has no bending stiffness
• is taken into account in the FEM analysis model in various ways, depending on the selected type of diaphragm; see details below
• exactly in the same way as for a load panel, loads applied to the diaphragm are distributed to the beams (or other structural entities) underlying the diaphragm; only the generated loads are sent to the solver and applied to the corresponding finite elements

Rigid diaphragm 2D member

• no finite element mesh
• a rigid diaphragm constraint (similar to a rigid link) ensures that the diaphragm acts as a rigid body in its own plane, but has no out-of-plane stiffness

Semi-rigid diaphragm 2D member

• uses a finite element mesh, in the same way as a standard FEM 2D member
• the bending stiffness is the nominal standard FEM stiffness divided by a reduction factor (default k_red = 1000)
• the in-plane stiffness is the nominal standard FEM stiffness, unchanged

The corresponding, modified orthotropy matrix can be written as follows:

Flexible diaphragm 2D member

• uses a finite element mesh, in the same way as a standard FEM 2D member
• the bending stiffness is the nominal standard FEM stiffness divided by a reduction factor (default = 1000)
• the in-plane stiffness is the nominal standard FEM stiffness with its shear and Poisson's components (d₃₃ resp. d₁₂) set to zero

The corresponding, modified orthotropy matrix can be written as follows:

Supported load types

Load type	2D Member		Load Panel
	element type = Load Panel or element behaviour = Flexible/Rigid/Semi-Rigid Diaphragm	element behaviour = Standard FEM
Point force in node	✔ Supported 1	✔ Supported	✘ Not supported 4
Point force – free	✔ Supported 2	✔ Supported	✔ Supported 2
Line force on 2D member edge	✔ Supported 1	✔ Supported	✘ Not supported 5
Line force – free	✔ Supported 2	✔ Supported	✔ Supported 2
Surface load on 2D member	✔ Supported	✔ Supported	✔ Supported
Surface load – free	✔ Supported	✔ Supported	✔ Supported
Thermal load on 2D member	✘ Not supported 3	✔ Supported	✘ Not supported 5
Moment on node	✘ Not supported 3	✔ Supported	✘ Not supported 4
Moment – free	✘ Not supported 6	✔ Supported	✘ Not supported 6
Line moment on 2D member edge	✘ Not supported 3	✔ Supported	✘ Not supported 5
2D member displacement, curvature	✘ Not supported 3	✔ Supported	✘ Not supported 5
Single Traffic Load	✔ Supported	✔ Supported	✔ Supported

¹ Load transfer method must be set to ‘Accurate(FEM), fixed link with beams’ or ‘Accurate(FEM), hinged link with beams’

² Except for load transfer method ‘Tributary Area’

³ Load can be applied but a warning message explaining that the load will be ignored will be displayed prior to analysis

⁴ Cannot be applied since a node cannot be added to a load panel

⁵ Cannot be applied since a load panel is not a 2D member

⁶ The load is ignored

Special cases

Openings

Opening on a 2D member with element type = Load panel or element behaviour = Flexible/Rigid/Semi-Rigid Diaphragm

• If the opening has the option “Load panel” switched ON, the opening is completely ignored. Loads applied inside the opening are applied to the 2D member, as if there would be no opening
• If the opening has the option “Load panel” switched OFF, all loads applied inside the opening are ignored

Opening on a 2D member with all other element behaviour = Standard FEM

• If the opening has the option “Load panel” switched ON, loads applied inside the opening are transferred to the edges of the opening
• If the opening has the option “Load panel” switched OFF, all loads applied inside the opening are ignored

Openings on a Load panel

• All loads applied inside the opening are ignored

Copying 2D members

If a 2D member (with element type set to “Load Panel” or with element behaviour set to “Flexible diaphragm”, “Rigid diaphragm”, or “Semi-Rigid Diaphragm”) has ‘Selection of Entities’ set to ‘User Selection’ and the member is copied, in the newly created copy, the entity selection will be lost (i.e. no entities are selected for load transfer in the copy).

Effect on Buckling Length

All 2D members (except 2D members with element type set to ‘Load Panel’) will brace and, therefore, affect the buckling length, of any 1D element which they intersect.

Average Number of Tiles of 1D elements linked to a Rigid Diaphragm

When plate ribs are used with a rigid diaphragm, the ‘Average number of tiles of 1D elements’ (Mesh setup) should be set to 4 or higher in order to obtain accurate results. If a rigid diaphragm with plate ribs exists in a project and this number is not set to 4 or higher, a warning message will appear during analysis. By clicking ‘OK’ for this warning message, the program will change this value to 4 automatically.

Integration Strips

An integration strip may be added to a 2D member with element type set to “Load Panel” or with element behaviour set to “Rigid diaphragm”, however, since there the 2D member has no physical in-plane stiffness, there are no results available. A warning message will be displayed explaining that results are not available.