How do I model a hinged connection between shell meshed surfaces?

Engineering analysis + design software

User Area > Advice

How do I model a hinged connection between shell meshed surfaces?

Joint elements can be used to model a hinged connection between two surfaces meshed with shell elements.

There are two assignment types:

Between two features (manual) - For this, a joint mesh attribute must be assigned to two features. The gap between the two features may be zero.
On single feature (automatic) - For this, a joint mesh attribute must be assigned to a single feature.

The approach outlined below uses the Between two features (manual) assignment type.

Geometry - Surface and Line Features

A joint mesh attribute can be assigned to the coincident edges (line features) of two surface features to create a connection between the surfaces. To facilitate the modelling process, a temporary gap may be introduced between the lines. A gap can be introduced by making a copy of one of the two surface features with the required offset and then deleting the original surface feature.

Creating New Geometry

When creating the geometry from scratch, the points and lines at the interface must be made unmergable to prevent LUSAS Modeller from automatically merging features that share the same coordinate positions. This can be achieved by selecting the relevant features and using the appropriate menu options as follows:

Geometry > Point > Make unmergable

Geometry > Line > Make unmergable

Modifying Existing Geometry (Example)

In this case, the geometry has already been created, with lines shared between the surfaces along X=0. To separate the surfaces and ensure that they are not connected, the shared lines and points must be unmerged. This can be done by selecting one point (e.g. P47) and one surface (e.g. S21), and then navigating to:

Geometry > Point > Unmerge

Surface 21 is deleted and replaced by Surface 22, as shown. Line 59 and Point 63 now belong only to Surface 22. Point 47 and Line 37 belong to Surface 14. The new features are unmergable.

The two surfaces are now connected only at Point 41. To disconnect them, select Point 41 and Line 55 belonging to Surface 22, then navigate to:

Geometry > Point > Unmerge

This process is repeated until all surfaces meeting at X=0 are fully disconnected.

Joint elements have no physical length in the stiffness matrix, and therefore any length assigned to them in the model may result in a solution that is not in true moment equilibrium. A warning to this effect is also provided in the LUSAS Solver text output file (*.OUT) and echoed in the Text Output window in Modeller.

It is recommended to use a local coordinate dataset to control the orientation of the joint element axes. The local coordinate dataset can be specified when assigning the joint mesh attribute.

Mesh Attributes

Surfaces should be meshed using an appropriate element type, typically shell or plate elements.

Where both translational and rotational stiffnesses need to be specified, the Joint for beams element type (JSH4) must be used. Where rotational stiffness is not required, the Joint no rotational stiffness element type (JNT4) should be used. In this example, JNT4 elements are used.

A local coordinate dataset should be used to control the orientation of the joint element axes. Further information on local coordinates can be found under the following Help menu item:

Help > Help Topics > Contents > Modeller Reference Manual > Chapter 5 : Model Attributes > Other Attributes> Local Coordinates

The number of divisions specified in the mesh definition must match the number of divisions along the lines of the surfaces to be joined.

The joint mesh attribute must be assigned to pairs of opposing lines. This can be achieved using either of the following methods:

First method: Select the two opposing lines in sequence, then drag and drop the joint mesh attribute from the Attributes TreeView onto the model in the graphics window. The first line selected becomes the primary assignment, and the second line becomes the secondary assignment. The joint geometric and material attributes must be assigned to the primary assignment line. Repeat this process for each pair of opposing lines.
Second method: Select the lines along one side of the gap and add them to the selection memory. Then select the corresponding lines along the opposing side of the gap and drag and drop the joint mesh attribute from the Attributes TreeView onto the model in the graphics window. The lines stored in the selection memory become the secondary assignments, and the opposing lines become the primary assignments. The joint geometric and material attributes must be assigned to the primary assignment lines.

For a linear joint material, the order in which the lines are selected does not affect the joint response.

The joint interface mesh is described in the following Help menu item:

Help > Help Topics > Contents > Modeller Reference Manual > Chapter 5 : Model Attributes > Meshing > Joint/Interface Element Meshes

After meshing, the joint element axes can be visualised by visiting the Layers treeview and selecting Mesh > (check) Show element axes

Geometric Attributes

A joint geometric attribute may be assigned where required. This attribute allows a joint length and eccentricity to be specified. Further information can be found in the Element Reference Manual.

If no joint geometric attribute is assigned, the joint length and geometric eccentricity are assumed to be zero.

Material Attributes

The joint material attribute controls the behaviour of the joint. Further information on all available joint materials can be found in the Help system:

Help > Help topics > Contents > Theory Manual Volume 1 > Chapter 4 Constitutive models > 4.12 Joint Models