Engineering analysis + design software

User Area > Advice

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

Interface joint elements can be used to connect surface elements (e.g. shells) without full fixity. This mesh is assigned to the two line features on the edge of the two separate surfaces (one line is designated "master" and one "slave"). The gap between these surfaces could be zero.

The approach outlined below will enable the generation of (for example) moment release between surfaces meshed with shell elements

Geometry - Surface and Line Features

Where a connection between two surface features with a coincident edge is required, a joint mesh can be created between the two parallel line features. A gap may be temporarily created between the two lines to aid modelling.  A gap may be created, for example, by making a copy of one surface feature with the desired offset, and the original surface deleted.

New Geometry

When creating the geometry from scratch the points and lines at the interface must be made "unmergable", so that they are not automatically merged by LUSAS Modeller if they share the same coordinate positions. This can be done by selecting the features and using the following menu items as appropriate:

Geometry > Point > Make unmergable

Geometry > Line > Make unmergable

Modifying Existing Geometry (Example)

In this case the geometry is already created with lines shared between the surfaces along X=0.  To separate these surfaces and ensure that they are not connected we need to unmerge the lines and points between them.  This can be done by selecting one point (eg P47) and one surface (eg. S21) and then go to:

 Geometry > Point > Unmerge

Surface 21 is deleted and replaced by surface 22 as shown.  Now line 59 and point 63 only belong to surface 22.  The new coexistent point 47 and line 37 belong to the opposite surface 14.  These new features are automatically set as unmergable. 

The two surfaces are now only connected at point 41.  To resolve this, point 41, and this time, the line 55 (of surface 22) are selected and again, go to:

Geometry > Point > Unmerge

This process is repeated, as if unstitching the surfaces, until the surfaces that meet at X=0 are separated.

Joint elements have no length in a stiffness matrix and so any length given in the model may result in a solution that is not in true moment equilibrium.  A warning to this effect will also occur in the LUSAS Solver text output file (*.OUT), and echoed to the Text Output window in Modeller. However, moving the features at each end of joint elements to be coincident can make it difficult to be sure of the orientation of the joints element axes (local x, y, z).  Therefore it is prudent always to use a local coordinate dataset to control the axes, which can be specified when assigning the joint mesh.

Mesh Attributes

Surfaces should be meshed in an appropriate manner, usually using shell or plate elements.

The appropriate mesh to connect to all 6 degrees of freedom for thin shells (QSI4), thick shells (QTS4, QTS8) and 3D beam elements is "joint for beams 3D" (JSH4).  Where no rotational stiffness is required however, it may be more appropriate to use "joint no rotational stiffness" (JNT4).  This reduces the input required for JSH4 as the rotational stiffnesses do not need to be calculated.

A local coordinate dataset to control the element axes orientation for the joints should be defined before the joint mesh attribute is assigned. More information on local coordinates may be found in the help menu item:

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

A JNT4 mesh (for no rotational stiffness at all) may be defined using the menu item:

Attributes > Mesh > Line > (drop down menus) Generic element type=Joint no rotational stiffness, Number of dimensions=3

The mesh definition should include the number of divisions along the lines of the surface features to be joined.

The mesh is assigned by selecting one line and adding it to the selection memory (this will be the ‘slave’ of the joints).  Then the opposing second line is selected and the joint mesh attribute is assigned by dragging and dropping it from the Attributes TreeView onto the model in the graphics window. Clear the selection memory after assigning the mesh. 

If the option "Mesh from master to slave" is ticked, then the points in normal selection will become the 'Master' assignments to which material and geometric attributes for the joint are then to be assigned.  The points in the selection memory will become slave points. For a linear joint material the order of master and slave lines does not matter.  The joint interface mesh is described in the help menu item:

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

When assigning the joint mesh attribute a local coordinate dataset may be specified to orientate the joint elements, if one is already defined (recommended approach for controlling joint local axes).  After meshing, the element axes can be visualised using:

TreeView > Layers tab > Mesh > (check) Show element axes

Geometric Attributes

Geometric properties are required for the 6-degree-of-freedom (6 DOF) JSH4 elements, but not for the 3-degree-of-freedom (3 DOF) JNT4 elements.  Refer to the Element Reference Manual for further information regarding the particular joint elements used.  To specify a geometric attribute for JSH4 elements go to:

Attributes > Geometric > Joint

to define a geometric eccentricity, which can be zero unless otherwise required.

Material Attributes

Surfaces should have an appropriate material attribute assigned (e.g. concrete, steel etc). 

The joint material attribute used controls how the joint will behave. Materials appropriate to common uses of joints are described below; full information on all available joint materials is given in the Help:

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

See also:


Help > Help topics > Contents > Modeller Reference Manual>Chapter 5 : Model Attributes>Material Properties>Joint Material Properties

For a simple hinge JNT4 joint with no rotational stiffness:

Attributes > Material > Joint > (drop down lists) Joint type=Spring stiffnesses, Freedoms=3

The material needs to be defined with 'Assignment' to 'Lines'. 

The number of "Freedoms" specified in the material should match the DOF in joint mesh attribute selected.  A stiffness value for each DOF should be entered. For JNT4, Freedom=3 should be used: the DOF are, in order, local x, y, z. For JSH4, Freedom=6 is appropriate: the DOF are, in order, local x, y, z, Thx, Thy, Thz. 

The image below demonstrates the use of joint elements to create a hinge connection between two shell surfaces.

For more information on the calculation of spring stiffnesses, please see Spring stiffnesses for joints

Ref: CSN/LUSAS/1017

Joints: Mesh | Geometric attributes | Material attributes | Spring stiffnesses | Supports | Loadcase properties

innovative | flexible | trusted

LUSAS is a trademark and trading name of Finite Element Analysis Ltd. Copyright 1982 - 2022. Last modified: November 29, 2022 . Privacy policy. 
Any modelling, design and analysis capabilities described are dependent upon the LUSAS software product, version and option in use.