Skip to content

Tendon

The Tendon element is used to simulate tendons or embedded rebars and can be defined using the Tendon element type and the Tendon section type. The parent elset must be defined as an individual property of the element. For tendon analysis, tendon stress can be applied using the Field value. The applicable parent elements are as follows:

  • 2D Beam Elements (Beam2D): B2D2H, B2D2MH
  • 3D Beam Elements (Beam3D): B3D2H, B3D2MH
  • Shell Elements (Shell): S3F, S4F, S3, S4, ...
  • Solid Shell Elements (CShell): CS6, CS8, ...
  • 2D Plane Solid Elements (Plane): CPE4, CPS4, CAX4, ...
  • 3D Solid Elements (Solid): C3D8, ...

The parent elset applied to the Tendon element must consist of elements from the same element group. The profile of the Tendon element is defined as a spline geometric shape. If the parent elset is a beam element group, the spline is defined in the ECS and is subject to the following constraints:

  • The beam elements must be continuously connected (a sorted elset can be used if necessary).
  • The ECS of the beam elements must be the same (the spline must be linear).
  • The coordinates of the spline are defined in the ECS, with the starting point of the first beam element as the origin.
  • The x-coordinate of the spline must monotonically increase according to the beam element's axial direction.

If the parent elset is not a beam element group, the spline is defined in the GCS and has no additional constraints.

▪ Notes

  • The Tendon element does not calculate the mass matrix (contributes only to stiffness).
Example
*Material, Type=IsoElasticity Name=tendon  
 E=200E9

*Construction, Type=Spline, Name=curve
 0.,  0., 0.
 15, -0.8 0.
 30., 0., 0.

*Section, Type=Tendon, Name=tendon
  tendon, 0.01, curve, 0.4, 0.2, Lobatto,4  # area, spline, mu, kappa, Lobatto|Legendre, ngauss

*Section, Type=Tendon, Name=tendon
  tendon, 0.01, curve, 0.4, 0.2, Lobatto,4  # area, spline, mu, kappa, Lobatto|Legendre, ngauss

*Element, Type=Tendon, ELSet=tendon
 1001, 1, S=tendon, Host=conc

*Step, Type=STATIC, Name=1
...

*Field, Type=TendonStress
 1001, 200E6, Left

*Element, Type=Tendon

Define Tendon element

*Element, Type=Tendon, ELSet=elset
  id, n1{, S=sec, H=hostElset }
First dataline and subsequent lines
  • H=hostElset: Section name. Section names must be unique.
Specifications
  • No. of nodes: 1
  • Fields: Uniaxial model response at the element center.
  • Compatible section: Tendon
  • Active DOFs: None

▪ Notes The n1 node is used only as a reference point for defining the geometry and does not contribute to the stiffness or mass matrix of the element.

*Section, Type=Tendon

Define the properties for Tendon element

*Section, Type=Tendon, Name=name
  material, area, spline, mu, kappa, {Lobatto|Legendre}, ngauss
Keyword line
  • Name=name: Section name. Section names must be unique.
First dataline
  • material: Material (required).
  • area: Area (required).
  • spline: Spline (required).
  • mu, kappa: Curvature and wobble friction coefficients (optional, default 0., 0.).
  • {Lobatto|Legendre|NewtonCotes}, ngauss: Integration method and number of integration points (optional, default is Lobatto, 4).