Skip to content

EmbeddedLine

The EmbeddedLine element is used to model embedded tendons or reinforcing bars, and is defined through the EmbeddedLine element type and the EmbeddedLine section type. When defining an EmbeddedLine section, the element profile is specified by a spline geometry. For each element, a host element set must be assigned. The applicable host element families are as follows:

  • 2D Beam elements: B2D2H, B2D2MH
  • 3D Beam elements: B3D2H, B3D2MH
  • Shell elements: S3F, S4F, S3, S4
  • Solid-shell elements: CS6, CS8
  • 2D Solid elements: CPE4, CPS4, CAX4, CPS3, CPE3, CAX3
  • 3D Solid elements: C3D8, C3D8I, C3D6

The host element set assigned to an EmbeddedLine element must consist of elements from the same family. For tendon analysis, prestressing loads can be applied using the *State command.

▪ Note

  • The EmbeddedLine element does not compute a mass matrix (it contributes only to stiffness).
  • Reinforcement modeling can alternatively be performed using truss elements(T3D2) combined with Embedded constraints. In this case, only straight bars can be represented and prestressing cannot be applied.
  • The EmbeddedLine element uses a single node, but only as a reference point for the spline geometry. No degrees of freedom are defined at that node.

Fig. 4.11-1 EmbeddedLine element

Fig. 4.11-1. EmbeddedLine element

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=EmbeddedLine, Name=tendon
  tendon, 0.01
  0.4, 0.2

*Element, Type=EmbeddedLine, ELSet=tendon
 1001, 1, S=tendon, L=curve, H=conc

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

*State, Type=TendonForce
 1001, 200E6, Left

*Element, Type=EmbeddedLine

Define EmbeddedLine element

*Element, Type=EmbeddedLine, ELSet=elset
  id, n1, S=sec, L=spline, H=hostElset
First data line and subsequent lines
  • L=spline: Spline defining the profile
  • H=hostElset: Host elset
Specifications
  • No. of nodes: 1
  • Fields: ED=[ED.X ED.Y ED.Z] and uniaxial material field at Gauss point
  • Compatible section: EmbeddedLine
  • 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.
  • The number of integration points depends on the integration scheme specified in the cross-section (Aligned or Unaligned).

*Section, Type=EmbeddedLine

Define the properties for EmbeddedLine element

*Section, Type=EmbeddedLine, Name=name
  material, area, { Aligned, ngauss | Unaligned, nsegment }
  mu, kappa
Keyword line
  • Name=name: Section name. Section names must be unique.
First data line
  • material: material (required)
  • area: area (required)
  • Aigned, ngauss: The spline is divided according to the host element for integration, and the Legendre integration with ngauss points is applied to each segment. (optional, default: Aligned, 3)
  • Unaligned, nsegment: The spline is divided into nsegment parts, and the Trapezoidal rule is applied for integration. In this mode, the subdivision does not match the host element mesh. If nsegment is not specified, it is determined automatically as twice the number of elements that the spline passes through. (optional) Total number of integration points are nsegment + 1.
Second data line (optional)
  • mu, kappa: Curvature and wobble friction coefficients (optional, default 0., 0.).

The curvature friction coefficient has a unit of 1/rad, and the wobble friction coefficient has a unit of 1/length. Their typical ranges are 0.15–0.3 /rad and 0.00021–0.007 /m, respectively.

Example
*SECTION, TYPE=EmbeddedLine, Name=case1
  steel,  0.1

*SECTION, TYPE=EmbeddedLine, Name=case2
  steel,  0.1, Aligned, 4

*SECTION, TYPE=EmbeddedLine, Name=case3
  steel,  0.1, Unaligned

*SECTION, TYPE=EmbeddedLine, Name=case4
  steel,  0.1, Unaligned, 10

*SECTION, TYPE=EmbeddedLine, Name=case5
  steel,  0.1
  0.4, 0.2