<!-- source-page: 271 -->

# 29.2 Truss elements

• “Truss elements,” Section 29.2.1   
• “Truss element library,” Section 29.2.2

<!-- source-page: 272 -->

<!-- source-page: 273 -->

# 29.2.1 TRUSS ELEMENTS

Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE

# References

• “Truss element library,” Section 29.2.2   
• \*SOLID SECTION   
• “Creating truss sections,” Section 12.13.12 of the Abaqus/CAE User’s Guide, in the HTML version of this guide

# Overview

Truss elements:

• are long, slender structural members that can transmit only axial force (nonstructural link elements are presented in “One-dimensional solid (link) element library,” Section 28.1.2); and   
• do not transmit moments.

# Typical applications

Truss elements are used in two and three dimensions to model slender, line-like structures that support loading only along the axis or the centerline of the element. No moments or forces perpendicular to the centerline are supported.

The two-dimensional truss elements can be used in axisymmetric models to represent components, such as bolts or connectors, where the strain is computed from the change in length in the r–z plane only. Two-dimensional trusses can also be used to define master surfaces for contact applications in Abaqus/Standard (see “Contact interaction analysis: overview,” Section 36.1.1). In this case the direction of the master surface’s outward normal is critical for proper detection of contact.

The 3-node truss element available in Abaqus/Standard is often useful for modeling curved reinforcing cables in structures, such as prestressed tendons in reinforced concrete or long slender pipelines used in the off-shore industry.

# Choosing an appropriate element

A 2-node straight truss element, which uses linear interpolation for position and displacement and has a constant stress, is available in both Abaqus/Standard and Abaqus/Explicit. In addition, a 3-node curved truss element, which uses quadratic interpolation for position and displacement so that the strain varies linearly along the element, is available in Abaqus/Standard.

Hybrid versions of the stress/displacement trusses, coupled temperature-displacement trusses, and piezoelectric trusses are available in Abaqus/Standard.

<!-- source-page: 274 -->

# Hybrid stress/displacement truss elements

Hybrid (mixed) versions of the stress/displacement trusses, in which the axial force is treated as an additional unknown, are available in two and three dimensions in Abaqus/Standard. These elements are useful (to offset the effects of numerical ill-conditioning on governing equations) when a truss represents a very rigid link whose stiffness is much larger than that of the overall structural model. In such a case a hybrid truss provides an alternative to a truly rigid link, modeled with multi-point constraints (see “General multi-point constraints,” Section 35.2.2) or rigid elements (see “Rigid elements,” Section 30.3.1).

# Coupled temperature-displacement truss elements

Coupled temperature-displacement truss elements are available in two and three dimensions in Abaqus/Standard. These elements have temperature as an additional degree of freedom (11). See “Fully coupled thermal-stress analysis,” Section 6.5.3, for information about fully coupled temperature-displacement analysis in Abaqus/Standard.

# Piezoelectric truss elements

Piezoelectric truss elements are available in two and three dimensions in Abaqus/Standard. These elements have electric potential as an additional degree of freedom (9). See “Piezoelectric analysis,” Section 6.7.2, for information about piezoelectric analysis.

# Naming convention

Truss elements in Abaqus are named as follows:

![](images/page-274_4ef18130bb6c2419d215ffe10528ded86084421425488fc8f1367a789d5f4c9f.jpg)

<details>
<summary>text_image</summary>

T 3D 2 H
truss
Optional: hybrid (H), coupled temperature-displacement (T), or piezoelectric (E)
number of nodes
two-dimensional (2D) or three-dimensional (3D)
</details>

For example, T2D3E is a two-dimensional, 3-node piezoelectric truss element.

# Element normal definition

For two-dimensional trusses the positive outward normal, , is defined by a $9 0 ^ { \circ }$ counterclockwise rotation from the direction going from node 1 to node 2 or node 3 of the element, as shown.

<!-- source-page: 275 -->

![](images/page-275_9604fa140a6f044703c8c9b5fab859731645797af8209745c4ab031acd086f9c.jpg)

<details>
<summary>text_image</summary>

n
1
2
</details>

![](images/page-275_58baa5859bc0d3870c3912a61fbc947de50935a6a3e1166609ee7861f47637e0.jpg)

<details>
<summary>text_image</summary>

n
1
2
3
</details>

# Defining the element’s section properties

You use a solid section definition to define the section properties. You must associate these properties with a region of your model.

Input File Usage: \*SOLID SECTION, ELSET=name

where the ELSET parameter refers to a set of truss elements.

Abaqus/CAE Usage: Property module:

Create Section: select Beam as the section Category and Truss as the section Type

Assign→Section: select regions

# Defining the cross-sectional area of a truss element

You can define the cross-sectional area associated with the truss element as part of the section definition. If you do not specify a value for the cross-sectional area, unit area is assumed.

When truss elements are used in large-displacement analysis, the updated cross-sectional area is calculated by assuming that the truss is made of an incompressible material, regardless of the actual material definition. This assumption affects cases only where the strains are large. It is adopted because the most common applications of trusses at large strains involve yielding metal behavior or rubber elasticity, in which cases the material is effectively incompressible. Therefore, a linear elastic truss element does not provide the same force-displacement response as a linear SPRINGA spring element when the axial strain is not infinitesimal.

Input File Usage: \*SOLID SECTION, ELSET=name

cross-sectional area

Abaqus/CAE Usage: Property module: Create Section: select Beam as the section Category and

Truss as the section Type: Cross-sectional area: cross-sectional area

# Assigning a material definition to a set of truss elements

You must associate a material definition with each solid section definition. No material orientation is permitted with truss elements.

<!-- source-page: 276 -->

<table><tr><td rowspan="2">Input File Usage:</td><td>*SOLID SECTION, MATERIAL=name</td></tr><tr><td>Any value given to the ORIENTATION parameter on the *SOLID SECTION option will be ignored by truss elements.</td></tr><tr><td>Abaqus/CAE Usage:</td><td>Property module: Create Section: select Beam as the section Category and Truss as the section Type: Material: name</td></tr></table>

# Using truss elements in large-displacement implicit analysis

Truss elements have no initial stiffness to resist loading perpendicular to their axis. If a stress-free line of trusses is loaded perpendicular to its axis in Abaqus/Standard, numerical singularities and lack of convergence can result. After the first iteration in a large-displacement implicit analysis, stiffness perpendicular to the initial line of the elements develops, sometimes allowing an analysis to overcome numerical problems.

In some cases loading the truss elements along their axis first or including initial tensile stress can overcome these numerical singularities. However, you must choose the magnitude of the loading or initial stress such that the final solution is unaffected.

<!-- source-page: 277 -->

# 29.2.2 TRUSS ELEMENT LIBRARY

Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE

# References

• “Truss elements,” Section 29.2.1   
• \*SOLID SECTION

# Overview

This section provides a reference to the truss elements available in Abaqus/Standard and Abaqus/Explicit.

# Element types

# 2D stress/displacement truss elements

T2D2 2-node linear displacement

T2D2H(S) 2-node linear displacement, hybrid

T2D3(S) 3-node quadratic displacement

T2D3H(S) 3-node quadratic displacement, hybrid

Active degrees of freedom

1, 2

Additional solution variables

Element type T2D2H has one additional variable and element type T2D3H has two additional variables relating to axial force.

# 3D stress/displacement truss elements

T3D2 2-node linear displacement

T3D2H(S) 2-node linear displacement, hybrid

T3D3(S) 3-node quadratic displacement

T3D3H(S) 3-node quadratic displacement, hybrid

Active degrees of freedom

1, 2, 3

Additional solution variables

Element type T3D2H has one additional variable and element type T3D3H has two additional variables relating to axial force.

<!-- source-page: 278 -->

# 2D coupled temperature-displacement truss elements

<table><tr><td>T2D2T(S)</td><td>2-node, linear displacement, linear temperature</td></tr><tr><td>T2D3T(S)</td><td>3-node, quadratic displacement, linear temperature</td></tr></table>

Active degrees of freedom

1, 2 at middle node for T2D3T   
1, 2, 11 at all other nodes

Additional solution variables

None.

# 3D coupled temperature-displacement truss elements

<table><tr><td>T3D2T(S)</td><td>2-node, linear displacement, linear temperature</td></tr><tr><td>T3D3T(S)</td><td>3-node, quadratic displacement, linear temperature</td></tr></table>

Active degrees of freedom

1, 2, 3 at middle node for T3D3T   
1, 2, 3, 11 at all other nodes

Additional solution variables

None.

# 2D piezoelectric truss elements

<table><tr><td>T2D2E(S)</td><td>2-node, linear displacement, linear electric potential</td></tr><tr><td>T2D3E(S)</td><td>3-node, quadratic displacement, quadratic electric potential</td></tr></table>

Active degrees of freedom

1, 2, 9

Additional solution variables

None.

# 3D piezoelectric truss elements

<table><tr><td>T3D2E(S)</td><td>2-node, linear displacement, linear electric potential</td></tr><tr><td>T3D3E(S)</td><td>3-node, quadratic displacement, quadratic electric potential</td></tr></table>

Active degrees of freedom

1, 2, 3, 9

Additional solution variables

None.

<!-- source-page: 279 -->

Nodal coordinates required

2D: X, Y   
3D: X, Y, Z

Element property definition

You must provide the cross-sectional area of the element. If no area is given, Abaqus assumes unit area.

Input File Usage: \*SOLID SECTION

Abaqus/CAE Usage: Property module: Create Section: select Beam as the section Category and Truss as the section Type

Element-based loading

Distributed loads

Distributed loads are available for elements with displacement degrees of freedom. They are specified as described in “Distributed loads,” Section 34.4.3.

<table><tr><td>Load ID (*DLOAD)</td><td>Abaqus/CAE Load/Interaction</td><td>Units</td><td>Description</td></tr><tr><td>BX</td><td>Body force</td><td> $FL^{-3}$ </td><td>Body force in global X-direction.</td></tr><tr><td>BY</td><td>Body force</td><td> $FL^{-3}$ </td><td>Body force in global Y-direction.</td></tr><tr><td>BZ</td><td>Body force</td><td> $FL^{-3}$ </td><td>Body force in global Z-direction. (Only for 3D trusses.)</td></tr><tr><td>BXNU</td><td>Body force</td><td> $FL^{-3}$ </td><td>Nonuniform body force in global X-direction with magnitude supplied via user subroutine DLOAD in Abaqus/Standard and VDLOAD in Abaqus/Explicit.</td></tr><tr><td>BYNU</td><td>Body force</td><td> $FL^{-3}$ </td><td>Nonuniform body force in global Y-direction with magnitude supplied via user subroutine DLOAD in Abaqus/Standard and VDLOAD in Abaqus/Explicit.</td></tr><tr><td>BZNU</td><td>Body force</td><td> $FL^{-3}$ </td><td>Nonuniform body force in global Z-direction with magnitude supplied via user subroutine DLOAD in Abaqus/Standard and VDLOAD</td></tr></table>

<!-- source-page: 280 -->

<table><tr><td>Load ID (*DLOAD)</td><td>Abaqus/CAE Load/Interaction</td><td>Units</td><td>Description</td></tr><tr><td></td><td></td><td></td><td>in Abaqus/Explicit. (Only for 3D trusses.)</td></tr><tr><td> $CENT^{(S)}$ </td><td>Not supported</td><td> $FL^{-4}$  $(ML^{-3}T^{-2})$ </td><td>Centrifugal load (magnitude is input as  $\rho\omega^{2}$ , where  $\rho$  is the mass density per unit volume,  $\omega$  is the angular velocity).</td></tr><tr><td> $CENTRIF^{(S)}$ </td><td>Rotational body force</td><td> $T^{-2}$ </td><td>Centrifugal load (magnitude is input as  $\omega^{2}$ , where  $\omega$  is the angular velocity).</td></tr><tr><td> $CORIO^{(S)}$ </td><td>Coriolis force</td><td> $FL^{-4}T$  $(ML^{-3}T^{-1})$ </td><td>Coriolis force (magnitude is input as  $\rho\omega$ , where  $\rho$  is the mass density per unit volume,  $\omega$  is the angular velocity).</td></tr><tr><td>GRAV</td><td>Gravity</td><td> $LT^{-2}$ </td><td>Gravity loading in a specified direction (magnitude is input as acceleration).</td></tr><tr><td> $ROTA^{(S)}$ </td><td>Rotational body force</td><td> $T^{-2}$ </td><td>Rotary acceleration load (magnitude is input as  $\alpha$ , where  $\alpha$  is the rotary acceleration).</td></tr></table>

# Abaqus/Aqua loads

Abaqus/Aqua loads are specified as described in “Abaqus/Aqua analysis,” Section 6.11.1. They are available only for stress/displacement trusses.

<table><tr><td>Load ID(*CLOAD/*DLOAD)</td><td>Abaqus/CAELoad/Interaction</td><td>Units</td><td>Description</td></tr><tr><td> $FDD^{(A)}$ </td><td>Not supported</td><td> $FL^{-1}$ </td><td>Transverse fluid drag load.</td></tr><tr><td> $FD1^{(A)}$ </td><td>Not supported</td><td>F</td><td>Fluid drag force on the first end of the truss (node 1).</td></tr><tr><td> $FD2^{(A)}$ </td><td>Not supported</td><td>F</td><td>Fluid drag force on the second end of the truss (node 2 or node 3).</td></tr><tr><td> $FDT^{(A)}$ </td><td>Not supported</td><td> $FL^{-1}$ </td><td>Tangential fluid drag load.</td></tr><tr><td> $FI^{(A)}$ </td><td>Not supported</td><td> $FL^{-1}$ </td><td>Fluid inertia load.</td></tr></table>
