# Truss Elements

What is a Truss Element?

Truss elements are two-node members which allow arbitrary orientation in the XYZ coordinate system. The truss transmits axial force only and, in general, is a three degree-of-freedom (DOF) element (i.e., three global translation components at each end of the member). Trusses are used to model structures such as towers, bridges and buildings.

The three-dimensional (3-D) truss element is assumed to have a constant cross-sectional area and can be used in linear elastic analysis.  Linear elastic material behavior is defined only by the modulus of elasticity.  Linear trusses can also be used to simulate translational and displacement boundary elements.

Trusses, by definition, cannot have rotational DOFs, even if you released these DOFs when you applied the boundary conditions.  You can apply translational DOFs as needed.

Figure 1: Formulation of a Truss Element

When to Use Truss Elements

The basic guidelines for when to use a truss element are:

• The length of the element is much greater than the width or depth (approx 8-10 times).

• It is connected to the rest of the model with hinges that do not transfer moments.

• The external applied forces are only at joints.

Truss Element Parameters

When using spring elements, specify the axial cross-sectional area of the truss elements in this part in the "Cross-Sectional Area" field in the "Element Definition" dialog. This value must be greater than zero and is required for an analysis.

If you are performing a thermal stress analysis on this part, specify the temperature at which the elements in this part will experience no thermally induced stresses in the "Stress Free Reference Temperature" field.  Element based loads associated with constraint of thermal growth are calculated using the average of the temperatures specified on the nodal point data lines. The reference temperature is used to calculate the temperature change. Thermal loading may be used to achieve other types of member loadings. For these cases, an equivalent temperature change (dT) is used.

Basic Steps for Using Truss Elements

• Be sure that a unit system is defined.

• Be sure that the model is using a structural analysis type.

• Right click on the "Element Type" heading for the part that you want to be truss elements.

• Select the "Truss" command.

• Right click on the "Element Definition" heading for the part that you want to be truss elements.

• Select the "Modify Element Definition..." command.

• In the "Element Definition" dialog, type a value in the "Cross Sectional Area" field.

• If you are running a thermal stress analysis, type a value in the "Stress Free Reference Temperature" field. This is the temperature at which no stresses are present in the model. The difference between this temperature and the nodal temperatures will create the stress.

• Press the "OK" button.

Using Truss Elements to Model an Initial Lack of Fit

The following equations may be used to calculate the equivalent temperature change associated with an initial lack of fit of a truss member between two points.  A positive value would mean that the element is initially too short.

where:

where:

Tavg = the average of the nodal temperatures of the two nodes of the truss element.

Tsf = the stress free reference temperature of the part.

D = the desired elongation or shrinkage of the truss element.

a = the thermal coefficient of expansion of the part.

L = the unloaded length of the truss element.

Using Truss Elements to Model an Initial Prestress

The following equations may be used to calculate the equivalent temperature change associated with an initial prestress used to deform a truss member to fit between two points:

where:

where:

Tavg = the average of the nodal temperatures of the two nodes of the truss element.

Tsf - the stress free reference temperature of the part.

P = the axial force in the truss element.

E = the modulus of elasticity of the truss element.

A = the cross-sectional area of the truss element.

a = the thermal coefficient of expansion of the part.

Note that the force P is the initial force in the truss element when the rest of the structure has no force. If the rest of the structure were infinitely stiff, then the result of the analysis would be an axial force of P in the heated truss element. Since the structure is usually not infinitely stiff, one result of the preload is that the structure deforms and relieves a portion of the thermal preload. See the page "Setting Up and Performing the Analysis: Linear: Loads and Constraints: Beam Preload" for a methodology if the load P is the final desired load in the truss after the structure deforms due to the preload.