www.kxcad.net Home > CAE Index > ANSYS Index > Release 11.0 Documentation for ANSYS


2-D Spar (or Truss)

MP ME ST PR PRN DS DSS <> <> <> <> PP <>

Product Restrictions

LINK1 Element Description

LINK1 can be used in a variety of engineering applications. Depending upon the application, you can think of the element as a truss, a link, a spring, etc. The 2-D spar element is a uniaxial tension-compression element with two degrees of freedom at each node: translations in the nodal x and y directions. As in a pin-jointed structure, no bending of the element is considered. See LINK1 in the Theory Reference for ANSYS and ANSYS Workbench for more details about this element. See LINK8 for a description of a 3-D spar element.

Figure 1.1  LINK1 Geometry

LINK1 Input Data

Figure 1.1: "LINK1 Geometry" shows the geometry, node locations, and the coordinate system for this element. The element is defined by two nodes, the cross-sectional area, an initial strain, and the material properties. The element x-axis is oriented along the length of the element from node I toward node J. The initial strain in the element (ISTRN) is given by Δ/L, where Δ is the difference between the element length, L, (as defined by the I and J node locations) and the zero-strain length.

Node and Element Loads describes element loads. You can input temperatures and fluences as element body loads at the nodes. The node I temperature T(I) defaults to TUNIF. The node J temperature defaults to T(I). Similar defaults occur for fluence except that zero is used instead of TUNIF. You can request a lumped mass matrix formulation, which may be useful for certain analyses such as wave propagation, with the LUMPM command.

"LINK1 Input Summary" summarizes the element input. Element Input gives a general description of element input.

LINK1 Input Summary


I, J

Degrees of Freedom


Real Constants
AREA - Cross-sectional area
ISTRN - Initial strain
Material Properties


Surface Loads


Body Loads
Temperatures -- 

T(I), T(J)

Fluences -- 

FL(I), FL(J)

Special Features
Creep (CREEP)
Swelling (SWELL)
Elasticity (MELAS)
Other material (USER)
Stress stiffening
Large deflection
Birth and death


Items in parentheses refer to data tables associated with the TB command.



LINK1 Output Data

The solution output associated with the element is in two forms:

Figure 1.2: "LINK1 Stress Output" illustrates several items. A general description of solution output is given in Solution Output. See the Basic Analysis Guide for ways to view results.

Figure 1.2  LINK1 Stress Output

The Element Output Definitions table uses the following notation:

A colon (:) in the Name column indicates the item can be accessed by the Component Name method [ETABLE, ESOL]. The O column indicates the availability of the items in the file Jobname.OUT. The R column indicates the availability of the items in the results file.

In either the O or R columns, Y indicates that the item is always available, a number refers to a table footnote that describes when the item is conditionally available, and a - indicates that the item is not available.

Table 1.1  LINK1 Element Output Definitions

ELElement NumberYY
NODESElement node numbers (I and J)YY
MATMaterial number for the elementYY
VOLU:Element volume-Y
XC, YCLocation where results are reportedY2
TEMPTemperature at nodes I and JYY
FLUENFluence at nodes I and JYY
MFORXMember force in the element coordinate system X directionYY
SAXLAxial stress in the elementYY
EPELAXLAxial elastic strain in the elementYY
EPTHAXLAxial thermal strain in the elementYY
EPINAXLAxial initial strain in the elementYY
SEPLEquivalent stress from the stress-strain curve11
SRATRatio of trial stress to the stress on yield surface11
EPEQEquivalent plastic strain11
HPRESHydrostatic pressure11
EPPLAXLAxial plastic strain11
EPCRAXLAxial creep strain11
EPSWAXLAxial swelling strain11
  1. Only if the element has a nonlinear material

  2. Available only at centroid as a *GET item.

The Item and Sequence Number... table lists output available through the ETABLE command using the Sequence Number method. See The General Postprocessor (POST1) in the Basic Analysis Guide and The Item and Sequence Number Table for further information. The table uses the following notation:

Output Quantity Name

output quantity as defined in the Element Output Definitions table.


predetermined Item label for ETABLE command


sequence number for single-valued or constant element data


sequence number for data at nodes I and J

Table 1.2  LINK1 Item and Sequence Numbers

Output Quantity NameETABLE and ESOL Command Input

LINK1 Assumptions and Restrictions

  • The spar element assumes a straight bar, axially loaded at its ends, of uniform properties from end to end.

  • The length of the spar must be greater than zero, so nodes I and J must not be coincident.

  • The spar must lie in an X-Y plane and must have an area greater than zero.

  • The temperature is assumed to vary linearly along the length of the spar.

  • The displacement shape function implies a uniform stress in the spar.

  • The initial strain is also used in calculating the stress stiffness matrix, if any, for the first cumulative iteration.

LINK1 Product Restrictions

When used in the product(s) listed below, the stated product-specific restrictions apply to this element in addition to the general assumptions and restrictions given in the previous section.

ANSYS Professional. 

  • The DAMP material property is not allowed.

  • Fluence body loads cannot be applied.

  • The only special features allowed are stress stiffening and large deflections.