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

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" 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.

**Nodes**I, J

**Degrees of Freedom**UX, UY

**Real Constants**AREA - Cross-sectional area ISTRN - Initial strain **Material Properties**EX, ALPX (or CTEX

*or*THSX), DENS, DAMP**Surface Loads**None

**Body Loads****Temperatures --**T(I), T(J)

**Fluences --**FL(I), FL(J)

**Special Features**Plasticity (BISO, MISO, BKIN, MKIN, KINH, DP, ANISO) Creep (CREEP) Swelling (SWELL) Elasticity (MELAS) Other material (USER) Stress stiffening Large deflection Birth and death ### Note

Items in parentheses refer to data tables associated with the

**TB**command.**KEYOPTS**None

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

Nodal displacements included in the overall nodal solution

Additional element output as shown in Table 1.1: "LINK1 Element Output Definitions".

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.

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**

Name | Definition | O | R |
---|---|---|---|

EL | Element Number | Y | Y |

NODES | Element node numbers (I and J) | Y | Y |

MAT | Material number for the element | Y | Y |

VOLU: | Element volume | - | Y |

XC, YC | Location where results are reported | Y | 2 |

TEMP | Temperature at nodes I and J | Y | Y |

FLUEN | Fluence at nodes I and J | Y | Y |

MFORX | Member force in the element coordinate system X direction | Y | Y |

SAXL | Axial stress in the element | Y | Y |

EPELAXL | Axial elastic strain in the element | Y | Y |

EPTHAXL | Axial thermal strain in the element | Y | Y |

EPINAXL | Axial initial strain in the element | Y | Y |

SEPL | Equivalent stress from the stress-strain curve | 1 | 1 |

SRAT | Ratio of trial stress to the stress on yield surface | 1 | 1 |

EPEQ | Equivalent plastic strain | 1 | 1 |

HPRES | Hydrostatic pressure | 1 | 1 |

EPPLAXL | Axial plastic strain | 1 | 1 |

EPCRAXL | Axial creep strain | 1 | 1 |

EPSWAXL | Axial swelling strain | 1 | 1 |

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.

**Item**predetermined Item label for

**ETABLE**command**E**sequence number for single-valued or constant element data

**I,J**sequence number for data at nodes I and J

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.

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.