Release 11.0 Documentation for ANSYS
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.
I, J
UX, UY
| AREA - Cross-sectional area |
| ISTRN - Initial strain |
EX, ALPX (or CTEX or THSX), DENS, DAMP
None
T(I), T(J)
FL(I), FL(J)
| Plasticity (BISO, MISO, BKIN, MKIN, KINH, DP, ANISO) |
| 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.
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 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
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.
