4.1 LINK1 2-D Spar

4.1 LINK1 2-D Spar (UP19980821 )

You can use LINK1 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 two-dimensional 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 Section 14.1 of the ANSYS Theory Reference for more details about this element. See Section 4.8 for a description of a three-dimensional spar element, LINK8.

Figure 4.1-1 LINK1 2-D Spar



4.1.1 Input Data

Figure 4.1-1 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. Properties that you do not input default as described in Section 2.4. The initial strain in the element (ISTRN) is given by /L, where is the difference between the element length, L, (as defined by the I and J node locations) and the zero-strain length.

Section 2.7 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.

Table 4.1-1 summarizes the element input. Section 2.1 gives a general description of element input.

Table 4.1-1 LINK1 Input Summary

Element Name

LINK1

Nodes

I, J

Degrees of Freedom

UX, UY

Real Constants

AREA, ISTRN

Material Properties

EX, ALPX, DENS, DAMP

Surface Loads

None

Body Loads

Temperatures: T (I), T (J)
Fluences: FL (I), FL (J)

Special Features

Plasticity, Creep, Swelling, Stress stiffening, Large deflection,
Birth and death

4.1.2 Output Data

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

Figure 4.1-2 illustrates several items. A general description of solution output is given in Section 2.2. See the ANSYS Basic Analysis Procedures Guide for ways to view results.

Figure 4.1-2 LINK1 Stress Output



Table 4.1-2 uses the following notation:

A colon (:) in the Name column indicates the item can be accessed by the Component Name method [ETABLE, ESOL] (see Section 2.2.2). The O and R columns indicate the availability of the items in the file Jobname.OUT (O) or in the results file (R), a Y indicates that the item is always available, a number refers to a table footnote which describes when the item is conditionally available, and a - indicates that the item is not available.

Table 4.1-2 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

CENT: X, Y

Center location of the element XC, YC

-

Y

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

1. Only if the element has a nonlinear material

Table 4.1-3 lists output available through the ETABLE command using the Sequence Number method. See Chapter 5 of the ANSYS Basic Analysis Procedures Guide and Section 2.2.2.2 for further information. Table 4.1-3 uses the following notation:

Table 4.1-3 LINK1 Item and Sequence Numbers for the ETABLE and ESOL Commands

Name

Item

E

I

J

SAXL

LS

1 - -
EPELAXL

LEPEL

1 - -
EPTHAXL

LEPTH

1 - -
EPSWAXL

LEPTH

2 - -
EPINAXL

LEPTH

3 - -
EPPLAXL

LEPPL

1 - -
EPCRAXL

LEPCR

1 - -
SEPL

NLIN

1 - -
SRAT

NLIN

2 - -
HPRES

NLIN

3 - -
EPEQ

NLIN

4 - -
MFORX

SMISC

1 - -
FLUEN

NMISC

- 1 2
TEMP

LBFE

- 1 2

4.1.3 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 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.

4.1.4 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/LinearPlus