mkb02-link1.pdf

LINK1

Strona 1 z 5

Main TOC • Using Help • Copyright

Element Reference > Part I. Element Library >LINK1

LINK1 Ï 2-D Spar (or Truss)

MP ME ST PR PP ED

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 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 the ANSYS,

Inc. Theory Reference for more details about this element. See LINK8 for a description of a three-

dimensional spar element.

Figure 1.1. LINK1 2-D Spar

Input Data

LINK1 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 ∆/L, where ∆ 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.

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

mk:@MSITStore:C:\Moje%20dokumenty\MKB\Ansys\ansyshelp.chm::/Hlp_E_LINK1.html

06.11.02

LINK1

Strona 2 z 5

input.

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

Output Data

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 LINK1 Element Output Definitions .

Stress output illustrates several items. A general description of solution output is given in Solution

Output . See the ANSYS Basic Analysis Guide for ways to view results.

Figure 1.2. LINK1 Stress Output

mk:@MSITStore:C:\Moje%20dokumenty\MKB\Ansys\ansyshelp.chm::/Hlp_E_LINK1.html

06.11.02

LINK1

Strona 3 z 5

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

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

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 ANSYS Basic Analysis Guide

and The Item and Sequence Number Table for further information. The table uses the following notation:

Name

output quantity as defined in the Element Output Definitions table.

Item

predetermined Item label for ETABLE command

mk:@MSITStore:C:\Moje%20dokumenty\MKB\Ansys\ansyshelp.chm::/Hlp_E_LINK1.html

06.11.02

LINK1

Strona 4 z 5

sequence number for single-valued or constant element data

I,J

sequence number for data at nodes I and J

Table 1.2. 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

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.

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.

mk:@MSITStore:C:\Moje%20dokumenty\MKB\Ansys\ansyshelp.chm::/Hlp_E_LINK1.html

06.11.02

LINK1

Strona 5 z 5

Chapter 4. Element Library

Home

PLANE2

mk:@MSITStore:C:\Moje%20dokumenty\MKB\Ansys\ansyshelp.chm::/Hlp_E_LINK1.html

06.11.02

Plik z chomika:

Inne pliki z tego folderu:

Inne foldery tego chomika: