3-D Spar (or Truss)

Compatible Products: – | Pro | Premium | Enterprise | Ent PP | Ent Solver | –

LINK180 Element Description

LINK180 is a 3-D spar that is useful in a variety of engineering applications. The element can be used to model trusses, sagging cables, links, springs, and so on. The element is a uniaxial tension-compression element with three degrees of freedom at each node: translations in the nodal x, y, and z directions. Tension-only (cable) and compression-only (gap) options are supported. As in a pin-jointed structure, no bending of the element is considered. Plasticity, creep, rotation, large deflection, and large strain capabilities are included.

By default, LINK180 includes stress-stiffness terms in any analysis that includes large-deflection effects. Elasticity, isotropic hardening plasticity, kinematic hardening plasticity, Hill anisotropic plasticity, Chaboche nonlinear hardening plasticity, and creep are supported. To simulate the tension-/compression-only options, a nonlinear iterative solution approach is necessary. Added mass, hydrodynamic added mass and loading, and buoyant loading are available.

See LINK180 for more information about this element.

Figure 180.1:  LINK180 Geometry

LINK180 Geometry

LINK180 Input Data

The geometry, node locations, and the coordinate system for this element are shown in Figure 180.1: LINK180 Geometry. The element is defined by two nodes, the cross-sectional area (A) input via the SECTYPE and SECDATA commands, added mass per unit length (ADDMAS) input via the SECCONTROL command, and the material properties.

The element x-axis is oriented along the length of the element from node I toward node J. If ocean loading is present, the global origin is normally at the mean sea level, with the global Z-axis pointing away from the center of the earth; however, the vertical location can be adjusted via Zmsl (Val6) on the OCDATA command (following the OCTYPE,BASIC command).

Element loads are described in Nodal Loading. Temperatures may be input as element body loads at the nodes. The node I temperature T(I) defaults to TUNIF. The node J temperature T(J) defaults to T(I).

LINK180 allows a change in cross-sectional area as a function of axial elongation. By default, the cross-sectional area changes such that the volume of the element is preserved, even after deformation. The default is suitable for elastoplastic applications. By using KEYOPT(2), you may choose to keep the cross section constant or rigid.

LINK180 offers compression-and-tension, tension-only, and compression-only options. Specify the desired behavior via the SECCONTROL command.

For ocean loading, hydrodynamic added mass and loading, and buoyant loading, are available via the OCDATA and OCTABLE commands.

When ocean loading is applied, the loading is nonlinear (that is, based on the square of the relative velocity between the structure and the water). Accordingly, the full Newton-Raphson option (NROPT,FULL) may be necessary to achieve optimal results. (Full Newton-Raphson is applied automatically in an analysis involving large-deflection effects [NLGEOM,ON].)

You can apply an initial stress state to this element via the INISTATE command. For more information, see Initial State in the Mechanical APDL Advanced Analysis Guide.

The "LINK180 Input Summary" table summarizes the element input. Element Input gives a general description of element input.

LINK180 Input Summary


I, J

Degrees of Freedom


Material Properties

TB command: See Element Support for Material Models for this element.


Surface Loads


Body Loads
Temperatures -- 

T(I), T(J)

Special Features
Birth and death
Initial state
Large deflection
Large strain
Linear perturbation
Nonlinear stabilization
Ocean loading
Stress stiffening

Cross-section scaling (applies only when large-deflection effects [NLGEOM,ON] are specified):

0 -- 

Enforce incompressibility; cross section is scaled as a function of axial stretch (default).

1 -- 

Section is assumed to be rigid.


Hydrodynamic output (not available in harmonic analyses that include ocean wave effects (HROCEAN)):

0 -- 

None (default)

1 -- 

Additional hydrodynamic printout

LINK180 Output Data

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

Several items are illustrated in Figure 180.2: LINK180 Stress Output. A general description of solution output is given in Solution Output. Element results can be viewed in POST1 via PRESOL,ELEM.

Figure 180.2:  LINK180 Stress Output

LINK180 Stress Output

The Element Output Definitions table uses the following notation:

A colon (:) in the Name column indicates that 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 “-” indicates that the item is not available.

Table 180.1:  LINK180 Element Output Definitions

ELElement numberYY
MATMaterial numberYY
SECIDSection numberY-
XC, YC, ZCCenter locationY1
TEMPTemperatures T(I), T(J)YY
AREACross-sectional areaYY
FORCEMember force in the element coordinate systemYY
SxxAxial stressYY
EPELxxAxial elastic strainYY
EPTOxxTotal strainYY
EPEQPlastic equivalent strain22
Cur.Yld.FlagCurrent yield flag22
PlwkPlastic strain energy density22
PressureHydrostatic pressure22
CreqCreep equivalent strain22
Crwk_CreepCreep strain energy density22
EPPLxxAxial plastic strain22
EPCRxxAxial creep strain22
EPTHxxAxial thermal strain33
EXT PRESSExternal pressure at integration point44
EFFECTIVE TENSEffective tension on link44
The following values apply to ocean loading only: [4]
GLOBAL COORDElement centroid location5Y
VR, VZRadial and vertical fluid particle velocities (VR is always > 0) 5Y
AR, AZRadial and vertical fluid particle accelerations5Y
PHDYNDynamic fluid pressure head 5Y
ETAWave amplitude over integration point5Y
TFLUIDFluid temperature (printed if VISC is nonzero) 5Y
VISCViscosity (output if VISC is nonzero)5Y
REN, RETNormal and tangential Reynolds numbers (if VISC is nonzero) 5Y
CTInput tangential drag coefficients evaluated at Reynolds numbers 5Y
CDY, CDZInput normal drag coefficients evaluated at Reynolds numbers 5Y
CMY, CMZInput inertia coefficients evaluated at Reynolds numbers5Y
URT, URNTangential (parallel to element axis) and normal relative velocities5Y
ABURNVector sum of normal (URN) velocities 5Y
ANAccelerations normal to element5Y
FX, FY, FZHydrodynamic tangential and normal forces in element coordinates5Y
ARGUEffective position of wave (radians)5Y

  1. Available only at the centroid as a *GET item.

  2. Available only if the element has an appropriate nonlinear material.

  3. Available only if the element temperatures differ from the reference temperature.

  4. Values are given as the average of the hydrodynamic integration points, which are distributed along the wetted portion of the element.

  5. See KEYOPT(12) description.

The element printout also includes 'INT, SEC PTS' (which are always '1, Y Z' where Y and Z both have values of 0.0). These values are printed to maintain formatting consistency with the output printouts of the BEAM188, BEAM189, PIPE288, and PIPE289 elements.

Table 180.2: LINK180 Item and Sequence Numbers lists output available through ETABLE using the Sequence Number method. See The General Postprocessor (POST1) and The Item and Sequence Number Table in this reference for more information. The following notation is used in Table 180.2: LINK180 Item and Sequence Numbers:


output quantity as defined in Table 180.1: LINK180 Element Output Definitions


predetermined Item label for ETABLE and



sequence number for single-valued or constant element data


sequence number for data at nodes I and J

Table 180.2:  LINK180 Item and Sequence Numbers

Output Quantity NameETABLE and ESOL Command Input
EPTOxxLEPTO [1]-12
The following output quantities are valid for ocean loading only and are averaged values for the element: [3]
VR, VZNMISC4, 5-- --
AR, AZNMISC6, 7 [4]-- --
PHDYNNMISC8 [4]-- --
ETANMISC9 [4]-- --
REN, RETNMISC12, 13 [5]-- --
CTNMISC14-- --
CDY, CDZ NMISC15, 16-- --
CMY, CMZNMISC17, 18 [4]-- --
URT, URNNMISC19, 20, 21-- --
ABURNNMISC22 [4]-- --
ANNMISC23, 24 [4]-- --
FX, FY, FZNMISC25, 26, 27-- --
ARGUNMISC28 [4]-- --

  1. This item is not available via the ESOL command.

  2. External pressure (EXT PRESS) and effective tension (EFFECTIVE TENS) occur at mid-length.

  3. Values are given as the average of the hydrodynamic integration points, which are distributed along the wetted portion of the element.

  4. See KEYOPT(12) description.

  5. These quantities are output only if a Reynold's number dependency is used.

LINK180 Assumptions and Restrictions

  • The spar element assumes a straight bar, axially loaded at its ends, and 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 cross-sectional area must be 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.

  • Stress stiffening is always included in geometrically nonlinear analyses (NLGEOM,ON). Prestress effects can be activated by the PSTRES command.

  • To simulate the tension-/compression-only options, a nonlinear iterative solution approach is necessary.

  • When the element is used in an ocean environment:

LINK180 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 Mechanical Pro 

  • Birth and death is not available.

  • Initial state is not available.

  • Ocean loading is not available.

  • Linear perturbation is not available.

ANSYS Mechanical Premium 

  • Birth and death is not available.

Release 18.2 - © ANSYS, Inc. All rights reserved.