MET 415 - FEA Applications I

Prof. Dave Johnson, psuprofdj@psu.edu, Penn State Erie, The Behrend College

Line Elements


Represent structures that are "long" compared to their cross-section.

These elements are the simplest (geometrically speaking), and are efficient models, but are complex in usage (postprocessing - but is easier with PowerGraphics + /ESHAPE)

Beams give "general system performance," not localized behavior

Normally solid modeling and automatic meshing is NOT useful for line element models.  Often use direct definition of nodes and elements.

Truss (spar) elements are a subset of beam-type elements which can’t carry moments (i.e., have no bending DOF’s). These are commonly called "two-force members", carrying only axial load.

ANSYS Truss elements: LINK180 (3D)

Every node in a truss model is a ball and socket (or spherical) joint.

Use only one element between pins.

DOF’s: UX, UY, UZ (in 3D)

Material Props: Modulus, Density, ALPX

Section Data: Area, Added Mass (SECTYPE, SECDATA, SECCONTROL)

Preprocessor > Sections > Link > Add

ANSYS BEAM Elements: BEAM188, BEAM189 (3D)

DOFs: UX, UY, UZ, ROTZ, ROTY, ROTX (in 3D)

Material Props: Modulus, Density, ALPX, Shear Modulus,

Special options: tapered sect., offset from nodes, moment release

Beam Coordinate systems orient the element’s y- and z-axes for moments IYY and IZZ (could be: strong and weak bending directions)

The beam’s neutral axis is (default) along the line of nodes (element x-axis).

For BEAM188 & 189, ANSYS has 11 predefined sections, or you can sketch your own:

Preprocessor > Sections > Beam > Common Sections

Preprocessor > Sections > Beam > Custom Sections

You must orient the cross-section.

ANSYS: uses an "extra" node (K) (or keypoint)

ANSYS 13.0 Structural Analysis Guide, Chapter 1. Overview of Structural Analyses,
Section 1.2. Elements Used in Structural Analyses

Spars LINK180
Beams BEAM188, BEAM189
Pipes PIPE288, PIPE289, ELBOW290

Why pick a truss or a beam ?  

Truss (LINK180) "joints" 

Symmetry ?

How to make a "pin joint" on BEAM models ?


Nuclear piping network model: 122 nodes, 129 elements:

42 straight pipe element that could yield (PIPE20*), 8 pipe elbows that could yield (PIPE60*), 10 lumped mass elements (MASS21), 12 elastic pipe elements (PIPE16*), 15 support spring elements (COMBIN40), 6 linear spring elements at right end - steam generator (COMBIN14), 34 contact elements to contain dangerous pipe whip (CONTAC52). [*Note: In ANSYS 13, PIPE16, PIPE20, PIPE60 have been replaced with PIPE288 and ELBOW290]

This model is loaded with internal pipe pressure, temperature load which cause thermal expansion and effects material properties.  The simulation also include seismic loading (earthquake), as well as a pressure wave transmitted in the fluid (both are dynamic conditions).

Results needed: membrane stress and membrane+bending stress in the pipe, pipe support loads, whip restraint loads, steam generator loads, valve velocity.

            Several ASME codes are checked to certify safety and acceptable design.

Areas and lines: simple solid model of a machinery base plate

SHELL181 and BEAM188 model.  BEAM188 with section shape and offset defined.


NOTE (Not on class handout) 2012 Storage Racks:

Three shelf validation model:

60 nodes, 41 elements [ (6) MASS21, (3) COMBIN14 springs, (30) BEAM188, (2) CONTA178 ]

7680 load steps (earthquake, 30 seconds time history).  Solve time ~15 minutes.