mkb04plane42(1).pdf

Strona 1 z 7

Main TOC • Using Help • Copyright

Element Reference > Part I. Element Library >PLANE42

PLANE42 — 2-D Structural Solid

MP ME ST PR PP ED

Element Description

PLANE42 is used for 2-D modeling of solid structures. The element can be used either as a plane element

(plane stress or plane strain) or as an axisymmetric element. The element is defined by four nodes having

two degrees of freedom at each node: translations in the nodal x and y directions. The element has

plasticity, creep, swelling, stress stiffening, large deflection, and large strain capabilities.

An option is available to suppress the extra displacement shapes. See the ANSYS, Inc. Theory Reference

for more details about this element. See PLANE82 for a multi-node version of this element. See

PLANE25 for an axisymmetric version that accepts nonaxisymmetric loading.

Figure 42.1. PLANE42 2-D Structural Solid

Input Data

The geometry, node locations, and the coordinate system for this element are shown in PLANE42 . The

element input data includes four nodes, a thickness (for the plane stress option only) and the orthotropic

material properties. Orthotropic material directions correspond to the element coordinate directions. The

element coordinate system orientation is as described in Coordinate Systems .

Element loads are described in Node and Element Loads . Pressures may be input as surface loads on the

element faces as shown by the circled numbers on PLANE42 . Positive pressures act into the element.

Temperatures and fluences may be input as element body loads at the nodes. The node I temperature T(I)

defaults to TUNIF. If all other temperatures are unspecified, they default to T(I). For any other input

pattern, unspecified temperatures default to TUNIF. Similar defaults occurs for fluence except that zero is

used instead of TUNIF.

file://C:\TEMP\BYXIS108.htm

06.11.02

Strona 2 z 7

The nodal forces, if any, should be input per unit of depth for a plane analysis (except for KEYOPT(3) =

3) and on a full 360° basis for an axisymmetric analysis. KEYOPT(2) is used to include or suppress the

extra displacement shapes.

KEYOPT(5) and KEYOPT(6) provide various element printout options (see Element Solution ).

KEYOPT(9) = 1 is used to read initial stress data from a user subroutine. For details about these user

subroutines, see the ANSYS Guide to User Programmable Features .

You can include the effects of pressure load stiffness in a geometric nonlinear analysis using

SOLCONTROL ,,,INCP. Pressure load stiffness effects are included in linear eigenvalue buckling

automatically. If an unsymmetric matrix is needed for pressure load stiffness effects, use

NROPT ,UNSYM.

A summary of the element input is given in Input Summary . A general description of element input is

given in Element Input .

PLANE42 Input Summary

Element Name

PLANE42

Nodes

I, J, K, L

Degrees of Freedom

UX, UY

Real Constants

None, if KEYOPT (3) = 0, 1, 2

Thickness, if KEYOPT (3) = 3

Material Properties

EX, EY, EZ, (PRXY, PRYZ, PRXZ or NUXY, NUYZ, NUXZ),

ALPX, ALPY,ALPZ, DENS, GXY, DAMP

Surface Loads

Pressures --

face 1 (J-I), face 2 (K-J), face 3 (L-K), face 4 (I-L)

Body Loads

Temperatures --

T(I), T(J), T(K), T(L)

Fluences --

FL(I), FL(J), FL(K), FL(L)

Special Features

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

Adaptive descent

KEYOPT(1)

0 --

Element coordinate system is parallel to the global coordinate system

1 --

Element coordinate system is based on the element I-J side

KEYOPT(2)

0 --

Include extra displacement shapes

1 --

file://C:\TEMP\BYXIS108.htm

06.11.02

Strona 3 z 7

Suppress extra displacement shapes

KEYOPT(3)

0 --

Plane stress

1 --

Axisymmetric

2 --

Plane strain (Z strain = 0.0)

3 --

Plane stress with thickness input

KEYOPT(5)

0 --

Basic element solution

1 --

Repeat basic solution for all integration points

2 --

Nodal Stress Solution

KEYOPT(6)

0 --

Basic element solution

1 --

Surface solution for face I-J also.

2 --

Surface solution for both faces I-J and K-L also. (Surface solution available for linear

materials only)

3 --

Nonlinear solution at each integration point also.

4 --

Surface solution for faces with nonzero pressure

KEYOPT(9)

0 --

No user subroutine to provide initial stress (default)

1 --

Read initial stress data from user subroutine USTRESS

Note

See the ANSYS Guide to User Programmable Features for user written subroutines

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 Element Output Definitions

Several items are illustrated in Stress output .

The element stress directions are parallel to the element coordinate system. Surface stresses are available

file://C:\TEMP\BYXIS108.htm

06.11.02

Strona 4 z 7

on any face. Surface stresses on face IJ, for example, are defined parallel and perpendicular to the IJ line

and along the Z axis for a plane analysis or in the hoop direction for an axisymmetric analysis. A general

description of solution output is given in Solution Output . See the ANSYS Basic Analysis Guide for ways

to view results.

Figure 42.2. PLANE42 Stress Output

Stress directions shown are for KEYOPT(1) = 0

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 42.1. PLANE42 Element Output Definitions

Name

Definition

O R

Element Number

Y Y

NODES

Nodes - I, J, K, L

Y Y

MAT

Material number

Y Y

THICK

Average thickness

Y Y

VOLU:

Volume

Y Y

XC, YC

Location where results are reported

Y 3

PRES

Pressures P1 at nodes J,I; P2 at K,J; P3 at L,K; P4 at I,L Y Y

TEMP

Temperatures T(I), T(J), T(K), T(L)

Y Y

FLUEN

Fluences FL(I), FL(J), FL(K), FL(L)

Y Y

S: X, Y, Z, XY

Stresses (SZ = 0.0 for plane stress elements)

Y Y

S: 1, 2, 3

Principal stresses

Y -

S: INT

Stress intensity

Y -

S: EQV

Equivalent stress

Y Y

EPEL: X, Y, Z, XY Elastic strains

Y Y

EPEL: 1, 2, 3

Principal elastic strain

Y -

file://C:\TEMP\BYXIS108.htm

06.11.02

Strona 5 z 7

EPEL: EQV Equivalent elastic strain [ 4 ] - Y

EPTH: X, Y, Z, XY Average thermal strain Y Y

EPTH: EQV Equivalent thermal strain [ 4 ] - Y

EPPL: X, Y, Z, XY Plastic strain 1 1

EPPL: EQV Equivalent plastic strain [ 4 ] - 1

EPCR: X, Y, Z, XY Creep strains 1 1

EPCR: EQV Equivalent creep strains [ 4 ] - 1

EPSW: Swelling strain 1 1

NL: EPEQ Equivalent plastic strain 1 1

NL: SRAT Ratio of trial stress to stress on yield surface 1 1

NL: SEPL Equivalent stress on stress-strain curve 1 1

NL: HPRES Hydrostatic pressure - 1

FACE Face label 2 2

EPEL(PAR,PER, Z) Surface elastic strains (parallel, perpendicular, Z or hoop) 2 2

TEMP

Surface average temperature

2 2

S(PAR,PER,Z)

Surface stresses (parallel, perpendicular, Z or hoop)

2 2

SINT

Surface stress intensity

2 2

SEQV

Surface equivalent stress

2 2

LOCI: X, Y, Z

Integration point locations

- Y

1. Nonlinear solution, output only if the element has a nonlinear material.

2. Surface output (if KEYOPT(6) is 1,2, or 4)

3. Available only at centroid as a *GET item.

4. The equivalent strains use an effective Poisson's ratio: for elastic and thermal this value is set by the

user ( MP ,PRXY); for plastic and creep this value is set at 0.5.

Table 42.2. PLANE42 Miscellaneous Element Output

Description Names of Items Output O R

Nonlinear Integration Pt. Solution EPPL, EPEQ, SRAT, SEPL, HPRES, EPCR, EPSW 1 -

Integration Point Solution

TEMP, SINT, SEQV, EPEL, S

2 -

Nodal Stress Solution

TEMP, S, SINT, SEQV

3 -

1. Output at each integration point, if the element has a nonlinear material and KEYOPT(6) = 3

2. Output at each integration point, if KEYOPT(5) = 1

3. Output at each node, if KEYOPT(5) = 2

Note

For axisymmetric solutions with KEYOPT(1) = 0, the X,Y,Z, and XY stress and strain

outputs correspond to the radial, axial, hoop, and in-plane shear stresses and strains,

respectively.

file://C:\TEMP\BYXIS108.htm

06.11.02

Plik z chomika:

Inne pliki z tego folderu:

Inne foldery tego chomika: