4.43 SHELL43 Plastic Large Strain Shell

4.43 SHELL43 Plastic Large Strain Shell (UP19980821 ) SHELL43 is well suited to model linear, warped, moderately-thick shell structures. The element has six degrees of freedom at each node: translations in the nodal x, y, and z directions and rotations about the nodal x, y, and z axes. The deformation shapes are linear in both in-plane directions. For the out-of-plane motion, it uses a mixed interpolation of tensorial components.

The element has plasticity, creep, stress stiffening, large deflection, and large strain capabilities. See Section 14.43 of the ANSYS Theory Reference for more details about this element. For a thin shell capability or if plasticity or creep is not needed, the elastic quadrilateral shell (SHELL63) may be used. If convergence difficulties are encountered and large strain capability is needed, use SHELL181. Also, we recommend using SHELL181 for nonlinear structures.

Figure 4.43-1 SHELL43 Plastic Large Strain Shell



4.43.1 Input Data

The geometry, node locations, and the coordinate system for this element are shown in Figure 4.43-1. The element is defined by four nodes, four thicknesses, and the orthotropic material properties. A triangular-shaped element may be formed by defining the same node number for nodes K and L as described in Section 2.8.

Orthotropic material directions correspond to the element coordinate directions. The element coordinate system orientation is as described in Section 2.3. The element x axis may be rotated an angle THETA (in degrees) from the element x axis toward the element y axis. Properties not input default as described in Section 2.4.

The element may have variable thickness. The thickness is assumed to vary smoothly over the area of the element, with the thickness input at the corner nodes. If the element has a constant thickness, only TK(I) need be input. If the thickness is not constant, all four thicknesses must be input.

A nominal in-plane rotational stiffness about the element z axis is used for KEYOPT(3)=0 or 1. A more realistic rotational stiffness (Allman rotation) may alternately be defined (KEYOPT(3)=2). In this case, real constants ZSTIF1 and ZSTIF2 are used to control the two spurious zero energy modes usually introduced by the Allman rotation. Default values of 1.0E-6 and 1.0E-3 are provided for ZSTIF1 and ZSTIF2, respectively. ADMSUA is the added mass per unit area.

Element loads are described in Section 2.7. Pressures may be input as surface loads on the element faces as shown by the circled numbers on Figure 4.43-1. Positive pressures act into the element. Edge pressures are input as force per unit length. Temperatures may be input as element body loads at the "corner" locations (1-8) shown in Figure 4.43-1. The first corner temperature T1 defaults to TUNIF. If all other temperatures are unspecified, they default to T1. If only T1 and T2 are input, T1 is used for T1, T2, T3, and T4, while T2 (as input) is used for T5, T6, T7, and T8. For any other input pattern, unspecified temperatures default to TUNIF.

A summary of the element input is given in Table 4.43-1. A general description of element input is given in Section 2.1.

Table 4.43-1 SHELL43 Input Summary

Element Name

SHELL43

Nodes

I, J, K, L

Degrees of Freedom

UX, UY, UZ, ROTX, ROTY, ROTZ

Real Constants

TK(I), TK(J), TK(K), TK(L), THETA, ZSTIF1,
ZSTIF2, ADMSUA

Material Properties

EX, EY, EZ, (PRXY, PRYZ, PRXZ or NUXY, NUYZ, NUXZ), ALPX, ALPY, ALPZ, DENS, GXY, GYZ, GXZ, DAMP

Surface Loads

Pressures:
face 1 (I-J-K-L) (bottom, in +Z direction),
face 2 (I-J-K-L) (top, in -Z direction),
face 3 (J-I), face 4 (K-J), face 5 (L-K), face 6 (I-L)

Body Loads

Temperatures:
T1, T2, T3, T4, T5, T6, T7, T8
Fluences:
FL1, FL2, FL3, FL4, FL5, FL6, FL7, FL8

Special Features

Plasticity, Creep, Stress stiffening, Large deflection, Large strain, Birth and death, Adaptive descent

KEYOPT(3)

0 - Include in-plane extra displacement shapes
1 - Suppress extra displacement shapes
2 - Include Allman rotational stiffness (use real constants ZSTIF1 and ZSTIF2)

KEYOPT(4)

0 - No user subroutine to define element coordinate system
4 - Element x-axis located by user subroutine USERAN (see the Guide to ANSYS User Programmable Features for user written subroutines)

KEYOPT(5)

0 - Basic element solution
1 - Repeat basic solution for all integration points and top, middle and bottom surfaces
2 - Nodal stress solution

KEYOPT(6)

0 - Basic element solution
1 - Nonlinear integration point solution

4.43.2 Output Data

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

Several items are illustrated in Figure 4.43-2.

The element stress directions and force resultants (NX, MX, TX, etc.) are parallel to the element coordinate system. The basic element printout is given at the center of the top of surface IJKL, the element centroid, and at the center of the bottom of surface IJKL. For triangular element configurations, the face centers and the element centroid are averaged values. 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 4.43-2 SHELL43 Stress Output



The following notation is used in Table 4.43-2:

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 4.43-2 SHELL43 Element Output Definitions

Name

Definition

O

R

EL

Element number and name

Y Y
NODES

Nodes - I, J, K, L

Y Y
MAT

Material number

Y Y
THICK

Average thickness

Y Y
VOLU:

Volume

Y Y
CENT: X, Y, Z

Center location XC, YC, ZC

- Y
PRES

Pressures P1 at NODES I, J, K, L; P2 at I, J, K, L; P3 at J,I; P4 at K,J; P5 at L,K; P6 at I,L

Y Y
TEMP

Temperatures T1, T2, T3, T4, T5, T6, T7, T8

Y Y
LOC

TOP, MID, BOT, or integration point location

1 1
S:INT

Stress intensity

1 1
S:EQV

Equivalent stress

1 1
EPEL: X, Y, Z, XY, YZ, XZ

Elastic strains

1 1
EPEL: 1, 2, 3

Principal elastic strains

1 1
S: X, Y, Z,
XY, YZ, XZ

Stresses

1 1
S: 1, 2, 3

Principal stresses

1 1
T(X,Y,XY)

In-plane element X, Y, and XY forces

Y Y
M(X,Y,XY)

Element X, Y, and XY moments

Y Y
N(X,Y)

Out-of-plane element X and Y shear forces

Y Y
EPPL: X, Y, Z, XY, YZ, XZ

Average plastic strains

2 2
NL:EPEQ

Average equivalent plastic strain

2 2
NL:SRAT

Ratio of trial stress to stress on yield surface

2 2
NL:SEPL

Average equivalent stress from stress-strain curve

2 2
EPCR: X, Y, Z, XY, YZ, XZ

Average creep strains (X, Y, Z, XY, YZ, XZ)

2 2
1. The following stress solution repeats for top, middle, and bottom surfaces (and also for all integration points if KEYOPT(5)=1)

2. Nonlinear solution output for top, middle, and bottom surfaces, if the element has a nonlinear material

Table 4.43-2a SHELL43 Miscellaneous Element Output

Description

Names of Items Output

O

R

Nonlinear Integration Pt. Solution

EPPL, EPEQ, SRAT, SEPL, EPCR

1 -
Nodal Stress Solution

TEMP, S(X, Y, Z, XY, YZ, XZ), SINT, SEQV

2 -
1. Output at each integration point, if the element has a nonlinear material and KEYOPT(6)=1

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

Table 4.43-3 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 of this manual for more information. The following notation is used in Table 4.43-3:

Table 4.43-3 SHELL43 Item and Sequence Numbers for the ETABLE and ESOL Commands

Name

Item

E

I

J

K

L

TX

SMISC

1 - - - -
TY

SMISC

2 - - - -
TXY

SMISC

3 - - - -
MX

SMISC

4 - - - -
MY

SMISC

5 - - - -
MXY

SMISC

6 - - - -
NX

SMISC

7 - - - -
NY

SMISC

8 - - - -
P1

SMISC

- 9 10 11 12
P2

SMISC

- 13 14 15 16
P3

SMISC

- 18 17 - -
P4

SMISC

- - 20 19 -
P5

SMISC

- - - 22 21
P6

SMISC

- 23 - - 24
THICK

NMISC

49 - - - -
Top

S:1

NMISC

- 1 6 11 16
S:2

NMISC

- 2 7 12 17
S:3

NMISC

- 3 8 13 18
S:INT

NMISC

- 4 9 14 19
S:EQV

NMISC

- 5 10 15 20
Bottom

S:1

NMISC

- 21 26 31 36
S:2

NMISC

- 22 27 32 37
S:3

NMISC

- 23 28 33 38
S:INT

NMISC

- 24 29 34 39
S:EQV

NMISC

- 25 30 35 40

Corner Location

1

2

3

4

5

6

7

8

FLUEN

NMISC

41 42 43 44 45 46 47 48

4.43.3 Assumptions and Restrictions

Zero area elements are not allowed. This occurs most often whenever the elements are not numbered properly. Zero thickness elements or elements tapering down to a zero thickness at any corner are not allowed. Under bending loads, tapered elements produce inferior stress results and refined meshes may be required. Use of this element in triangular form produces results of inferior quality compared to the quadrilateral form. However, under thermal loads, when the element is doubly curved (warped), triangular SHELL43 elements produce more accurate stress results than do quadrilateral shaped elements. Quadrilateral SHELL43 elements may produce inaccurate stresses under thermal loads for doubly curved or warped domains. The applied transverse thermal gradient is assumed to vary linearly through the thickness. The out-of-plane (normal) stress for this element varies linearly through the thickness. The transverse shear stresses (SYZ and SXZ) are assumed to be constant through the thickness.

Shear deflections are included. Elastic rectangular elements without membrane loads give constant curvature results, i.e., nodal stresses are the same as the centroidal stresses. For linearly varying results use SHELL63 (no shear deflection) or SHELL93 (with midside nodes). Triangular elements are not geometrically invariant and the element produces a constant curvature solution. Only the lumped mass matrix is available.

4.43.4 Product Restrictions

There are no product-specific restrictions for this element.