4.93 SHELL93 8-Node Structural Shell

4.93 SHELL93 8-Node Structural Shell (UP19980821 ) SHELL93 is particularly well suited to model curved shells. 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 quadratic in both in-plane directions. The element has plasticity, stress stiffening, large deflection, and large strain capabilities. See Section 14.93 of the ANSYS Theory Reference for more details about this element.

Figure 4.93-1 SHELL93 8-Node Structural Shell



4.93.1 Input Data

The geometry, node locations, and the coordinate system for this element are shown in Figure 4.93-1. The element is defined by eight nodes, four thicknesses, and the orthotropic material properties. Midside nodes may not be removed from this element. See Section 2.4.2 of the ANSYS Modeling and Meshing Guide for additional information about the use of midside nodes. A triangular-shaped element may be formed by defining the same node number for nodes K, L and O.

Orthotropic material directions correspond to the element coordinate directions. The element coordinate system orientation is as described in Section 2.3. The element x and y axes are in the plane of the element. The x axis may be rotated an angle THETA (in degrees) toward the 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. The thickness at the midside nodes is taken as the average of the corresponding 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. The total thickness of each shell element must be less than twice the radius of curvature, and should be less than one-fifth the radius of curvature. 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 4.93-1. 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 4.93-1. 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. Only the lumped mass matrix is available.

A summary of the element input is given in Table 4.93-1. A general description of element input is given in Section 2.1.

Table 4.93-1 SHELL93 Input Summary

Element Name

SHELL93

Nodes

I, J, K, L, M, N, O, P

Degrees of Freedom

UX, UY, UZ, ROTX, ROTY, ROTZ

Real Constants

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

Material Properties

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

Temperature:
T1, T2, T3, T4, T5, T6, T7, T8

Special Features

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

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 more information on user written subroutines)

KEYOPT(5)

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

KEYOPT(6)

0 - Basic element printout
1 - Nonlinear integration point printout

4.93.2 Output Data

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

Several items are illustrated in Figure 4.93-2. Printout includes the moments about the x face (MX), the moments about the y face (MY), and the twisting moment (MXY). The moments are calculated per unit length in the element coordinate system. 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 face IJKL, the element centroid, and at the center of the bottom of face IJKL. 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 4.93-2 SHELL93 Stress Output



The following notation is used in Table 4.93-2:

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 4.93-2 SHELL93 Element Output Definitions

Name

Definition

O

R

EL

Element number and name

Y Y
NODES

Nodes - I, J, K, L, M, N, O, P

Y Y
MAT

Material number

Y Y
THICK

Average thickness

Y Y
VOLU:

Volume

Y Y
CENT: X, Y, Z

Global 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

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

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

Table 4.93-2a SHELL93 Miscellaneous Element Output

Description

Names of Items Output

O

R

Nonlinear Integration Pt. Solution

EPPL, EPEQ, SRAT, SEPL

1 -
Nodal Stress Solution

TEMP, S, SINT, SEQV

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

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

Table 4.93-3 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 4.93-3:

Table 4.93-3 SHELL93 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 - - - -
THICK

NMISC

49 - - - -
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
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
Bot

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

4.93.3 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. The applied transverse thermal gradient is assumed to vary linearly through the thickness. Shear deflections are included in this element. 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. The transverse shear strains are assumed to be small in a large strain analysis. This element may produce inaccurate stress under thermal loads for doubly curved or warped domains.

4.93.4 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/LinearPlus