4.51 SHELL51 Axisymmetric Structural Shell

4.51 SHELL51 Axisymmetric Structural Shell (UP19980821 ) SHELL51 has four degrees of freedom at each node: translations in the nodal x, y, and z directions and a rotation about the nodal z axis. Extreme orientations of the conical shell element result in a cylindrical shell element or an annular disc element. The shell element may have a linearly varying thickness. The element has plasticity, creep, swelling, stress stiffening, large deflection, and torsion capability. See Section 14.51 of the ANSYS Theory Reference for more details about this element. An axisymmetric conical shell element without nonlinear properties is described in Section 4.61.

Figure 4.51-1 SHELL51 Axisymmetric Structural Shell



4.51.1 Input Data

The geometry, node locations, and the coordinate system for this element are shown in Figure 4.51-1. The element is defined by two nodes, two end thicknesses, and the orthotropic material properties. For material property labels, the x-direction corresponds to the meridional direction of the shell element. The y-direction is through-the-thickness. The z-direction corresponds to the (or circumferential) direction. Properties not input default as described in Section 2.4.

The element may have variable thickness. The thickness is assumed to vary linearly between the nodes. If the element has a constant thickness, only TK(I) is required. Real constant ADMSUA is used to define an 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 4.51-1. Positive normal pressures act into the element. The pressures are applied at the surfaces of the element rather than at the centroidal plane so that some thickness effects can be considered. These include the increase or decrease in size of surface area the load is acting on and (in the case of a nonzero Poisson's ratio) an interaction effect causing the element to grow longer or shorter under equal pressures on both surfaces. Material properties EY, PRXY, and PRYZ (or EY, NUXY, and NUYZ) are required for this effect.

Temperatures and fluences may be input as element body loads at the four corner locations shown in Figure 4.51-1. 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, T3 defaults to T2 and T4 defaults to T1. For any other input pattern, unspecified temperatures default to TUNIF. Similar defaults occurs for fluence except that zero is used instead of TUNIF.

Nodal forces, if any, should be input on a full 360° basis. KEYOPT(3) is used to include or suppress the extra displacement shapes.

A summary of the element input is given in Table 4.51-1. A general description of element input is given in Section 2.1.

Table 4.51-1 SHELL51 Input Summary

Element Name

SHELL51

Nodes

I, J

Degrees of Freedom

UX, UY, UZ, ROTZ

Real Constants

TK ( I ), TK ( J ) (TK ( J ) defaults to TK ( I ) for constant thickness), ADMSUA

Material Properties

EX, EY, EZ, (PRXY, PRYZ, PRXZ or NUXY, NUYZ, NUXZ), ALPX, ALPZ, DENS, GXZ, DAMP (X is meridional, Y is through-thickness, Z is circumferential)

Surface Loads

Pressures:
face 1 (I-J) (top, in -Y direction),
face 2 (I-J) (bottom, in +Y direction)

Body Loads

Temperatures: T1, T2, T3, T4
Fluences: FL1, FL2, FL3, FL4

Special Features

Plasticity, Creep, Swelling, Stress stiffening, Large deflection,

KEYOPT(3)

0 - Include extra displacement shapes
1 - Suppress extra displacement shapes

KEYOPT(4)

0 - No printout of member forces and moments
1 - Print member forces and moments in the element coordinate system

4.51.2 Output Data

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

Several items are illustrated in Figure 4.51-2. The printout is displayed at the top, middle, and bottom locations (through-the-thickness) at element mid-length. 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 4.51-2 SHELL51 Stress Output



The following notation is used in Table 4.51-2:

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 4.51-2 SHELL51 Element Output Definitions

Name

Definition

O

R

EL

Element number

Y Y
NODES

Nodes - I, J

Y Y
MAT

Material number

Y Y
LEN

Distance between node I and node J

Y Y
CENT: X, Y

Global coordinates XC, YC

Y Y
TEMP

Temperatures T1, T2, T3, T4

Y Y
PRES

Pressures P1 (top) at nodes I,J; P2 (bottom) at nodes I,J

Y Y
FLUEN

Fluences FL1, FL2, FL3, FL4

Y Y
T(X, Z, XZ)

In-plane element X, Z, and XZ forces

Y Y
M(X, Z, XZ)

Element X, Z, and XZ moments

Y Y
MFOR(X, Y, Z)

Member forces for each node in the element coordinate system

1 1
MMOMZ

Member moment for each node in the element coordinate system

1 1
S(M, THK, H, MH)

Stresses (meridional, through-thickness, hoop, meridional-hoop)

2 2
EPEL(M, THK, H,
MH)

Elastic strains (meridional, through-thickness, hoop, meridional-hoop)

2 2
EPTH(M, THK, H,
MH)

Thermal strains(meridional, through-thickness, hoop, meridional-hoop)

2 2
EPPL(M, THK, H,
MH)

Plastic strains (meridional, through-thickness, hoop, meridional-hoop)

2 2
EPCR(M, THK, H,
MH)

Creep strains (meridional, through-thickness, hoop, meridional-hoop)

2 2
EPSW

Swelling strain

2 2
SEPL

Equivalent stress from stress-strain curve

2 2
SRAT

Ratio of trial stress to stress on yield surface

2 2
HPRES

Hydrostatic pressure

2 2
EPEQ

Equivalent plastic strain

2 2
S(1, 2, 3)

Principal stresses

2 2
SINT

Stress intensity

2 2
SEQV

Equivalent stress

2 2
1. If KEYOPT(4)=1

2. The item repeats at TOP, MID, and BOT locations

Table 4.51-3 lists output available through the ETABLE command using the Sequence Number method. See Chapter 5 of the ANSYS Basic Analysis Procedures Guide The following notation is used in Table 4.51-3:

Table 4.51-3 SHELL51 Item and Sequence Numbers for the ETABLE and ESOL Commands

Name

Item

Top

Mid

Bot

SM

LS

1 5 9
STHK

LS

2 6 10
SH

LS

3 7 11
SMH

LS

4 8 12
EPELM

LEPEL

1 5 9
EPELTHK

LEPEL

2 6 10
EPELH

LEPEL

3 7 11
EPELMH

LEPEL

4 8 12
EPTHM

LEPTH

1 6 11
EPTHTHK

LEPTH

2 7 12
EPTHH

LEPTH

3 8 13
EPTHMH

LEPTH

4 9 14
EPSW

LEPTH

5 10 15
EPPLM

LEPPL

1 5 9
EPPLTHK

LEPPL

2 6 10
EPPLH

LEPPL

3 7 11
EPPLMH

LEPPL

4 8 12
EPCRM

LEPCR

1 5 9
EPCRTHK

LEPCR

2 6 10
EPCRH

LEPCR

3 7 11
EPCRMH

LEPCR

4 8 12
SEPL

NLIN

1 5 9
SRAT

NLIN

2 6 10
HPRES

NLIN

3 7 11
EPEQ

NLIN

4 8 12
S1

NMISC

1 6 11
S2

NMISC

2 7 12
S3

NMISC

3 8 13
SINT

NMISC

4 9 14
SEQV

NMISC

5 10 15

E

I

J

MFORX

SMISC

- 1 7
MFORY

SMISC

- 2 8
MFORZ

SMISC

- 3 9
MMOMZ

SMISC

- 6 12
TX

SMISC

13 - -
TZ

SMISC

14 - -
TXZ

SMISC

15 - -
MX

SMISC

16 - -
MZ

SMISC

17 - -
MXZ

SMISC

18 - -
P1

SMISC

- 19 20
P2

SMISC

- 23 24

Corner Location

1

2

3

4

FLUEN

NMISC

16 17 18 19
TEMP

LBFE

1 2 3 4

4.51.3 Assumptions and Restrictions

The axisymmetric shell element must be defined in the global X-Y plane with the Y axis the axis of symmetry. The element must not have a zero length. Both ends must have non-negative X coordinate values and the element must not lie along the global Y axis.

Even though the element has a displacement shape which permits a cubic displacement function, it should be thought of as a constant-curvature element, since plastic effects are considered only midway between the two nodes.

If the element has a constant thickness, only TK(I) need be defined. TK(I) must not be zero. The element thickness varies linearly from node I to node J. Some thick shell effects have been included in the formulation of SHELL51 but it cannot be properly considered to be a thick shell element. If these effects are important, it is recommended to use PLANE42. Nonlinear material properties must be isotropic. The element may not be deactivated with the EKILL command.

Stress stiffening effects are based on the average section stress midway between nodes I and J. An assemblage of flat shell elements can produce an approximation to a curved shell surface, but each flat element should not extend over more than a 5° arc.

4.51.4 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