4.63 SHELL63 Elastic Shell

Figure 4.63-1 SHELL63 Elastic Shell

4.63.1 Input Data

The thickness is assumed to vary smoothly over the area of the element, with the thickness input at the four 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 elastic foundation stiffness (EFS) is defined as the pressure required to produce a unit normal deflection of the foundation. The elastic foundation capability is bypassed if EFS is less than, or equal to, zero.

For certain nonhomogeneous or sandwich shell applications, the following real constants are provided: RMI is the ratio of the bending moment of inertia to be used to that calculated from the input thicknesses. RMI defaults to 1.0. CTOP and CBOT are the distances from the middle surface to the extreme fibers to be used for stress evaluations. Both CTOP and CBOT are positive, assuming that the middle surface is between the fibers used for stress evaluation. If not input, stresses are based on the input thicknesses. 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 4.63-1. Positive pressures act into the element. Edge pressures are input as force per unit length. The lateral pressure loading may be an equivalent (lumped) element load applied at the nodes (KEYOPT(6)=0) or distributed over the face of the element (KEYOPT(6)=2). The equivalent element load produces more accurate stress results with flat elements representing a curved surface or elements supported on an elastic foundation since certain fictitious bending stresses are eliminated.

Temperatures may be input as element body loads at the "corner" locations (1-8) shown in Figure 4.63-1. 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.

KEYOPT(1) is available for neglecting the membrane stiffness or the bending stiffness, if desired. A reduced out-of-plane mass matrix is also used when the bending stiffness is neglected.

KEYOPT(2) is used to activate the consistent tangent stiffness matrix (i.e., a matrix composed of the main tangent stiffness matrix plus the consistent stress stiffness matrix) in large deflection analyses [NLGEOM,ON]. You can often obtain more rapid convergence in a geometrically nonlinear analysis, such as a nonlinear buckling or postbuckling analysis, by activating this option. However, you should not use this option if you are using the element to simulate a rigid link or a group of coupled nodes. The resulting abrupt changes in stiffness within the structure make the consistent tangent stiffness matrix unsuitable for such applications.

KEYOPT(3) allows you to include (KEYOPT(3)=0 or 2) or suppress (KEYOPT(3)=1) extra displacement shapes. It also allows you to choose the type of in-plane rotational stiffness used:

• KEYOPT(3)=0 or 1 activates a spring-type in-plane rotational stiffness about the element z-axis
• KEYOPT(3)=2 activates a more realistic in-plane rotational stiffness (Allman rotational stiffness-the program uses default penalty parameter values of d₁=1.0E-6 and d₂=1.0E-3).

KEYOPT(7) allows a reduced mass matrix formulation (rotational degrees of freedom terms deleted). This option is useful for improved bending stresses in thin members under mass loading.

KEYOPT(8) allows a reduced stress stiffness matrix (rotational degrees of freedom deleted). This option can be useful for calculating improved mode shapes and a more accurate load factor in linear buckling analyses of certain curved shell structures.

A summary of the element input is given in Table 4.63-1. A general description of element input is given in Section 2.1.

Table 4.63-1 SHELL63 Input Summary

Element Name	SHELL63
Nodes	I, J, K, L
Degrees of Freedom	UX, UY, UZ, ROTX, ROTY, ROTZ
Real Constants	TK (I), TK (J), TK (K), TK (L), EFS, THETA, RMI, CTOP, CBOT, (Blank), (Blank), (Blank), (Blank), (Blank), (Blank), (Blank), (Blank), (Blank), ADMSUA
Material Properties	EX, EY, EZ, (PRXY, PRYZ, PRXZ or NUXY, NUYZ, NUXZ), ALPX, ALPY, ALPZ, DENS, GXY, 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
Special Features	Stress stiffening, Large deflection, Birth and death
KEYOPT(1)	0 - Bending and membrane stiffness 1 - Membrane stiffness only 2 - Bending stiffness only
KEYOPT(2)	0 - Use only the main tangent stiffness matrix when NLGEOM is ON. (Stress stiffening effects used in linear buckling or other linear prestressed analyses must be activated separately with PSTRES,ON.) 1 - Use the consistent tangent stiffness matrix (i.e., a matrix composed of the main tangent stiffness matrix plus the consistent stress stiffness matrix) when NLGEOM is ON and when KEYOPT(1)=0. (SSTIF,ON will be ignored for this element when KEYOPT(2)=1 is activated.) Note that if SOLCONTROL is ON and NLGEOM is ON, KEYOPT(2) is automatically set to 1; i.e., the consistent tangent will be used.
KEYOPT(3)	0 - Include extra displacement shapes, and use spring-type in-plane rotational stiffness about the element z-axis (the program automatically adds a small stiffness to prevent numerical instability for non-warped elements if KEYOPT(1)=0). 1 - Suppress extra displacement shapes, and use spring-type in-plane rotational stiffness about the element z-axis (the program automatically adds a small stiffness to prevent numerical instability for non-warped elements if KEYOPT(1)=0). 2 - Include extra displacement shapes, and use the Allman in-plane rotational stiffness about the element z-axis). See Section 14.43.6 of the ANSYS Theory Reference.
KEYOPT(5)	0 - Basic element printout 2 - Nodal stress printout
KEYOPT(6)	0 - Reduced pressure loading (must be used if KEYOPT(1)=1) 2 - Consistent pressure loading
KEYOPT(7)	0 - Consistent mass matrix 1 - Reduced mass matrix
KEYOPT(8)	0 - "Nearly" consistent stress stiffness matrix (default) 1 - Reduced stress stiffness matrix
KEYOPT(9)	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)

4.63.2 Output Data

• nodal displacements included in the overall nodal solution
• additional element output as shown in Table 4.63-2

Figure 4.63-2 SHELL63 Stress Output

The following notation is used in Table 4.63-2:

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 4.63-2 SHELL63 Element Output Definitions

Name	Definition	O	R
EL	Element number	Y	Y
NODES	Nodes - I, J, K, L	Y	Y
MAT	Material number	Y	Y
AREA	Area	Y	Y
CENT: X, Y, Zb	Global X, Y, Z location	Y	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
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
FOUND.PRESS	Foundation pressure (if nonzero)	Y	-
LOC	Top, middle, or bottom	Y	Y
S: X, Y, Z, XY	Combined membrane and bending stresses	Y	Y
S: 1, 2, 3	Principal stresses	Y	Y
S:INT	Stress intensity	Y	Y
S:EQV	Equivalent stress	Y	Y

Table 4.63-2a SHELL63 Miscellaneous Element Output

Description	Names of Items Output	O	R
Nodal Stress Solution	TEMP, S(X, Y, Z, XY), SINT, SEQV	1	-

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

Table 4.63-3 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 4.63-3:

Name - output quantity as defined in the Table 4.63-2

Item - predetermined Item label for ETABLE command

E - sequence number for single-valued or constant element data

I,J,K,L - sequence number for data at nodes I,J,K,L

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	-	-	-	-
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

4.63.3 Assumptions and Restrictions

An assemblage of flat shell elements can produce a good approximation to a curved shell surface provided that each flat element does not extend over more than a 15° arc. If an elastic foundation stiffness is input, one-fourth of the total is applied at each node. Shear deflection is not included in this thin-shell element.

A triangular element may be formed by defining duplicate K and L node numbers as described in Section 2.8. The extra shapes are automatically deleted for triangular elements so that the membrane stiffness reduces to a constant strain formulation. For large deflection analyses, if KEYOPT(1)=1 (membrane stiffness only), the element must be triangular.

The four nodes defining the element should lie in an exact flat plane; however, a small out-of-plane tolerance is permitted so that the element may have a slightly warped shape. A moderately warped element will produce a warning message in the printout. If the warpage is too severe, a fatal message results and a triangular element should be used, see Section 2.8. If the lumped mass matrix formulation is specified [LUMPM,ON], the effect of the implied offsets on the mass matrix is ignored for warped SHELL63 elements.

4.63.4 Product Restrictions

ANSYS/LinearPlus

• The DAMP material property is not allowed.
• The only special features allowed are stress stiffening and large deflection.
• KEYOPT(2) can only be set to 0 (default).
• KEYOPT(9) can only be set to 0 (default).