SHELL63


Elastic Shell

Valid Products: Pro | Premium | Enterprise | PrepPost | Solver | AS add-on

SHELL63 Element Description

Although this archived element is available for use in your analysis, Ansys, Inc. recommends using a current-technology element such as SHELL181 (KEYOPT(3) = 2).

SHELL63 has both bending and membrane capabilities. Both in-plane and normal loads are permitted. 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. Stress stiffening and large deflection capabilities are included. A consistent tangent stiffness matrix option is available for use in large deflection (finite rotation) analyses. See SHELL63 for more details about this element. Similar elements are SHELL181 (plastic capability) and SHELL281 (midside node capability). The ETCHG command converts SHELL157 elements to SHELL63.

Figure 63.1: SHELL63 Geometry

SHELL63 Geometry

xIJ = Element x-axis if ESYS is not supplied.

x = Element x-axis if ESYS is supplied.


SHELL63 Input Data

The geometry, node locations, and the coordinate system for this element are shown in Figure 63.1: SHELL63 Geometry. The element is defined by four nodes, four thicknesses, an elastic foundation stiffness, 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. The element x-axis may be rotated by an angle THETA (in degrees).

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 Element Loading. Pressures may be input as surface loads on the element faces as shown by the circled numbers on Figure 63.1: SHELL63 Geometry. Positive pressures act into the element. Because shell edge pressures are input on a per-unit-length basis, per-unit-area quantities must be multiplied by the shell thickness. 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 63.1: SHELL63 Geometry. 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 (that is, 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).

Using the Allman stiffness will often enhance convergence behavior in large deflection (finite rotation) analyses of planar shell structures (that is, flat shells or flat regions of shells).

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.

KEYOPT(11) = 2 is used to store midsurface results in the results file for single or multi-layer shell elements. If you use SHELL,MID, you will see these calculated values, rather than the average of the TOP and BOTTOM results. You should use this option to access these correct midsurface results (membrane results) for those analyses where averaging TOP and BOTTOM results is inappropriate; examples include midsurface stresses and strains with nonlinear material behavior, and midsurface results after mode combinations that involve squaring operations such as in spectrum analyses.

A summary of the element input is given in "SHELL63 Input Summary". A general description of element input is given in Element Input.

SHELL63 Input Summary

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
See Table 63.1: SHELL63 Real Constants for a description of the real constants
Material Properties

EX, EY, EZ, (PRXY, PRYZ, PRXZ or NUXY, NUYZ, NUXZ), ALPX, ALPY, ALPZ (or CTEX, CTEY, CTEZ or THSX, THSY, THSZ), DENS, GXY, BETD, ALPD, DMPR

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)

Element stiffness:

0 -- 

Bending and membrane stiffness

1 -- 

Membrane stiffness only

2 -- 

Bending stiffness only

KEYOPT(2)

Stress stiffening option:

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 (that is, 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.)

KEYOPT(3)

Extra displacement shapes:

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).


Note:  For models with large rotation about the in-plane direction, KEYOPT(3) = 0 results in some transfer of moment directly to ground.


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 the Mechanical APDL Theory Reference.

KEYOPT(5)

Extra stress output:

0 -- 

Basic element printout

2 -- 

Nodal stress printout

KEYOPT(6)

Pressure loading:

0 -- 

Reduced pressure loading (must be used if KEYOPT(1) = 1)

2 -- 

Consistent pressure loading

KEYOPT(7)

Mass matrix:

0 -- 

Consistent mass matrix

1 -- 

Reduced mass matrix

KEYOPT(8)

Stress stiffness matrix:

0 -- 

"Nearly" consistent stress stiffness matrix (default)

1 -- 

Reduced stress stiffness matrix

KEYOPT(9)

Element coordinate system defined:

0 -- 

No user subroutine to define element coordinate system

4 -- 

Element x-axis located by user subroutine USERAN


Note:  See the Guide to User-Programmable Features for user written subroutines


KEYOPT(11)

Specify data storage:

0 -- 

Store data for TOP and BOTTOM surfaces only

2 -- 

Store data for TOP, BOTTOM, and MID surfaces

Table 63.1: SHELL63 Real Constants

No.NameDescription
1TK(I)Shell thickness at node I
2TK(J)Shell thickness at node J
3TK(K)Shell thickness at node K
4TK(L)Shell thickness at node L
5EFSElastic foundation stiffness
6THETAElement X-axis rotation
7RMIBending moment of inertia ratio
8CTOPDistance from mid surface to top
9CBOTDistance from mid surface to bottom
10, ..., 18(Blank)- -
19ADMSUAAdded mass/unit area

SHELL63 Output Data

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

Several items are illustrated in Figure 63.2: SHELL63 Stress Output. 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 are parallel to the element coordinate system. A general description of solution output is given in Solution Output. See the Basic Analysis Guide for ways to view results.

Figure 63.2: SHELL63 Stress Output

SHELL63 Stress Output

xIJ = Element x-axis if ESYS is not supplied.

x = Element x-axis if ESYS is supplied.


The Element Output Definitions table uses the following notation:

A colon (:) in the Name column indicates that 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 letter or number refers to a table footnote that describes when the item is conditionally available, and “-” indicates that the item is not available.

Table 63.2: SHELL63 Element Output Definitions

NameDefinitionOR
ELElement NumberYY
NODESNodes - I, J, K, LYY
MATMaterial numberYY
AREAAREAYY
XC, YC, ZCLocation where results are reportedY1
PRESPressures 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, LYY
TEMPTemperatures T1, T2, T3, T4, T5, T6, T7, T8YY
T(X, Y, XY)In-plane element X, Y, and XY forcesYY
M(X, Y, XY)Element X, Y, and XY momentsYY
FOUND.PRESSFoundation pressure (if nonzero)Y-
LOCTop, middle, or bottomYY
S:X, Y, Z, XYCombined membrane and bending stressesYY
S:1, 2, 3Principal stressYY
S:INTStress intensityYY
S:EQVEquivalent stressYY
EPEL:X, Y, Z, XYAverage elastic strainYY
EPEL:EQVEquivalent elastic strain [2]-Y
EPTH:X, Y, Z, XYAverage thermal strainYY
EPTH:EQVEquivalent thermal strain [2]-Y

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

  2. The equivalent strains use an effective Poisson's ratio: for elastic and thermal this value is set by the user (MP,PRXY).

Table 63.3: SHELL63 Miscellaneous Element Output

DescriptionNames of Items OutputOR
Nodal Stress Solution TEMP, S(X, Y, Z, XY), SINT, SEQV1-

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

Table 63.4: SHELL63 Item and Sequence Numbers lists output available through the ETABLE command using the Sequence Number method. See The General Postprocessor (POST1) in the Basic Analysis Guide and The Item and Sequence Number Table in this manual for more information. The following notation is used in Table 63.4: SHELL63 Item and Sequence Numbers:

Name

output quantity as defined in the Table 63.2: SHELL63 Element Output Definitions

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

Table 63.4: SHELL63 Item and Sequence Numbers

Output Quantity NameETABLE and ESOL Command Input
ItemEIJKL
TXSMISC1----
TYSMISC2----
TXYSMISC3----
MXSMISC4----
MYSMISC5----
MXYSMISC6----
P1SMISC-9101112
P2SMISC-13141516
P3SMISC-1817--
P4SMISC--2019-
P5SMISC---2221
P6SMISC-23--24
Top
S:1NMISC-161116
S:2NMISC-271217
S:3NMISC-381318
S:INTNMISC-491419
S:EQVNMISC-5101520
Bot
S:1NMISC-21263136
S:2NMISC-22273237
S:3NMISC-23283338
S:INTNMISC-24293439
S:EQVNMISC-25303540

SHELL63 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 and vary bilinearly over the shell surface.

  • An assemblage of flat shell elements can produce a good approximation of 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 Degenerated Shape Elements. 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.

  • For KEYOPT(1) = 0 or 2, the four nodes defining the element should lie as close as possible to a flat plane (for maximum accuracy), but a moderate amount of warping is permitted. For KEYOPT(1) = 1, the warping limit is very restrictive. In either case, an excessively warped element may produce a warning or error message. In the case of warping errors, triangular elements should be used (see Degenerated Shape Elements). Shell element warping is described in detail in Warping Factor in Mechanical APDL Theory Reference.

  • 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.

SHELL63 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 Professional  —  

  • The ALPD and BETD material properties are 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).