Ansys Shell 63 Elementansys Shell 63 Elementansys Shell 63 Element

SHELL63

http://www.et.byu.edu/docs/ansys/ansys8.0/Hlp_E_SHELL63.html

SHELL63

Element Reference> Part I. Element Library>

SHELL63 Elastic Shell MP ME ST <> <> PR <> <> <> PP ED

SHELL63 Element Description 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 in the ANSYS, Inc. Theory Reference for more details about this element. Similar elements are SHELL43 and SHELL181 (plastic capability), and SHELL93 (midside node capability). The ETCHG command converts SHELL57 and SHELL157 elements to SHELL63. Figure 63.1 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).

1 of 10

12/6/07 11:29 PM

SHELL63

http://www.et.byu.edu/docs/ansys/ansys8.0/Hlp_E_SHELL63.html

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 Node and Element Loads. 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. 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 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.

2 of 10

12/6/07 11:29 PM

SHELL63

http://www.et.byu.edu/docs/ansys/ansys8.0/Hlp_E_SHELL63.html

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, 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) Element stiffness:

3 of 10

12/6/07 11:29 PM

SHELL63

http://www.et.byu.edu/docs/ansys/ansys8.0/Hlp_E_SHELL63.html

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.) Note that if SOLCONTROL is ON and NLGEOM is ON, KEYOPT(2) is automatically set to 1; that is, the consistent tangent will be used. 2 -Use to turn off consistent tangent stiffness matrix (i.e., a matrix composed of the main tangent stiffness matrix plus the consistent stress stiffness matrix) when SOLCONTROL is ON. Sometimes it is necessary to turn off the consistent tangent stiffness matrix if the element is used to simulate rigid bodies by using a very large real constant number . KEYOPT(2) = 2 is the same as KEYOPT(2) = 0, however, KEYOPT(2) = 0 is controlled by SOLCONTROL, ON or OFF, while KEYOPT(2) = 2 is independent of SOLCONTROL. 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 --

4 of 10

12/6/07 11:29 PM

SHELL63

http://www.et.byu.edu/docs/ansys/ansys8.0/Hlp_E_SHELL63.html

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 ANSYS, Inc. 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)

5 of 10

12/6/07 11:29 PM

SHELL63

http://www.et.byu.edu/docs/ansys/ansys8.0/Hlp_E_SHELL63.html

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 ANSYS 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.

Name

Description

1

TK(I)

Shell thickness at node I

2

TK(J)

Shell thickness at node J

3

TK(K)

Shell thickness at node K

4

TK(L)

Shell thickness at node L

5

EFS

Elastic foundation stiffness

6

THETA

Element X-axis rotation

7

RMI

Bending moment of inertia ratio

8

CTOP

Distance from mid surface to top

9

CBOT

Distance from mid surface to bottom

10, ..., 18

(Blank)

--

19

ADMSUA

Added mass/unit area

SHELL63 Output Data The solution output associated with the element is in two forms: Nodal displacements included in the overall nodal solution

6 of 10

12/6/07 11:29 PM

SHELL63

http://www.et.byu.edu/docs/ansys/ansys8.0/Hlp_E_SHELL63.html

Additional element output as shown in Table 63.2: "SHELL63 Element Output Definitions" 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 ANSYS Basic Analysis Guide for ways to view results. Figure 63.2 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 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 number refers to a table footnote that describes when the item is conditionally available, and a - indicates that the item is not available. Table 63.2 SHELL63 Element Output Definitions Name

7 of 10

Definition

O

R

EL

Element Number

Y

Y

NODES

Nodes - I, J, K, L

Y

Y

MAT

Material number

Y

Y

12/6/07 11:29 PM

SHELL63

http://www.et.byu.edu/docs/ansys/ansys8.0/Hlp_E_SHELL63.html

Name

Definition

O

R

Y

Y

AREA

AREA

XC, YC, ZC

Location where results are reported

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 stress

Y

Y

S:INT

Stress intensity

Y

Y

S:EQV

Equivalent stress

Y

Y

EPEL:X, Y, Z, XY

Average elastic strain

Y

Y

EPEL:EQV

Equivalent elastic strain [2]

-

Y

EPTH:X, Y, Z, XY

Average thermal strain

Y

Y

EPTH:EQV

Equivalent thermal strain [2]

-

Y

Y

1

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 Description Nodal Stress Solution

Names of Items Output TEMP, S(X, Y, Z, XY), SINT, SEQV

O

R

1

-

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 ANSYS 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

8 of 10

12/6/07 11:29 PM

SHELL63

http://www.et.byu.edu/docs/ansys/ansys8.0/Hlp_E_SHELL63.html

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 Name

ETABLE and ESOL Command Input 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

-

-

P5

SMISC

-

-

P6

SMISC

-

23

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

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

-

20

-

19 -

-

22

-

21 -

24

Top

Bot

SHELL63 Assumptions and Restrictions

9 of 10

12/6/07 11:29 PM

SHELL63

http://www.et.byu.edu/docs/ansys/ansys8.0/Hlp_E_SHELL63.html

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 Triangle, Prism and Tetrahedral 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 Triangle, Prism and Tetrahedral Elements). Shell element warping tests are described in detail in tables of Applicability of Warping Tests and Warping Factor Limits in the ANSYS, Inc. 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 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).

10 of 10

12/6/07 11:29 PM