4.99 SHELL99 Linear Layered Structural Shell

4.99 SHELL99 Linear Layered Structural Shell (UP19980821 ) SHELL99 may be used for layered applications of a structural shell model. While SHELL99 does not have some of the nonlinear capabilities of SHELL91, it usually has a smaller element formulation time. SHELL99 allows up to 250 layers. If more than 250 layers are required, a user-input constitutive matrix is available.

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. See Section 14.99 of the ANSYS Theory Reference for more details about this element.

Figure 4.99-1 SHELL99 Linear Layered Structural Shell



4.99.1 Input Data

The geometry, node locations, and the coordinate system for this element are shown in Figure 4.99-1. The element is defined by eight nodes, average or corner layer thicknesses, layer material direction angles, and 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 more 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.

The following graph shows element formation and stress recovery time as a function of the number of layers. While SHELL91 uses less time for elements of under three layers, SHELL99 uses less time for elements with three or more layers.



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. ADMSUA is the added mass per unit area.

The input may be either in matrix form or layer form, depending upon KEYOPT(2). If matrix form, the matrices must be computed outside of the ANSYS program. See Section 14.99.3 of the ANSYS Theory Reference. Briefly, the force-strain and moment-curvature relationships defining the matrices for a linear variation of strain through the thickness (KEYOPT(2)=2) may be defined as:

where these terms are defined in Section 14.99.3 of the ANSYS Theory Reference. The submatrix [A] is input by real constants as:



Submatrices [B] and [D] are input similarly. Note that all submatrices are symmetric. {MT} and {BT} are for thermal effects. Real constants also include the element average density (AVDENS) and the element average thickness (THICK). As flat elements have been seen to give better results than curved elements for KEYOPT(2)=2, midside nodes are internally redefined for this case to be on a straight line connecting the corner nodes midway between the nodes for geometric computations. If KEYOPT(2)=3, quadratic effects are also included with matrices [E], [F], and {QT}, and midside nodes are not redefined. Section 4.99.3 provides a limitation on the use of matrix input. No stresses, thermal strains, or failure criteria are available with matrix input.

For non-matrix input, the element coordinate system orientation is as described in Section 2.3. The local coordinate system for each layer is defined as shown in Figure 4.99-2. The layer number (LN) can range from 1 to 250. In this local right-handed system, the x' axis is rotated an angle THETA(LN) (in degrees) from the element x axis toward the element y axis.

The total number of layers must be specified (NL). The properties of all layers should be entered (LSYM = 0). If the properties of the layers are symmetrical about the mid-thickness of the element (LSYM = 1), only half of properties of the layers, up to and including the middle layer (if any), need to be entered. While all layers may be printed, two layers may be specifically selected to be output (LP1 and LP2, with LP1 usually less than LP2).

The material properties of each layer may be orthotropic in the plane of the element. The real constant MAT is used to define the layer material number instead of the element material number applied with the MAT command. MAT defaults to 1 if not input. The material X direction corresponds to the local layer x' direction. Properties not input default as described in Section 2.4.

Use TREF and BETAD to supply global values for reference temperature and damping, respectively. Alternatively, use the MAT command to specify element-dependent values for reference temperature (MP,REFT) or damping (MP,DAMP); layer material numbers are ignored for this purpose.

Each layer of the laminated shell element may have a variable thickness (TK) by selecting KEYOPT(2)=1. The thickness is assumed to vary bilinearly over the area of the layer, with the thickness input at the corner node locations. If the layer has a constant thickness, only TK(I) need be input. If the thickness is not constant, all four corner 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.

You can specify the nodes to be at the top, middle or bottom surface of the element. The choice is made through the node offset option (KEYOPT(11)). This option is very convenient, for example, when modelling laminated structures with ply drop-off, where the location of the top or bottom surface may be better defined than the location of the midplane as shown in Figure 4.91-4.

You can also define two elements that share the same nodes, but with each element having a different setting of KEYOPT(11), as shown in Figure 4.91-5.

The failure criteria selection is input in the data table [TB], as described in Table 4.99-1a. Three predefined criteria are available and up to six user-defined criteria may be entered with user subroutines. See Section 14.99 of the ANSYS Theory Reference for an explanation of the three predefined failure criteria. See Guide to ANSYS User Programmable Features for an explanation of user subroutines.

Element loads are described in Section 2.7. Pressures may be input as surface loads on the element faces. The edge pressures act at the nodal plane as shown by circled numbers 3 through 6 on Figure 4.99-1. The mass matrix is also assumed to act at the nodal plane. Depending on KEYOPT(11), the nodal plane may be at the midsurface, or at the top or bottom surface. 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 4.99-1. 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.

A summary of the element input is given in Table 4.99-1. A general description of element input is given in Section 2.1.

Table 4.99-1 SHELL99 Input Summary

Element Name

SHELL99

Nodes

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

Degrees of Freedom

UX, UY, UZ, ROTX, ROTY, ROTZ

Real Constants

If KEYOPT(2) = 0, supply the following 12+(3*NL) constants:
NL, LSYM, LP1, LP2, EFS, ADMSUA,
(Blank), (Blank), (Blank), (Blank), (Blank), (Blank),
MAT, THETA, TK for layer 1, MAT, THETA, TK for layer 2, etc. up to layer NL

If KEYOPT(2) = 1, Supply the following 12+(6*NL) constants:
NL, LSYM, LP1, LP2, EFS, ADMSUA,
(Blank), (Blank), (Blank), (Blank), (Blank), (Blank),
MAT, THETA, TK(I), TK(J), TK(K), TK(L) for layer 1, etc. up to layer NL

If KEYOPT(2) = 2, supply the following 79 constants: A(21), B(21), D(21), MT(6), BT(6), AVDENS, THICK, EFS, ADMSUA

If KEYOPT(2) = 3, supply the following 127 constants:
A(21), B(21), D(21), E(21), F(21), MT(6), BT(6), QT(6), AVDENS, THICK, EFS, ADMSUA

Material Properties

If KEYOPT(2) = 0 or 1, supply the following 13*NM properties where NM is the number of materials (maximum is NL):
EX, EY, EZ, ALPX, ALPY, ALPZ, (PRXY, PRYZ, PRXZ or NUXY, NUYZ, NUXZ), DENS, GXY, GYZ, GXZ, for each of the NM materials.

If KEYOPT(2) = 2 or 3, supply none of the above.

Supply DAMP and REFT only once for the element (use MAT command to assign material property set). See the discussion in Section 4.99.1 for more details.

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 if KEYOPT(2) = 0 or 1, or
none if KEYOPT(2) = 2 or 3

Special Features

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

KEYOPT(2)

0 - Constant thickness layer input (250 layers maximum)
1 - Tapered layer input (125 layers maximum)
2 - Matrix input using linear logic
3 - Matrix input using quadratic logic

KEYOPT(3)

0 - Basic element printout
1 - Integration point strain printout
2 - Nodal force and moment printout in element coordinates
3 - Force and moment per unit length printout (available only if KEYOPT(2) = 0 or 1)
4 - Combination of all three options

KEYOPT(4)

0 - No user subroutines used to define element coordinate system
4 - Element x-axis located by user subroutine USERAN
5 - Element x-axis located by user subroutine USERAN and layer x-axes located by user subroutine USANLY (see the Guide to ANSYS User Programmable Features for user written subroutines)

KEYOPT(5)

Determines whether strains or stresses will be used with KEYOPT(6)
0 - Strain results will be used
1 - Stress results will be used
2 - Both strain and stress results will be used

KEYOPT(6)

Used for printout control. Note-no stresses, thermal strains, or failure criteria are available with matrix input.
0 - Basic element printout, as well as the summary of the maximum of all the failure criteria
1 - Same as 0 but also print the summary of all the failure criteria and the summary of the maximum of the interlaminar shear stress
2 - Same as 1 but also print the layer solution at the integration points in the bottom layer (or LP1) and the top layer (or LP2)
3 - Same as 1 but also print the layer solution at the element centroid for all layers, as well as the interlaminar shear stress solution between layers
4 - Same as 1 but also print the layer solution at the corner nodes for all layers, as well as the interlaminar shear stress solution between layers
5 - Same as 1 but also print the layer solution with the failure criterion values at the integration points for all layers, as well as the interlaminar shear stress solution between layers

KEYOPT(8)

0 - Store data for bottom of bottom layer (or LP1) and top of top layer (or LP2). Also store data for maximum failure criteria layer.
1 - Store data for all layers. Warning: Volume of data may be excessive.

KEYOPT(9)

Not available if KEYOPT(2) = 0 or 1 with NL = 1
0 - Evaluate strains and stresses at top and bottom of each layer
1 - Evaluate at mid-thickness of each layer

KEYOPT(10)

0 - No material property matrices printed
1 - Print material property matrices integrated through thickness for first element, if it is a SHELL99 element

KEYOPT(11)

0 - Nodes located at midsurface
1 - Nodes located at bottom surface
2 - Nodes located at top surface


The failure criteria table is started by using the TB command (with Lab=FAIL). The data table is input in two parts:

Data not input are assumed to be zero. See Section 14.99 of the ANSYS Theory Reference for an explanation of the predefined failure criteria. The six failure criterion keys are defined with the TBDATA command following a special form of the TBTEMP command [TBTEMP,,CRIT] to indicate that the failure criterion keys are defined next. The constants (C1-C6) entered on the TBDATA command are:

Table 4.99-1a SHELL99 Orthotropic Material Failure Criteria Data

Constant

Meaning

1 Maximum Strain Failure Criterion - Output as FC1 (uses strain constants 1-9)
0 - Do not include this predefined criterion.
1 - Include this predefined criterion.
-1 - Include user-defined criterion with subroutine USRFC1.

2 Maximum Stress Failure Criterion - Output as FC2 (uses stress constants 10-18)

Options are the same as for constant 1, except subroutine is USRFC2.

3 Tsai-Wu Failure Criterion - Output as FC3 (uses constants 10-21)
0 - Do not include this predefined criterion
1 - Include the Tsai-Wu strength index
2 - Include the inverse of the Tsai-Wu strength ratio
-1 - Include user-defined criterion with subroutine USRFC3

4-6 User-defined Failure Criteria - Output as FC4 TO FC6
0 - Do not include this criterion.
-1 - Include user-defined criteria with subroutines
USRFC4, USRFC5, USRFC6, respectively.

The failure data, which may be temperature-dependent, must be defined with the TBDATA command following a temperature definition on the TBTEMP command. Strains must have absolute values less than 1.0. Up to six temperatures (NTEMP=6 maximum on the TB command) may be defined with the TBTEMP commands. The constants (C1-C21) entered on the TBDATA command (6 per command), after each TBTEMP command, are:

Table 4.99-1b TBDATA Constants for the TBTEMP Command

Constant - (Symbol) - Meaning
1
- () - Failure strain in material x-direction in tension (must be positive).
2 - () - Failure strain in material x-direction in compression (default = -) (may not be positive).
3 - () - Failure strain in material y-direction in tension (must be positive).
4 - () - Failure strain in material y-direction in compression (default = -) (may not be positive).
5 - ( ) - Failure strain in material z-direction in tension (must be positive).
6 - () - Failure strain in material z-direction in compression (default = -) (may not be positive).
7 - () - Failure strain in material x-y plane (shear) (must be positive).
8 - (

) - Failure strain in material y-z plane (shear) (default = ).
9 - () - Failure strain in material x-z plane (shear) (default = ).
10 - () - Failure stress in material x-direction in tension (must be positive).
11 - () - Failure stress in material x-direction in compression (default = -) (may not be positive).
12 - () - Failure stress in material y-direction in tension (must be positive).
13 - () - Failure stress in material y-direction in compression (default = -) (may not be positive).
14 - () - Failure stress in material z-direction in tension (must be positive).
15 - () - Failure stress in material z-direction in compression (default = -) (may not be positive).
16 - () - Failure stress in material x-y plane (shear) (must be positive).
17 - () - Failure stress in material y-z plane (shear) (default = ).
18 - () - Failure stress in material x-z plane (shear) (default = ).
19 - () - x-y coupling coefficient for Tsai-Wu Theory (default =-1.0).
20 - () - y-z coupling coefficient for Tsai-Wu Theory (default = -1.0).
21 - () - x-z coupling coefficient for Tsai-Wu Theory (default =-1.0).

Note-Tsai-Wu coupling coefficients must be between -2.0 and 2.0. Values between -1.0 and 0.0 are recommended. For 2-D analysis, set , , , and to a value several orders of magnitude larger than , , or ; and set Cxz and Cyz to zero.


4.99.2 Output Data

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

Several items are illustrated in Figure 4.99-2. The element stress directions correspond to the layer local coordinate directions.

Various layer printout options are available. For integration point output, integration point 1 is nearest node I, 2 nearest J, 3 nearest K, and 4 nearest L. Failure criterion output is evaluated only at the in-plane integration points. (See Section 14.99 of the ANSYS Theory Reference). After the layer printout, the in-plane forces and moments are listed for the entire element if KEYOPT(3)=3 or 4. These are shown in Figure 4.99-2. The moments include the moment about the x-face (MX), the moment about the y-face (MY), and the twisting moment (MXY). The forces and moments are calculated per unit length in the element coordinate system and are the combined sum for all layers. If KEYOPT(3) = 2 or 4 for this element, the 6 member forces and moments are also printed for each node (in the element coordinate system). KEYOPT(8) controls the amount of data output on the postdata file for processing with the LAYER or LAYERP26 command. 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 4.99-2 SHELL99 Stress Output

The following notation is used in Table 4.99-2:

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 4.99-2 SHELL99 Element Output Definitions

Name

Definition

O

R

EL

Element number

Y Y
NODES

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

Y Y
VOLU:

Volume

Y Y
TTOP, TBOT

Average temperatures at top and bottom faces

Y Y
CENT: X, Y, Z

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

1 1
INT

Integration point number

2 -
POS

Top (TOP), Bottom (BOT), Mid-thickness (MID) of element

2 -
XI, YI, ZI

Global X,Y,Z location of integration point

2 -
EPTO: X, Y, Z, XY, YZ, XZ

Total strains (no thermal strain adjustment) in element coordinates

2 2
NUMBER

Layer number

3 -
MAT

Material number of this layer

3 -
THETA

Material direction angle for layer (THETA)

3 -
AVE THICK

Average thickness of layer

3 -
ACC AVE THICK

Accumulative average thickness (thickness of element from layer 1 to this layer)

3 -
AVE TEMP

Average temperature of layer

3 -
POS

Top (TOP), Bottom (BOT), Mid-thickness (MID) of layer
(see KEYOPT(9) for control options)

3 -
LOC

Center location (avg) (if KEYOPT(6)=3)

3 -
NODE

Corner node number (if KEYOPT(6)=4)

3 -
INT

Integration point number (if KEYOPT(6)=2 or 5)

3 -
EPEL: X, Y, Z, XY, YZ, XZ

Elastic strains (in layer local coordinates)

4 -
S: X, Y, Z,
XY, YZ, XZ

Stresses (in layer local coordinates)

4 -
FC1,...,FC6,
FCMAX

Failure criterion values and maximum at each integration point, output only if KEYOPT(6)=5

4 -
FC

Failure criterion number (FC1 to FC6, FCMAX)

5 Y
VALUE

Maximum value for this criterion (if value exceeds 9999.999, 9999.999 will be output)

5 Y
LN

Layer number where maximum occurs

5 Y
EPELF (X, Y, Z, XY, YZ, XZ)

Elastic strains (in layer local coordinates) causing the maximum value for this criterion in the element.

5 Y
SF (X, Y, Z, XY, YZ, XZ)

Stresses (in layer local coordinates) causing the maximum value for this criterion in the element.

5 Y
LAYERS

Interface location

6 6
ILSXZ

Interlaminar SXZ shear stress

6 6
ILSYZ

Interlaminar SYZ shear stress

6 6
ILANG

Angle of shear stress vector (measured from the element x axis toward the element y axis in degrees)

6 6
ILSUM

Shear stress vector sum

6 6
LN1, LN2

Layer numbers which define location of maximum interlaminar shear stress (ILMAX)

7 Y
ILMAX

Maximum interlaminar shear stress (occurs between LN1 and LN2)

7 Y
T(X, Y, XY)

Element total in-plane forces per unit length (in element coordinates)

8 8
N(X, Y)

Out-of-plane element X and Y shear forces

8 8
M(X, Y, XY)

Element total moments per unit length (in element coordinates)

9 9
MFOR(X, Y, Z)

Member forces for each node in the element coordinate system

10 -
MMOM(X, Y, Z)

Member moments for each node in the element coordinate system

10 -
1. If KEYOPT(2)=0 or 1

2. Integration point strain solution (if KEYOPT(3)=1 or 4)

3. Layer solution (if KEYOPT(2)=0 or 1 and KEYOPT(6)>1)

4. The item output is controlled with KEYOPT(5)

5. Summary of failure criteria calculation (only if KEYOPT(2)=0 or 1).
If KEYOPT(6)=0, only maximum of all failure criteria (FCMAX) in element is output.
Output of the elastic strains and/or stresses (depending on KEYOPT(5)) for each failure criterion and the maximum of all criteria (FCMAX).

6. Interlaminar stress solution (if KEYOPT(2)=0 or 1 and KEYOPT(6)>2)

7. Printed only if KEYOPT(2)=0 or 1, and KEYOPT(6)#0

8. Output at the corner nodes only if KEYOPT(2)=0 or 1, and KEYOPT(3)=3 or 4

9. Output at the corner nodes only if KEYOPT(2)=0 or 1, KEYOPT(3)=3 or 4, and KEYOPT(9) # 1

10. Output only if KEYOPT(3)=2 or 4

Table 4.99-3 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 4.99-3:

Table 4.99-3 SHELL99 Item and Sequence Numbers for the ETABLE and ESOL Commands

Name

Item

Bottom of Layer i

Top of Layer NL

ILSXZ

SMISC

(2*i)+7 (2*NL)+9
ILSYZ

SMISC

(2*i)+8 (2*NL)+10
ILSUM

NMISC

(2*i)+5 (2*NL)+7
ILANG

NMISC

(2*i)+6 (2*NL)+8
Name

Item

I

J

K

L

P1

SMISC

(2*NL)+11 (2*NL)+12 (2*NL)+13 (2*NL)+14
P2

SMISC

(2*NL)+15 (2*NL)+16 (2*NL)+17 (2*NL)+18
P3

SMISC

(2*NL)+20 (2*NL)+19
P4

SMISC

(2*NL)+22 (2*NL)+21
P5

SMISC

(2*NL)+24 (2*NL)+23
P6

SMISC

(2*NL)+25 (2*NL)+26
Name

Item

E

TX

SMISC

1
TY

SMISC

2
TXY

SMISC

3
MX

SMISC

4
MY

SMISC

5
MXY

SMISC

6
NX

SMISC

7
NY

SMISC

8
FCMAX (over all layers)

NMISC

1
VALUE

NMISC

2
LN

NMISC

3
ILMAX

NMISC

4
LN1

NMISC

5
LN2

NMISC

6
FCMAX (at layer i)

NMISC

2*(NL+i)+7
VALUE (at layer i)

NMISC

2*(NL+i)+8
FC

NMISC

4*NL+8+15(N-1)+1
VALUE

NMISC

4*NL+8+15(N-1)+2
LN

NMISC

4*NL+8+15(N-1)+3
EPELFX

NMISC

4*NL+8+15(N-1)+4
EPELFY

NMISC

4*NL+8+15(N-1)+5
EPELFZ

NMISC

4*NL+8+15(N-1)+6
EPELFXY

NMISC

4*NL+8+15(N-1)+7
EPELFYZ

NMISC

4*NL+8+15(N-1)+8
EPELFXZ

NMISC

4*NL+8+15(N-1)+9
SFX

NMISC

4*NL+8+15(N-1)+10
SFY

NMISC

4*NL+8+15(N-1)+11
SFZ

NMISC

4*NL+8+15(N-1)+12
SFXY

NMISC

4*NL+8+15(N-1)+13
SFYZ

NMISC

4*NL+8+15(N-1)+14
SFXZ

NMISC

4*NL+8+15(N-1)+15
Note-The i in Table 4.99-3 (where i= 1, 2, 3 ..., NL) refers to the layer number of the shell. NL is the maximum layer number as input for real constant NL (1 <= NL <= 250). N refers to the failure criterion number: N=1 for the first failure criterion, N=2 for the second failure criterion, and so on.

4.99.3 Assumptions and Restrictions

Zero area elements are not allowed. This occurs most often whenever the elements are not numbered properly. Zero thickness layers or layers tapering down to a zero thickness at any corner are not allowed. If KEYOPT(11) = 0, all nodes are assumed to be at the mid-thickness of the element. The offset effect of the layers from the node is automatically included. No slippage is assumed between the element layers. Shear deflections are included in the element, however, normals to the center plane before deformation are assumed to remain straight after deformation. This element may produce inaccurate stress under thermal loads for doubly curved or warped domains.

The applied transverse thermal gradient is assumed to be linear through the element and over the element surface. The stress varies linearly through the thickness of each layer. Interlaminar transverse shear stresses are based on the assumption that no shear is carried at the top and bottom surfaces of an element. Further, these interlaminar shear stresses are only computed at the centroid and are not valid along the element boundaries. If accurate edge interlaminar shear stresses are required, shell-to-solid submodeling should be used. The element matrices are reformed every iteration unless option 1 of the KUSE command is active. Only the lumped mass matrix is available. The mass matrix is assumed to act at the nodal plane.

The large deflection option for SHELL99 is not as convergent as it is for SHELL91 (the nonlinear layered shell element). SHELL91 may be the preferred element type when constructing models that include large deflection

If you have defined the element using the node offset option (KEYOPT(11) 0), be aware of the following:

4.99.4 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