The element has variable thickness, stress stiffening, large deflection, and a cloth option. See Section 14.41 of the ANSYS Theory Reference for more details about this element. Another element having "membrane only" capability as an option is SHELL63.
Figure 4.41-1 SHELL41 Membrane Shell
The element may have variable thickness. 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. 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 4.41-1. Positive pressures act into the element. Edge pressures are input as force per unit length. The pressure loading is converted to equivalent element loads applied at the nodes. Temperatures may be input as element body loads at the nodes. The node I temperature T(I) defaults to TUNIF. If all other temperatures are unspecified, they default to T(I). For any other input pattern, unspecified temperatures default to TUNIF.
A nonlinear option may be selected with KEYOPT(1). This "cloth" option allows the element to wrinkle when it goes into compression. Wrinkling may be in one (or both) orthogonal directions.
Any out-of-planeness within the element or roundoff error in nodal location may cause an instability in the displacement solution. To counteract this, a slight normal stiffness may be added to the element with the EFS real constant. KEYOPT(2) is used to include or suppress the extra displacement shapes. KEYOPT(4) provides various element printout options (see Section 2.2.2).
A summary of the element input is given in Table 4.41-1. A general description of element input is given in Section 2.1.
Table 4.41-1 SHELL41 Input Summary
| Element Name
|
SHELL41
|
| Nodes
|
I, J, K, L
|
| Degrees of Freedom
|
UX, UY, UZ
|
| Real Constants
|
TK ( I ), TK ( J ), TK ( K ), TK ( L ), THETA, EFS, ADMSUA (where TK ( J ), TK ( K ), TK ( L ) default to TK ( I ))
|
| Material Properties
|
EX, EY, PRXY or NUXY, ALPX, ALPY, DENS, GXY, DAMP
(X-direction defined by THETA real constant)
|
| 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: T ( I ), T ( J ), T ( K ), T ( L )
|
| Special Features
|
Stress Stiffening, Large Deflection, Nonlinear (if KEYOPT(1) = 2),
Birth and death, Adaptive descent
|
| KEYOPT(1)
|
0 - Stiffness acts in both tension and compression 2 - Stiffness acts in tension, collapses in compression ("cloth" option)
|
| KEYOPT(2)
|
0 - Include extra displacement shapes 1 - Suppress extra displacement shape
|
| KEYOPT(4)
|
0 - Basic element printout 1 - Repeat basic printout at integration points 2 - Nodal stress printout
|
| KEYOPT(5)
|
0 - No member force printout 1 - Print member forces in the element coordinate system
|
| KEYOPT(6)
|
0 - No edge printout 1 - Edge printout for mid-point of side I-J 2 - Edge printout for mid-points of both sides I-J and K-L Note-Edge printout valid only for isotropic materials
|
Figure 4.41-2 SHELL41 Stress Output
The following notation is used in Table 4.41-2:
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 4.41-2 SHELL41 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
|
Surface area
|
Y | Y |
| CENT: X, Y, Z
|
Global location XC, YC, ZC
|
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 T(I), T(J), T(K), T(L)
|
Y | Y |
| S: X, Y, Z, XY
|
Stresses
|
Y | Y |
| S: 1, 2, 3
|
Principal stresses
|
Y | Y |
| S:INT
|
Stress intensity
|
Y | Y |
| S:EQV
|
Equivalent stress
|
Y | Y |
| ANGLES
|
Diagonal tension angles (degrees) between element
x-axis and tensile stress directions
|
1 | 1 |
| CURRENT STATS.
|
Element statuses at end of this time step
|
2 | 2 |
| OLD STATUSES
|
Element statuses at end of previous time step
|
2 | 2 |
| TEMP
|
Edge average temperature
|
3 | 3 |
| EPEL(PAR,PER,Z)
|
Edge elastic strains (parallel, perpendicular, Z)
|
3 | 3 |
| S(PAR,PER,Z)
|
Edge stresses (parallel, perpendicular, Z)
|
3 | 3 |
| SINT
|
Edge stress intensity
|
3 | 3 |
| SEQV
|
Edge equivalent stress
|
3 | 3 |
| FX, FY, FZ
|
Nodal forces
|
- | Y |
2. Output at the integration points only if KEYOPT(1)=2. The element status is given by the
following values:
0 - Tension in both (orthogonal) directions
1 - Tension in one direction, collapse in other direction
2 - Collapse in both directions
3. Edge I-J output, if KEYOPT(6) is greater than zero.
Table 4.41-2a SHELL41 Miscellaneous Element Output
| Description
|
Names of Items Output
|
O
|
R
|
| Integration Point Stress Solution
|
TEMP, S(X, Y, Z, XY), SINT, SEQV
|
1 | - |
| Nodal Stress Solution
|
TEMP, S(X, Y, Z, XY), SINT, SEQV
|
2 | - |
| Edge K-L
|
TEMP, EPEL(PAR, PER, Z), S(PAR, PER, Z), SINT, SEQV
|
3 | - |
| Member Forces
|
FX, FY, FZ
|
4 | - |
2. Output at each node, if KEYOPT(4)=2
3. Output if KEYOPT(6)=2
4. Output at each node (in the element coordinate system) if KEYOPT(5)=1
Table 4.41-3 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 4.41-3:
| Name
|
Item
|
I
|
J
|
K
|
L
|
| FX
|
SMISC
|
1 | 4 | 7 | 10 |
| FY
|
SMISC
|
2 | 5 | 8 | 11 |
| FZ
|
SMISC
|
3 | 6 | 9 | 12 |
| P1
|
SMISC
|
13 | 14 | 15 | 16 |
| P2
|
SMISC
|
17 | 18 | 19 | 20 |
| P3
|
SMISC
|
22 | 21 | - | - |
| P4
|
SMISC
|
- | 24 | 23 | - |
| P5
|
SMISC
|
- | - | 26 | 25 |
| P6
|
SMISC
|
27 | - | - | 28 |
| 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 |
|
|
|
Corner Location
|
|||
| 1
|
2
|
3
|
4
|
||
| ANGLE
|
NMISC
|
21 | 23 | 25 | 27 |
| STAT
|
NMISC
|
22 | 24 | 26 | 28 |
A triangular element may be formed by defining duplicate K and L node numbers (see Section 2.8). The extra shapes are automatically deleted for triangular elements so that a constant strain element results. The triangular shape is required for large deflection analyses since a four-node element may warp during deflection. Edge stress printout is valid only if the conditions described in Section 2.2.2 are met.
Modeling hints: An assembly of SHELL41 elements describing a flat plane should be exactly flat; otherwise singularities may develop in the direction perpendicular to the plane. Very weak spar elements (LINK8) tied to the nodes in the plane and to a common ground point may be added to provide a small normal stiffness, or the EFS real constant may be used to counteract the singularity problem. Also, stress stiffening will help stabilize the solution after the first substep if the membrane element is in a tension field. An assemblage of flat elements can produce an approximation to a curved surface, but each flat element should not extend over more than a 15° arc.