This element is used in explicit dynamic analyses only. Refer to the LS-DYNA Theoretical Manual for more information.
Figure 4.163-1 SHELL163 Explicit Thin Structural Shell
ESOP is the option for the spacing of integration points, and can be either 0 or 1. ESOP is used only if KEYOPT(4)>0. If you set ESOP=0, you must define real constants S(i), and WF(i) to define the integration point locations. If KEYOPT(3)=1, then you must also define BETA(i) and MAT(i) for each integration point. Set ESOP=1 if the integration points are equally spaced through the thickness such that the shell is subdivided into NIP layers of equal thickness (up to 100 layers).
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.
If you set ESOP=0 and define the integration points using S(i), and WF(i), and possibly BETA(i) and MAT(i), note the following:
); see Figure 4.163-2. If using these real constants
to define integration points, then S(i) and WF(i) must both be specified for each
integration point (maximum of 100). BETA(i) is the material angle (in degrees)
at the i-th integration point and must be specified for each integration point.
The material model (i.e., BKIN, MKIN, MISO, etc.) is not allowed to change
within an element, although the material properties (i.e., EX, NUXY, etc.), as
defined per MAT(i), can change. However, the density may not vary through
the thickness of the shell element. If more than one material is used, and the
densities vary between materials, the density of the material of the first layer will
be used for the entire element.
If KEYOPT(4)=0, the integration rule is defined by KEYOPT(2). The Gauss rule (KEYOPT(2)=0) is valid for up to five layers (integration points). The trapezoidal rule (KEYOPT(2)=1) allows up to 100 layers, but is not recommended for less than 20 layers, especially if bending is involved.
Figure 4.163-2 In the user defined shell integration rule, the ordering of the integration points is arbitrary.
Use the EDLOAD command to apply nodal loads and other load types described below. For detailed information on how to apply loads in an explicit dynamic analysis, see Chapter 4 of the ANSYS/LS-DYNA User's Guide.
Pressures can be input as surface loads on the element midsurfaces. Positive normal pressures act into the element (i.e., positive pressure acts in the negative z direction). Note, however, that pressure is actually applied to the midsurface. See Figure 4.163-3
Figure 4.163-3 Nodal numbering for pressure loads. Positive pressure acts in the negative z-direction
Base accelerations and angular velocities in the x, y, and z directions can be applied at the nodes using the EDLOAD command. To apply these loads, you need to first select the nodes and create a component. The load is then applied to that component. Each node in the component will have the specified load.
You can also use the EDLOAD command to apply loads (displacements, forces, etc.) on rigid bodies.
For this element, you can choose from the following materials:
KEYOPT(1) allows you to specify 1 of 11 element formulations for SHELL163 (see Input Summary, below). A brief description about each element formulation follows:
The Hughes-Liu element formulation (KEYOPT(1)=1) is based on a degenerated continuum formulation. This formulation results in substantially large computational costs, but it is effective when very large deformations are expected. This formulation treats warped configurations accurately but does not pass the patch test. It uses one-point quadrature with the same hourglass control as the Belytschko-Tsay.
The Belytschko-Tsay (default) element formulation (KEYOPT(1)=0 or 2) is the fastest of the explicit dynamics shells. It is based on the Mindlin-Reissner assumption, so transverse shear is included. It does not treat warped configurations accurately, so it should not be used in coarse mesh models. One-point quadrature is used with hourglass control. A default value is set for the hourglass parameter. When hourglassing appears, you should increase this parameter to avoid hourglassing. It does not pass the patch test.
The BCIZ Triangular Shell element formulation (KEYOPT(1)=3) is based on a Kirhhoff plate theory and uses cubic velocity fields. Three sets of quadrature points are used in each element, so it is relatively slow. It passes the patch test only when the mesh is generated from three sets of parallel lines.
The C0 Triangular Shell element formulation (KEYOPT(1)=4) is based on a Mindlin-Reissner plate theory and uses linear velocity fields. One quadrature point is used in the element formulation. This formulation is rather stiff, so it should not be used for constructing an entire mesh, only to transition between meshes.
The Belytschko-Tsay membrane element formulation (KEYOPT(1)=5) is the same as the Belytschko-Tsay but with no bending stiffness.
The S/R Hughes-Liu element formulation (KEYOPT(1)=6) is the same as the Hughes-Liu, but instead of using one-point quadrature with hourglass control, this formulation uses selective reduced integration. This increases the cost by a factor of 3 to 4, but avoids certain hourglass modes; certain bending hourglass modes are still possible.
The S/R co-rotational Hughes-Liu element formulation (KEYOPT(1)=7) is the same as the S/R Hughes-Liu except it uses the co-rotational system.
The Belytschko-Leviathan shell formulation (KEYOPT(1)=8) is similar to the Belytschko-Wong- Chiang with one-point quadrature but it uses physical hourglass control, thus no user-set hourglass control parameters need to be set.
The fully-integrated Belytschko-Tsay membrane element formulation (KEYOPT(1)=9) is the same as the Belytschko-Tsay membrane except is uses a 2x2 quadrature instead of a one-point quadrature. This formulation is more robust for warped configurations.
The Belytschko-Wong-Chiang formulation (KEYOPT(1)=10) is the same as the Belytschko-Tsay except the shortcomings in warped configuration are avoided. Costs about 10% more.
The fast (co-rotational) Hughes-Liu formulation (KEYOPT(1)=11) is the same as the Hughes-Liu except this formulation uses the co-rotational system.
Of the eleven shell element formulations, only KEYOPT(1)=2, 8, and 10 are valid for an explicit-to-implicit sequential solution. For metal forming analyses, KEYOPT(1)=10 is recommended in order to properly account for warping.
A summary of the element input is given in Table 4.163-1. A general description of element input is given in Section 2.1.
Table 4.163-1 SHELL163 Input Summary
| Element Name
|
SHELL163
|
| Nodes
|
I, J, K, L
|
| Degrees of Freedom
|
UX, UY, UZ, VX, VY, VZ, AX, AY, AZ, ROTX, ROTY, ROTZ Note-For explicit dynamics analyses, V (X, Y, Z) refers to nodal velocity, and A (X, Y, Z) refers to nodal acceleration. Although V (X, Y, Z) and A (X, Y, Z) appear as DOFs, they are not actually physical DOFs. However, these quantities are computed as DOF solutions and stored for post-processing.
|
| Real Constants
|
SHRF, NIP, T1, T2, T3, T4, NLOC, ESOP, BETA(i), S(i), WF(i), MAT(i) (Specify NLOC only if KEYOPT(1)=1, 6, 7, or 11) (See Table 4.163-1a).
|
| Material Properties
|
EX, EY, EZ, NUXY, NUYZ, NUXZ, PRXY, PRXZ, PRYZ, GXY, GYZ, GXZ, DENS, DAMP (MP command) RIGID,HGLS (except KEYOPT(1)=3, 4), ORTHO (EDMP command) PLAW, BKIN, BISO, COMPOSITE, MOONEY, EOS (TB command; see Section 2.6)
|
| Surface Loads
|
Pressure (applied on midsurface)
|
| Body Loads
|
None
|
| Special Features
|
This element supports all nonlinear features allowed for an explicit dynamics analysis.
|
| KEYOPT(1)
|
Element formulation 1 -Hughes-Liu 0, 2 - Belytschko-Tsay (default) 3 - BCIZ triangular shell 4 - C0 triangular shell 5 - Belytschko-Tsay membrane 6 - S/R Hughes-Liu 7 - S/R co-rotational Hughes-Liu 8 - Belytschko-Levithan shell 9 - Fully integrated Belytschko-Tsay membrane 10 - Belytschko-Wong-Chiang 11 - Fast (co-rotational) Hughes-Liu
|
| KEYOPT(2)
|
Used for standard integration rules (KEYOPT(4)=0) 0 - Gauss rule (up to five integration points are permitted) 1 - Trapezoidal rule (up to 100 integration points are permitted)
|
| KEYOPT(3)
|
Flag for layered composite material mode 0 - Non-composite material mode 1 - Composite material mode; a material angle is defined for each through thickness integration point
|
| KEYOPT(4)
|
0 - Standard integration option n - User-defined integration rule ID (valid range: 1 to 9999; if selected, it overrides the integration rule set by KEYOPT(2))
|
| No.
|
Name
|
Description
|
| 1 | SHRF
|
Shear factor Suggested value: 5/6; if left blank, defaults to 1
|
| 2 | NIP
|
Number of integration points If input as 0 or blank, defaults to 2.
|
| 3 | T1
|
Shell thickness at node I
|
| 4 | T2
|
Shell thickness at node J
|
| 5 | T3
|
Shell thickness at node K
|
| 6 | T4
|
Shell thickness at node L
|
| 7 | NLOC
|
Location of reference surface = 1 top surface = 0 middle surface = -1 bottom surface If keyopt (1) = 1, 6, 7, or 11 only
|
| 8 | ESOP
|
Option for the spacing of integration points: 0 - Integration points are defined using real constants S(i) and WF(i). 1 - Integration points are equally spaced through the thickness such that the shell is subdivided into NIP layers of equal thickness.
|
| 9... 405 |
BETA(i)
|
Material angle at the i-th integration point.1
|
| 10... 406 |
S(i)
|
Coordinate of integration point in the range -1 to 1. i = 1, NIP (NIP = 100 max)1
|
| 11... 407 |
WF(i)
|
Weighting factor; i.e., the thickness associated with the integration
point divided by the actual shell thickness. i = 1, NIP (NIP = 100 max)1
|
| 12... 408 |
MAT(i)
|
Material ID for each layer.1
|
Stress data is always output from the bottom of the shell to the top. See Figure 4.163-2.
In all cases (default and otherwise), strain is always output for two layers only: Layer 1=bottom and layer 2=top.
The number of integration points specified by real constant NIP controls the output locations. If NIP=SHELLIP, then each layer corresponds to an integration point, and those are the locations where you will get output data. If NIP>SHELLIP, then data is output only at the SHELLIP number of locations (first bottom layer, then layers 2 through n moving up from the bottom). If NIP<SHELLIP (but NIP>2), then results are output only for NIP number of layers.
By default, the number of integration points (NIP) is 2, and the number of output locations/layers (SHELLIP) is 3. In this case, stress data is output in the following order: Layer 1=bottom, layer 2=middle, and layer 3=top. When SHELLIP=3, the middle layer will be an interpolated value if NIP is an even number or an actual value at an integration point if NIP is an odd number.
If NIP=1, the integration point is at the element midplane, and only one stress and one strain value are output.
For all formulations associated with SHELL163, strains (EPTO) and generalized stresses (M, T, N) are output in the element coordinate system, and stresses (S) are output in the global Cartesian system, except for the Hughes-Liu formulation. Strain output (EPTO) for the Hughes-Liu formulation (KEYOPT(1)=1) is output in the global Cartesian system. RSYS has no effect in post-processing LS-DYNA output.
The following notation is used in Table 4.163-2:
A colon (:) in the Name column indicates the item can be accessed by the Component Name method [ETABLE, ESOL] (see Section 2.2.2). These items are available in the results file.
Table 4.163-2 SHELL163 Element Output Definitions
| Name
|
Definition
|
| S(X, Y, Z, XY, YZ, XZ)
|
Stresses
|
| EPTO (X, Y, Z, XY, YZ, XZ)
|
Total strain
|
| M(X, Y, XY)
|
Element X, Y, and XY moments
|
| N(X. Y)
|
Out-of-plane X, Y shear
|
| T(X, Y, XY)
|
In-plane element X, Y, and XY forces
|
| NL:EPEQ
|
Equivalent plastic strain
|
| Thick
|
Element thickness
|
Table 4.163-3 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 4.163-3:
| Name
|
Item
|
E
|
| MX
|
SMISC
|
1 |
| MY
|
SMISC
|
2 |
| MXY
|
SMISC
|
3 |
| NX
|
SMISC
|
4 |
| NY
|
SMISC
|
5 |
| TX
|
SMISC
|
6 |
| TY
|
SMISC
|
7 |
| TXY
|
SMISC
|
8 |
| EPEQ (top)
|
NMISC
|
1 |
| EPEQ (middle)
|
NMISC
|
2 |
| EPEQ (bottom)
|
NMISC
|
3 |
| EPEQ
|
NMISC
|
n |
| Thick
|
NMISC
|
n+1 |
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.
A triangular element may be formed by defining duplicate K and L node numbers as described in Section 2.8. In this event, the C0 triangular shell element (KEYOPT(1)=4) will be used.
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 meshing fails. In this case, a triangular element should be used; see Section 2.8.