This example demonstrates the performance of the shell element
formulations in
Abaqus,
particularly with respect to the representation of inextensional bending modes
and complex membrane states.
A finite length circular cylinder shell with rigid diaphragms in
its ends, subjected to concentrated pinching loads, is analyzed; and the
results are compared with known solutions (see Lindberg et al., 1969).
The geometry and material properties used for the example are shown in
Figure 1.
No units are specified since the values given are in a self-consistent set of
units. The thickness of the cylinder is 1/100 of its radius, so the structure
can be considered a thin shell. The mesh covers a symmetric segment of the
cylinder, as indicated in the figure, with symmetry boundary conditions imposed
on three edges of the mesh, while the fourth edge (the end of the cylinder) is
supported by a rigid diaphragm.
Two mesh patterns are used in this example: a regular mesh, shown in
Figure 2,
and two types of irregular meshes (coarse and fine), shown in
Figure 3
and
Figure 4.
When triangular elements are used, each quadrilateral is divided into two
triangles. The irregular meshes are tested because such mesh patterns might be
used in cases where local effects must be modeled, and they allow an assessment
to be made of the distortion sensitivity of the elements. For comparison, the
cylinder is analyzed with all the general shell elements available in
Abaqus/Standard;
the
Abaqus/Explicit
analyses test only the S3R and S4R elements.
The submodeling capability in
Abaqus/Standard
is also used in this example to analyze the region in the vicinity of the
concentrated load. For shell-to-shell submodeling two regular mesh patterns of S8R elements, shown in
Figure 5,
are driven by various global analyses also using regular meshes. In each case
symmetry boundary conditions are imposed on two edges of the mesh, while
results from the global analyses are interpolated to the remaining two edges
through the submodeling technique. A shell-to-solid submodel is also available
for demonstration purposes.
The shell-to-solid coupling capability in
Abaqus/Standard
and
Abaqus/Explicit
is also used in this example. The region in the vicinity of the concentrated
load is meshed with continuum elements, and the rest of the cylinder is meshed
with shell elements (see
Figure 6).
S4R, S8R, C3D8I, C3D10, C3D10HS, and C3D20R elements are used in six different shell-to-solid combinations in
Abaqus/Standard;
S4R and C3D8R elements are used in
Abaqus/Explicit.
The displacements are small, so it is appropriate to ignore geometric
nonlinearities in the
Abaqus/Explicit
analyses. If the large-displacement theory is activated by considering
geometric nonlinearities, the results are unchanged in all cases since the
strains and rotations remain small. However, the analysis
CPU times typically increase by about 30%.
Two input files are provided for the continuum shell element model to
illustrate orienting the element thickness (stacking) direction independent of
the nodal connectivity using a cylindrical system.
Results and discussion
The result used for comparison is the radial displacement at the point where
the pinching load is applied. The solution given by Lindberg et al., based on
Flügge's (1973) series solution, is 0.1825 × 10−4.
Regular mesh
The results for the regular
Abaqus/Standard
mesh are shown in
Table 1.
The second-order elements (types S8R5 and S9R5) provide the most accurate solutions, whereas element type S8R (also a second-order element, but designed primarily for thick
shell applications) provides a rather less accurate solution. Element type STRI3 provides the most accuracy among the first-order elements. None
of the first-order elements provides acceptable solutions with the coarsest
meshes used.
Element type STRI65 appears to converge rather slowly compared to the other element
types. This result may appear counterintuitive, especially when compared to the
STRI3 results, which demonstrate better convergence in this problem.
Compared to STRI3, which is a flat facet element, element type STRI65 is preferable for modeling bending of thin shells and has
complete quadratic representation of membrane strains; therefore, STRI65 is expected to perform better than STRI3 provided the number of elements in the two meshes is the same. In
the present convergence study we have instead retained an equal number of
nodes, which results in the relatively poor performance of the STRI65 element.
The results for the regular
Abaqus/Explicit
mesh are shown in
Table 2.
The results suggest that element types S3R and S4R are initially stiff but then converge to the correct solution. In
addition, an energy plot is provided in
Figure 7,
which shows that by the end of the analysis a steady, static solution is
obtained.
Irregular mesh
The second type of irregular mesh has more distorted element shapes than the
first type of irregular mesh. The results for the two irregular
Abaqus/Standard
meshes are given in
Table 3;
and, as discussed in
The barrel vault roof problem,
they show less accurate results than the regular mesh problems.
Element types S8R5 and S9R5 again provide reasonably accurate results with fine meshes,
although the coarse mesh results with these elements demonstrate poor accuracy.
Interestingly, in this case all the first-order quadrilateral elements provide
quite accurate values even with coarse meshing. This result may be fortuitous
and should not be taken as a general indication of the quality of the elements
in distorted meshes. For element type S4R both stiffness-based and enhanced hourglass controls are used to
study the effect of mesh refinement and skew sensitivity. As expected, the
coarse mesh results for enhanced hourglass control show poor accuracy compared
with the fine mesh results.
The results for the irregular Abaqus/Explicit meshes are given in Table 4. These irregular meshes are more accurate despite the increased distortion
because mesh refinement is concentrated in the area of highest solution
gradients.
Submodeled analyses
Results from the submodeled
Abaqus/Standard
analyses for the shell-to-shell cases are given in
Table 5.
Clearly, the submodeling technique provides a more accurate solution in the
vicinity of the point load than the coarser global analyses. When S4R elements are used on the global level, the radial displacement at
the point of load application is within 40% of Lindberg's solution for the
coarse mesh and 13% for the finer mesh. The submodeling technique significantly
improves these results, giving radial displacements in the shell submodels
within 11% and 2% for all four combinations of meshes.
When S8R elements are used to mesh the quarter cylinder, solution accuracy
improves from within 6% on the global level to within 0.7% on the submodel
level. Displacement contours for the shell submodels are shown in
Figure 8
for a representative analysis in which a 5 × 5 mesh of S8R elements is used on the global level and a 10 × 10 mesh of S8R elements is used on the submodel level.
Submodel analyses are tested with output from input files
pinchcyl_s4r_reg55.inp,
pinchcyl_s4r_reg1010.inp, and
pinchcyl_s8r_reg55.inp. If
five degree of freedom shells (S4R5, S8R5, etc.) are used at the global level, only the displacement
degrees of freedom on the submodel boundary are driven since the rotations are
not written to the results file for these elements.
A shell-to-solid submodel is also available for this problem, with a 10 × 10
C3D8I element mesh and four elements across the shell thickness. The
submodel is driven from a 12 × 12 S4R element global model. The results are in good agreement with the
shell-to-shell submodel results. Since the submodel in this case is made of
solid elements, no comparison to the shell analytical solution is offered. The
use of the shell-to-solid submodeling capability would be more justified in the
case of concentrated loading applied on a finite area instead of the point
load.
Shell-to-solid coupling analyses
Six shell-to-solid coupling cases are analyzed in
Abaqus/Standard,
as listed in
Table 6.
In all six cases a 12 × 12 shell element mesh is used. As is clearly seen, the
shell-to-solid coupling analyses provide accurate solutions in the vicinity of
the point load. The radial displacement at the point of load application is
within 4.1% of Lindberg's solution for all six cases. As mentioned for
submodeling, the use of the shell-to-solid coupling capability would be more
justified in the case of concentrated loading applied on a finite area instead
of the point load.
The results for the
Abaqus/Explicit
shell-to-solid coupling analysis are given in
Table 7.
The radial displacement at the point of load application is within 32% of
Lindberg's solution.
Parametric study using the
Abaqus
parametric study capability
The performance of shell element formulations investigated in this example
can be analyzed conveniently in a parametric study using the scripting
capabilities offered in
Abaqus.
As an example we perform a parametric study in which eight analyses are
automatically executed; these analyses correspond to combinations of three
different (regular) mesh densities (5 × 5, 10 × 10, 20 × 20) for three
different element types (S4, S8R, and S3R).
pinchcyl_parametric.inp shows
the parametrized template input data used to generate the parametric variations
of the parametric study. The script file (pinchcyl_parametric.psf) is
used to perform the parametric study. The radial displacement at the point
where the pinching load is applied is reported in the following table for each
of the analyses of the parametric study:
Flügge, W., Stresses
in
Shells, Springer-Verlag, New
York, Second, 1973.
Lindberg, G.M.M., D. Olson, and G. R. Cowper, “New
Developments in the Finite Element Analysis of
Shells,” Quarterly Bulletin of the Division
of Mechanical Engineering and the National Aeronautical Establishment, National
Research Council of
Canada, vol. 4, 1969.
Tables
Table 1. Comparison of radial displacement results for pinched cylinder. Regular
meshes.
Abaqus/Standard
analysis.
Element type
Number of dof
Displacement
Error (compared to 1.825
× 10−5)
(× 10−5)
STRI3
216
1.134
−38%
726
1.696
−7%
2646
1.829
0.2%
S4R5
216
1.099
−40%
726
1.597
−12%
2646
1.778
−2.6%
S4
216
0.951
−47.8%
726
1.519
−16.7%
2646
1.750
−4.0%
S4R
216
1.089
−40.3%
726
1.591
−12.8%
2646
1.779
−2.5%
S4R*
216
0.954
–47.7%
726
1.525
–16.4%
2646
1.755
–3.8%
S8R5
726
1.804
−1.1%
2646
1.833
0.4%
S8R
576
1.721
−5.7%
2046
1.806
−1%
S9R5
726
1.804
−1.1%
2646
1.833
0.4%
STRI65
726
1.358
−25.6%
2646
1.765
−3.3%
S3R
216
0.653
−64%
726
1.328
−27%
2646
1.674
−8.3%
SC6R
216
0.652
–65.7%
726
1.327
–27.3%
2649
1.673
–8.3%
SC8R
216
1.123
–38.5%
726
1.608
–11.9%
2649
1.784
–2.25%
*Abaqus/Standard
finite-strain element with enhanced hourglass control.
Table 2. Comparison of radial displacement results for pinched cylinder. Regular
meshes.
Abaqus/Explicit
analysis.
Element type
Number of elements
Displacement
Error (compared to 1.825
× 10−5)
(× 10−5)
S3R
50
0.767
−58.%
200
1.390
−24.%
800
1.703
−6.7%
S4R
25
1.115
−39.%
100
1.616
−11.%
400
1.806
−1.0%
Table 3. Comparison of radial displacement results for pinched cylinder.
Irregular meshes.
Abaqus/Standard
analysis.
Element
Number of dof
Mesh type 1
Error
Mesh type 2
Error
type
Displacement
Displacement
(× 10−5)
(× 10−5)
STRI3
894
1.767
−3.2%
1.372
−25%
3318
1.810
−0.8%
1.663
−9%
S4R5
894
1.815
−0.5%
1.790
−1.9%
3318
1.835
0.5%
1.842
0.9%
S4R
894
1.814
−0.6%
1.781
−2.4%
3318
1.849
1.3%
1.862
2.0%
S4R*
894
1.764
–3.3%
1.618
–10.7%
3318
1.840
0.8%
1.845
1.1%
S4
894
1.687
−7.52%
1.454
−20.3%
3318
1.814
−0.58%
1.777
−2.5%
S8R5
918
1.803
−1.2%
1.519
−17%
3366
1.793
−1.8%
1.793
−1.8%
S8R
702
1.664
−9%
1.244
−32%
2550
1.726
−5.4%
1.726
−5.4%
S9R5
918
1.793
−1.8%
1.504
−18%
3366
1.831
0.3%
1.774
−2.8%
STRI65
918
1.723
−5.6%
1.551
−15.01%
3366
1.850
1.4%
1.824
−0.05%
S3R
894
1.565
−14%
1.270
−30%
3318
1.763
−3.4%
1.654
−9.4%
SC6R
894
1.563
–14.3%
1.273
–30.2%
3318
1.762
–3.4%
1.655
–9.3%
SC8R
894
1.821
–0.22%
1.767
–3.18%
3318
1.850
1.37%
1.865
2.19%
*
Abaqus/Standard
finite-strain element with enhanced hourglass control.
Table 4. Comparison of radial displacement results for pinched cylinder.
Irregular meshes.
Abaqus/Explicit
analysis.
Element type
Number of elements
Displacement
Error (compared to 1.825
× 10−5)
(× 10−5)
S3R
256
1.618
−11.3%
1024
1.794
−1.69%
S4R
128
1.848
1.24%
512
1.883
3.17%
Table 5. Comparison of radial displacement results for submodeled analyses in
Abaqus/Standard.
Reference solution: 1.825 × 10−5
Global
Global
Submodel
Displacement
Error
Element Type
Mesh Size
Mesh Size
(× 10−5)
S4R
5 × 5
n/a
1.092
−40.2%
5 × 5
1.6139
−11.6%
10 × 10
1.6259
−10.9%
10 × 10
n/a
1.592
−12.8%
5 × 5
1.7775
−2.6%
10 × 10
1.7881
−2.0%
S8R
5 × 5
n/a
1.721
−5.7%
5 × 5
1.8004
−1.3%
10 × 10
1.8123
−0.7%
Table 6. Comparison of radial displacement results for
Abaqus/Standard
shell-to-solid coupling analyses.
Shell element
Continuum element
Displacement
Error (compared to 1.825
× 10−5)
(× 10−5)
S4R
C3D8I
1.750
−4.11%
S4R
C3D10
1.775
−2.74%
S4R
C3D10HS
1.775
–2.74%
S4R
C3D20R
1.837
0.656%
S8R
C3D8I
1.766
−3.23%
S8R
C3D10
1.797
−1.53%
S8R
C3D10HS
1.797
–1.53%
S8R
C3D20R
1.854
1.59%
Table 7. Comparison of radial displacement results for
Abaqus/Explicit
shell-to-solid coupling analyses.