3-Node Axisymmetric Shell
The SHELL209 element is suitable for analyzing thin to moderately thick axisymmetric shell structures. It is a three-node element with three degrees of freedom at each node: translations in the X, Y directions, and a rotation about the Z-axis. A fourth translational degree of freedom in z direction can be included to model uniform torsion (KEYOPT(2) = 1). When the membrane option is used, the rotational degree of freedom is excluded. (For higher efficiency, the two-node element SHELL208 may be more suitable.)
The element is well suited for linear, large rotation, and/or large strain nonlinear applications. Changes in shell thickness and follower effects of distributed pressures are accounted for in nonlinear analyses, and it can be used for layered applications for modeling laminated composite shells or sandwich construction. See SHELL209 for more details about this element.
Figure 209.1: SHELL209 Geometry shows the geometry, node locations, and element coordinate system for this element. The element is defined by three nodes. For material property labels, the local x-direction corresponds to the meridional direction of the shell element. The local y-direction is the circumferential. The local z-direction corresponds to the through-the-thickness direction. Element formulation is based on logarithmic strain and true stress measures. Element kinematics allows for finite membrane strains (stretching). However, the curvature changes within an increment are assumed to be small.
The shell thickness and more general properties (such as material and number of integration points through the thickness) are specified via section commands (SECTYPE, SECDATA and SECCONTROL). Shell section commands allow for both single-layered and composite shell definitions. You can designate the number of integration points (1, 3, 5, 7, or 9) located through the thickness of each layer. If only one, the integration point is always located midway between the top and the bottom surfaces. If three or more, two points are located on the top and the bottom surfaces respectively and the remaining points are distributed evenly between these two points. The default for each layer is three integration points. The element can have variable thickness, as a tabular function of global/local coordinates or node numbers (SECFUNCTION).
Element loads are described in Nodal Loading. Pressure may be input as surface loads on the element faces as shown by the circled numbers on Figure 209.1: SHELL209 Geometry. Positive pressures act into the element.
Temperatures can be input as element body loads at the corners of the outside faces of the element and the corners of the interfaces between layers. The first corner temperature T1 defaults to TUNIF. If all other temperatures are unspecified, they default to T1. If KEYOPT(1) = 0 and exactly NL+1 (where NL is the number of layers in the shell section) temperatures are input, one temperature is used for the bottom corners of each layer, and the last temperature is for the top corners of the top layer. If KEYOPT(1) = 1 and if exactly NL temperatures are input, one temperature is used for the two corners of each layer. That is, T1 is used for T1, T2, and T3; T2 (as input) is used for T4, T5, and T6, etc. For any other input patterns, unspecified temperatures default to TUNIF.
Nodal forces, if any, should be input on a full 360° basis.
KEYOPT(1) is the membrane option. When KEYOPT(1) = 1, the element uses one integration point through-the-thickness and accounts for only membrane stiffness (that is, the bending and transverse shear stiffness are ignored).
KEYOPT(2) controls the torsion capability. When KEYOPT(2) = 1, the element allows constant torsion by allowing a translational degree of freedom UZ in the circumferential direction.
SHELL209 includes the effects of transverse shear deformation. The transverse shear stiffness E11 can be specified with SECCONTROL. For a single-layered shell with isotropic material, default transverse shear stiffness is kGh, in which k = 5/6, G is the shear modulus, and h is the thickness of the shell.
SHELL209 can be associated with linear elastic, elastoplastic, creep, or hyperelastic material properties.
Set KEYOPT(8) = 2 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.
Set KEYOPT(9) = 1 to read initial thickness data from a user subroutine.
KEYOPT(10) = 1 outputs normal stress component Sz, where z is shell normal direction. The element uses a plane-stress formulation that always leads to zero thickness normal stress. With KEYOPT(10) = 1, Sz is independently recovered during the element solution output from the applied pressure load.
The effects of pressure load stiffness are automatically included for this element. If an unsymmetric matrix is needed for pressure load stiffness effects, use NROPT,UNSYM.
I, J, K
|UX, UY, ROTZ -- If KEYOPT(1) = 0 and KEYOPT(2) = 0|
|UX, UY -- If KEYOPT(1) = 1 and KEYOPT(2) = 0|
|UX, UY, UZ, ROTZ -- If KEYOPT(1) = 0 and KEYOPT(2) = 1|
|UX, UY, UZ -- If KEYOPT(1) = 1 and KEYOPT(2) = 1|
|TB command: See Element Support for Material Models for this element.|
|MP command: EX, EY, EZ, PRXY, PRYZ, PRXZ (or NUXY, NUYZ, NUXZ),|
|ALPX, ALPY, ALPZ (or CTEX, CTEY, CTEZ or THSX, THSY, THSZ),|
|DENS, GXY, GYZ, GXZ, ALPD, BETD, DMPR|
|face 1 (I-J-K) (top, in -N direction),|
|face 2 (I-J-K) (bottom, in +N direction)|
|For KEYOPT(1) = 0:|
|T1, T2 T3 (corresponding to nodes I, J, and K) at bottom of layer 1, and T4, T5, T6 (corresponding to nodes I, J, and K) between layers 1-2. A similar relationship exists for all layers, ending with temperatures at the top of layer NL. For one-layer elements, therefore, six temperatures are used.|
|For KEYOPT(1) = 1:|
|T1, T2, T3 for layer 1; T4, T5, T6 for layer 2; similarly for all layers (3 * NL maximum). Hence, for one-layer elements, three temperatures are used.|
|Birth and death|
|Element technology autoselect|
Bending and membrane stiffness (default).
Membrane stiffness only.
Storage of layer data:
For multi-layer elements, store data for bottom of bottom layer and top of top layer. For single-layer elements, store data for TOP and BOTTOM. (Default)
Store data for TOP and BOTTOM for all layers.
Store data for TOP, BOTTOM, and MID for all layers. (The volume of data may be excessive.)
No user subroutine to provide initial thickness (default).
Read initial thickness data from user subroutine UTHICK
See the Guide to User-Programmable Features in the for information about user-written subroutines.
Thickness normal stress (Sz) output option:
Sz not modified (default, Sz = 0)
Recover and output Sz from applied pressure load
The solution output associated with the element is in two forms:
Nodal displacements included in the overall nodal solution.
Additional element output as shown in Table 209.1: SHELL209 Element Output Definitions
Several items are illustrated in Figure 209.2: SHELL209 Element Stress Output.
KEYOPT(8) controls the amount of data output on the result file for processing with the LAYER command. Interlaminar shear stress is available at the layer interfaces. Setting KEYOPT(8) = 1 or 2 is necessary for these stresses to be output in POST1. A general description of solution output is given in Solution Output. See the Basic Analysis Guide for ways to view results.
The element stress resultants (N11, M11, Q13, etc.) are parallel to the element coordinate system, as are the membrane strains and curvatures of the element. Such generalized strains are available through the SMISC option at the element centroid only. The transverse shear force Q13 are available only in resultant form: that is, use SMISC,5. Likewise, the transverse shear strain.
γ13 is constant through the thickness and only available as a SMISC item (SMISC,10).
ANSYS computes moments (M11, M22) with respect to the shell reference plane. By default, ANSYS adopts the shell midplane as the reference plane. To offset the reference plane to any other specified location, issue the SECOFFSET command. When there is a nonzero offset (L) from the reference plane to the midplane, moments with respect to the midplane ( ) can be recovered from stress resultants with respect to the reference plane as follows:
SHELL209 does not support extensive basic element printout. POST1 provides more comprehensive output processing tools; therefore, we suggest using OUTRES command to ensure that the required results are stored in the database.
The Element Output Definitions table uses the following notation:
A colon (:) in the Name column indicates that 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 “-” indicates that the item is not available.
Table 209.1: SHELL209 Element Output Definitions
|NODES||Nodes - I, J, K||-||Y|
|XC, YC||Location where results are reported||Y||4|
|PRES||Pressures P1 (top) at NODES I, J; P2 (bottom) at NODES I, J||-||Y|
|TEMP||Temperatures T1, T2 at bottom of layer 1, T3, T4 between layers 1-2, similarly for between next layers, ending with temperatures at top of layer NL (2*(NL+1) maximum)||-||Y|
|LOC||TOP, MID, BOT, or integration point location||-||1|
|S:X, Y, Z, XY, YZ, XZ||Stresses||3||1|
|S:1, 2, 3||Principal stresses||-||1|
|EPEL:X, Y, Z, XY,YZ,XZ||Elastic strains||3||1|
|EPEL:EQV||Equivalent elastic strain||-||1|
|EPTH:X, Y, Z, XY,YZ,XZ||Thermal strains||3||1|
|EPTH:EQV||Equivalent thermal strain||-||1|
|EPPL:X, Y, Z, XY,YZ,XZ||Average plastic strains||3||2|
|EPPL:EQV||Equivalent plastic strain||-||2|
|EPCR:X, Y, Z, XY,YZ,XZ||Average creep strains||3||2|
|EPCR:EQV||Equivalent creep strain||-||2|
|EPTO:X, Y, Z ,XY,YZ,XZ||Total mechanical strains (EPEL+EPPL+EPCR)||3||-|
|EPTO:EQV||Total equivalent mechanical strains||-||-|
|NL:EPEQ||Accumulated equivalent plastic strain||-||2|
|NL:CREQ||Accumulated equivalent creep strain||-||2|
|NL:SRAT||Plastic yielding (1 = actively yielding, 0 = not yielding)||-||2|
|SEND:ELASTIC, PLASTIC, CREEP, ENTO||Strain energy densities||-||2|
|N11, N22, N12||In-plane forces (per unit length)||-||Y|
|M11, M22||Out-of-plane moments (per unit length)||-||Y|
|Q13||Transverse shear forces (per unit length)||-||Y|
|E11, E22, E12||Membrane strains||-||Y|
|γ13||Transverse shear strain||-||Y|
|LOCI:X, Y, Z||Integration point locations||-||5|
|SVAR:1, 2, ... , N||State variables||-||6|
|ILSXZ||SXZ interlaminar shear stress||-||Y|
|ILSYZ||SYZ interlaminar shear stress||-||Y|
|ILSUM||Magnitude of the interlaminar shear stress vector||-||Y|
|ILANG||Angle of interlaminar shear stress vector (measured from the element x-axis toward the element y-axis in degrees)||-||Y|
|Sm: 11, 22, 12||Membrane stresses||-||Y|
|Sb: 11, 22||Bending stresses||-||Y|
|Sp: 11, 22, 12||Peak stresses||-||Y|
|St: 13||Averaged transverse shear stresses||-||Y|
Nonlinear solution output for top, middle, and bottom surfaces, if the element has a nonlinear material, or if large-deflection effects are enabled (NLGEOM,ON) for SEND.
Stresses, total strains, plastic strains, elastic strains, creep strains, and thermal strains in the element coordinate system are available for output (at all section points through thickness). If layers are in use, the results are in the layer coordinate system.
Available only at centroid as a *GET item.
Available only if OUTRES,LOCI is used.
Table 209.2: SHELL209 Item and Sequence Numbers lists output available through the ETABLE command using the Sequence Number method. See The General Postprocessor (POST1) and The Item and Sequence Number Table in this reference for more information. The following notation is used in Table 209.2: SHELL209 Item and Sequence Numbers:
Table 209.2: SHELL209 Item and Sequence Numbers
|Output Quantity Name||ETABLE and ESOL Command Input|
|Sp: 11 (at shell bottom)||SMISC||23||-||-||-|
|Sp: 22 (at shell bottom)||SMISC||24||-||-||-|
|Sp: 12 (at shell bottom)||SMISC||25||-||-||-|
|Sp: 11 (at shell top)||SMISC||26||-||-||-|
|Sp: 22 (at shell top)||SMISC||27||-||-||-|
|Sp: 12 (at shell top)||SMISC||28||-||-||-|
The axisymmetric shell element must be defined in the global X-Y plane with the Y-axis the axis of symmetry.
The element cannot have a zero length.
Zero thickness elements, or elements tapering down to a zero thickness at any corner, are not allowed (but zero thickness layers are allowed).
If multiple load steps are used, the number of layers may not change between load steps.
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.
Transverse shear stiffness of the shell section is estimated by an energy equivalence procedure (of the generalized section forces & strains vs. the material point stresses and strains). The accuracy of this calculation may be adversely affected if the ratio of material stiffnesses (Young's moduli) between adjacent layers is very high.
The calculation of interlaminar shear stresses is based on simplifying assumptions of unidirectional, uncoupled bending in each direction. If accurate edge interlaminar shear stresses are required, shell-to-solid submodeling should be used.
The section definition permits use of hyperelastic material models and elastoplastic material models in laminate definition. However, the accuracy of the solution is primarily governed by fundamental assumptions of shell theory. The applicability of shell theory in such cases is best understood by using a comparable solid model.
For nonlinear applications, this element works best with full Newton-Raphson solution scheme (NROPT,FULL,ON).
In a nonlinear analysis, the solution process terminates if the thickness at any integration point that was defined with a nonzero thickness vanishes (within a small numerical tolerance).
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 Mechanical Pro
Birth and death is not available.
Initial state is not available.
Linear perturbation is not available.
ANSYS Mechanical Premium
Birth and death is not available.