This Section gives a short description of all the “element”
types available in EUROPLEXUS for the spatial discretization
of the problem to be solved.
The code contains various formulations, including:
We describe now the different elements available for a one-dimensional, two-dimensional (plane or axisymmetric), or three-dimensional problem, by specifying, for each problem type:
Specific information relative to each particular element type follows these tables.
Stresses are computed at the integration points.
In the output (on the listing or on the result file) all
the stresses for a given element and for each of its
integration points will be printed. See chapter GBC_0010 as well.
The various elements available in 1D are presented below.
num. | Name | Dev | Gibi | npt | dof | ngp | Remarks |
22 | TUBE | SEG2 | CEA | 2 | 1 | 1 | fluid only (rigid tube) |
23 | TUYA | SEG2 | CEA | 2 | 7 | 2 | tube coupled with FSI |
24 | CL1D | POI1 | CEA | 1 | 1 | 1 | fluid boundary condition |
25 | BIFU | SUPE | CEA | 1:9 | 7 | 1 | bifurcation junction |
26 | CAVI | SUPE | CEA | 1:9 | 1 | 1 | cavity junction |
31 | CLTU | POI1 | CEA | 1 | 7 | 1 | boundary condition with FSI |
44 | ED1D | SEG2 | JRC | 2 | 1 | 1 | 1D/2D-3D structural coupling |
146 | BREC | SEG2 | CEA | 2 | 7 | 1 | pipeline rupture |
147 | TUVF | SEG2 | CEA | 2 | 1 | 1 | rigid tube (1D vfcc) |
148 | TYVF | SEG2 | CEA | 2 | 7 | 1 | tuvf coupled with FSI (1D vfcc) |
149 | BIVF | SEG2 | CEA | 2 | 1 | 1 | bifurcation junction (1D vfcc) |
150 | CAVF | SEG2 | CEA | 1:9 | 1 | 1 | cavity junction (1D vfcc) |
For these elements (apart ED1D), the "EULER"
option
is mandatory (see page GBA_0030). Furthermore, the mesh nodes must
have three coordinates. Thus, the directives for the type of
problem treated by these elements will always be of the form:
"TRIDIM" "EULER"
Note that, for the ED1D elements
the ED1D
is used to perform coupled
1-D/multi-d calculations, therefore the problem must be declared
either "AXIS"
or "CPLA"
or "DPLA"
or
"TRID"
and the "EULE"
is not needed.
These elements are specified hereafter:
This element allows to model the fluid contained within a fixed pipeline. It is assumed that fluid properties are the same in all points of a give cross-section of the pipe (one-dimensional calculation).
This element allows to introduce the different boundary conditions or localised singularities, in a pipeline meshed by elements of type "TUBE".
To assemble the different branches of a pipeline. The junction is done by a finite volume with an attached constitutive law, unlike in the case of a simple bifurcation.
This element allows to simply specify the relationships between the inputs and outputs of different branches which are joined together. The conservation of mass flow rate and pressure is ensured.
This element allows to treat the motions of pipelines in the presence of an internal flow. It results from the superposition of elements “TUBE” and “POUTRE”.
Similarly to “CL1D”, this element further allows to introduce coupled boundary conditions of the fluid-structure type (e.g. a closed pipe end).
This element allows to model a pipeline rupture. Before the optional rupture instant, this element behaves like a bifurcation.
This 1D finite volume element allows to model the fluid contained within a fixed pipeline. It is assumed that fluid properties are the same in all points of a give cross-section of the pipe (one-dimensional calculation).
This 1D finite volume element allows to treat the motions of pipelines in the presence of an internal flow. It results from the superposition of elements “TUVF” and “POUTRE”.
This 1D finite volume element allows to simply specify the relationships between the inputs and outputs of 2 branches which are joined together. The conservation of mass flow rate is ensured.
The BIVF element can be used only with 2 branches of fixed pipeline at the moment (tuvf element).
To assemble the different branches of a pipeline composed of 1D finite volume element. The junction is done by a finite volume with an attached constitutive law, unlike in the case of a simple bifurcation.
The 1D finite volume element are under development and testing at CEA and EDF and should therefore be used with great care.
A 2-node element used as an interface between a 1D structure and a multi-D structure.
This element can be used to couple a 2D or 3D model
to a 1D model to be calculated by the EURDYN-1D code,
developed at JRC Ispra (this “code” is now embedded
within EUROPLEXUS, so that its usage is transparent to
the EUROPLEXUS user). Of the two nodes, one is used to define
the location of the interface (i.e. the point at which forces
are transmitted between the two structures), while the other
is only used to indicate the direction in space along
which coupling is enforced.
This direction remains unchanged during deformation.
The distance between the two nodes is therefore irrelevant.
The 1D structure has to be separately modelled by EURDYN-1D,
which is seen by EUROPLEXUS as a standard element module.
A special set of input data for EURDYN-1D (ED1D “input deck”)
has to be prepared. This must be included within the
normal EUROPLEXUS input file, immediately after the CALCUL
directive and before any additional EUROPLEXUS directives
(see page I.23 and the EURDYN-1D manual listed in the References:
([33])).
The ED1D input deck must be immediately preceded by
a line containing "ED1D START"
(capitals, starting in column 1, followed only by blanks if any)
and be immediately followed by a line containing "ED1D END"
(capitals, starting in column 1, followed only by blanks if any).
The following (fixed) logical unit numbers are used
by the EURDYN-1D module:
Note that units 33 and 34 are used by default to store data for TPLOT (space plots) and for a restart, respectively. They are both unformatted. These values, however, can be changed from the input.
Since EURDYN-1D is a specialised module, its usage
can lead to important savings in the overall computation
cost in large, complex multi-D problems when one or more
portions of the structure can be conveniently represented
by a 1D model.
In setting up a coupled 1-D/multi-D model, the following
guidelines should be followed:
ED1D
interface element is placed at each point of connection
between the multi-D domain and the 1-D domain. An arbitrary
number of such interface elements can be used in a calculation,
according to user needs.ED1D
element must be so oriented that its first node
coincides with the interface (attachment) point, while the
second node only defines the orientation of the 1-D structure
(i.e., of the interaction force) in multi-D space. The length
of such elements is therefore irrelevant."PT1D"
directive of this material
should be used to assign the associated node index in the
1-D model.
Furthermore, note that a few directives, most notably saving for restart, are not available in coupled 1-D/multi-D computations.
Some care should also be taken in specifying the final times for
the calculation and times for printouts and data storages.
The following procedure is suggested in order to minimize
potential problems:
TI
and TF
, respectively.FINTIM
larger than TF
, say:
FINTIM = TF + (TF - TI) * K
with : 0.01 < K < 0.1
TPRINT(NPRINT) = TF
If the final 1-D results should appear on the listing, and choose a final space plots storage time:
TSTOR(NSSTOR) = TF
If space plots in the final 1-D configuration are desired.
TEND
larger than TF
,
but smaller than the 1-D value (FINTIM
) specified above:
TF < TEND < FINTIM
TF
if desired.
In this way, the coupled calculation will be stopped at the
end by the multi-D part of the code at time TEND
,
and the printouts and storages at TF
should be correctly
produced for both the 1-D and the multi-D models.
The only drawback of this method is that the ’space plots summary’
table in the 1-D listing is not produced at the end of the run
because the 1-D calculation is stopped before its declared final time
is actually reached. However, this is not a real problem, since the
1-D space plots file is nevertheless correctly generated.
The various elements available in 2D are presented below.
num. Name Gibi Dev npt dof ngp Remarks 1 COQU SEG2 CEA 2 3 2 thin shell 2 TRIA TRI3 CEA 3 2 1 triangle 3 BARR SEG2 CEA 2 2 1 bar (membrane only) 4 PONC POI1 CEA 1 2 1 circular bar(axisym.) 5 MEMB SEG2 CEA 2 2 1 ’virole’ in membrane (axisym.) 7 CL2D SEG2 CEA 2 2 1 boundary conditions 8 CAR1 QUA4 CEA 4 2 1 quadrangle with 1 Gauss pt. 9 CAR4 QUA4 CEA 4 2 4 quadrangle with 4 Gauss pt. 10 COQC SEG2 CEA 2 3 1 thin shell with shear 15 FS2D RAC2 CEA 4 2 1 F.S. coupling 28 PMAT POI1 CEA 1 2 1 material point 38 Q92 QUA8 JRC 9 2 4 9-node quadrilateral 39 Q93 QUA8 JRC 9 2 9 9-node quadrilateral 42 CL23 SEG3 JRC 3 2 2 3-node b.c.s 43 ED01 SEG2 JRC 2 3 10 beam/conical-shell 45 TVL1 TRI3 CEA 3 2 1 Van Leer triangle 46 CVL1 QUA4 CEA 4 2 1 Van Leer quadrangle 49 Q92A QUA8 JRC 9 2 4 Q92 on symmetry axis 52 FLU1 QUA4 JRC 4 2 1 fluid quadrilateral 54 PFEM POI1 JRC 1 2 1 particle finite element 56 ED41 SEG2 JRC 4 3 10 old version of ED01 58 ADQ4 QUA4 JRC 4 2 1 advection-diffusion quadrilateral 64 FL23 TRI3 JRC 3 2 1 fluid triangle 65 FL24 QUA4 JRC 4 2 1 fluid quadrilateral 70 CL22 SEG2 JRC 2 2 2 2-node b.c.s 71 Q41 QUA4 JRC 4 2 1 ALE structural quadrilateral 72 Q42 QUA4 JRC 4 2 4 ALE structural quadrilateral 73 Q41N QUA4 JRC 4 2 1 ALE structural quadrilateral 74 Q42N QUA4 JRC 4 2 4 ALE structural quadrilateral 75 Q41L QUA4 JRC 4 2 1 Lagr. structural quadrilateral 76 Q42L QUA4 JRC 4 2 4 Lagr. structural quadrilateral 77 Q95 QUA8 JRC 9 2 4 test version of Q92 97 MC23 TRI3 JRC 3 2 1 finite volume fluid triangle 98 MC24 QUA4 JRC 4 2 1 finite volume fluid quadrilateral 100 Q42G QUA4 JRC 4 2 4 ALE structural quadrilateral 105 MS24 QUA4 JRC 4 2 1 spectral "macro" quadrilateral 106 S24 QUA4 JRC 4 2 1 spectral "micro" quadrilateral 109 FUN2 SEG2 JRC 2 2 1 cable element 114 BSHT SEG2 CEA 2 2 - bushing with translational dof 118 MAP2 —- CEA 3 2 - Point on solid edge 121 MAP5 —- CEA 3 2 - Point on 2D shell 124 INT4 —- CEA 4 2 2 2D interface element 131 T3VF TRI3 CEA 3 2 1 triangle finite volume 132 Q4VF QUA4 CEA 4 2 1 quadrangle finite volume 140 DEBR POI1 JRC 1 2 - debris particle
The specifications for these elements are given hereafter:
Reference element for all calculations with 2D thin shells.
This element can equally well represent solids or fluids. However, if the mesh is not very regular, it may give rise to fluctuations in the distribution of masses, especially near the axis of revolution.
The element has 4 components of stress (SIG) and strain (EPST) (when used for solids), organized as follows.
This element is intended for the modeling of steel reinforcement in concrete structures, or of bars that work only in traction-compression.
This element should only be used to model circular steel reinforcement in axisymmetric concrete structures.
This element is similar to COQU, but has a purely membrane behaviour.
This element allows to specify a condition of absorbing medium or an impedance.
This element is especially used to represent fluids. However, due to its under-integration, it is strongly advised to add some anti-hourglass numerical damping, unless the boundary conditions themselves prevent the appearance of hourglass motions.
The element has 4 components of stress (SIG) and strain (EPST) (when used for solids), organized as follows.
This element is recommended for elastoplastic solids.
The element has 4 components of stress (SIG) and strain (EPST), organized as follows.
Simpler than "COQUE"
, it also enables to evaluate the
shear, if this is not too large.
Incompressible fluid elements which ensure the transmission of forces.
The first face (1-2) is in the fluid, the other (3-4) in the solid. To ensure a proper fluid-structure connection, it is useful that the sides 2-3 and 1-4 be as short as possible, possibly of zero length. In this last case, only the forces normal to faces 1-2 and 3-4 will be transmitted.
These elements are defined in the mesh but they work only through
the directive "LIAISON"
. It is therefore possible
to "activate" or "deactivate" this particular connection
depending on the problem to be treated, by modifying the
"LIAISON"
directive during a "REPRISE"
(see page SR.40).
This element is particularly aimed at modeling rigid projectiles,
in connection with the directive "IMPACT"
. It can also
be used to specify added masses.
This element has been developed for Van Leer fluids.
Similarly to TVL1, this element has been developed for Van Leer fluids.
The availability of the bushing element family allows to define generalized stiffness and damping between two nodes. The implemented model provides in 2D the element BSHT, with only translation degrees of freedom. All the characteristics of the bushing element are defined using "JOINT PROPERTIES" material type.
This element is used in order to glue one slave node to a master side.
The slave node should be on the side.
2 kinematic constraints are introduced in order to impose the translation dof
of the slave node.
These elements are defined in the topology but they work only through
the directive "LIAISON"
.
This element is used in order to glue one slave node to a master shell side.
The slave node should be on the side.
2 kinematic constraints are introduced in order to impose the translation dof
of the slave node and a kinematic constraint is added on the rotational dof
of the slave node.
These elements are defined in the topology but they work only through
the directive "LIAISON"
.
The INT4 element is pure displacement interface element dedicated to the modeling of interlayers, separating "standard" structural elements. In the particular case of a composite model, this element can be considered as representing a homogeneous resin layer ensuring the interlaminar stress transfer between adjacent plies. This approach is most often referred to as "mesoscopic" laminate modeling.
2D triangle finite volume element. The finite volume is defined as cell centred. Several options for the calculation can be chosen with OPTI VFCC.
2D quadrangle finite volume element. The finite volume is defined as cell centred. Several options for the calculation can be chosen with OPTI VFCC.
This element can be used for precise modelling of continua. It can undergo arbitrarily large deformations. Since it is underintegrated, it is locking-free, but it may occasionally suffer from mechanisms if boundary conditions are too loose. In such cases, use of the Q93 element (which, however, is more expensive) is recommended.
The element has 4 components of stress (SIG) and strain (EPST), organized as follows.
This is the fully-integrated version of the Q92 element. Its use is only recommended in plane cases, when mechanisms might occur.
The element has 4 components of stress (SIG) and strain (EPST), organized as follows.
This element is mainly used to specify uniform pressure conditions acting on the boundaries of quadratic elements of type Q92, Q93 or Q92A.
This element is integrated through the thickness (5 points
at each of 2 longitudinal stations) and offers accurate
modelling in highly nonlinear cases (spreading of plasticity
through the thickness). The effect of arbitrarily large
membrane strains over the element thickness is taken into
account, unless option "EDSS"
is used (see "OPTION"
).
The element has 4 components of stress (SIG) and strain (EPST), organized as follows.
Note that, as concerns the shear strains, the engineering values γ and not the tensor values є are used, with γ_{ij}=2є_{ij}.
This element should (only) be used in place of Q92 in axisymmetric problems, for those elements that have one side along the axis of symmetry (y-axis). It does not suffer from mechanisms.
The element has 4 components of stress (SIG) and strain (EPST), organized as follows.
This element offers a specialised treatment which is thought to be particularly effective for fluids, in conjunction with the A.L.E. formulation. An implicit phase for the calculation of pressure is introduced during time integration. The element can be degenerated to represent a triangle by simply repeating one of the nodes in the description of topology.
This element is used to represent a 2D (or 3D) continuum (usually a fluid) by means of the Particle Finite Element method (PFEM).
A 4-node version of the ED01 element that facilitates fluid-structure interaction for certain problems. Two nodes are used at each extremity of the element in order to define the element thickness. However, these are really one physical node since displacements, velocities etc. are coincident.
In the element numbering, the first two nodes must define an ’external side’ of the element. In other words, they must not be along the element thickness.
The element has 4 components of stress (SIG) and strain (EPST), organized as follows.
4-node quadrilateral for advection-diffusion problems.
This element is used to model advection-diffusion problems in incompressible fluids with heat transfer, according to JRC’s models.
3-node triangle for compressible fluids. This is an alternative to the degeneratable FLU1 quadrilateral.
4-node quadrilateral for compressible fluids. This is an alternative to the degeneratable FLU1 quadrilateral.
2-node boundary condition. This is recommended for use with 2-D Ispra models. This element automatically recognizes the element to which it is attached, and uses the most appropriate pressure discretization.
4-node quadrilateral for structural ALE calculations with reduced integration.
The element has 4 components of stress (SIG) and strain (EPST), organized as follows.
4-node quadrilateral for structural ALE calculations with full integration.
The element has 4 components of stress (SIG) and strain (EPST), organized as follows.
4-node quadrilateral for structural ALE calculations with reduced integration. Uses Godunov algorithm.
The element has 4 components of stress (SIG) and strain (EPST), organized as follows.
4-node quadrilateral for structural ALE calculations with full integration. Uses Godunov algorithm. This element doesn’t work well in some test cases, so it is advisable to use Q42G instead.
The element has 4 components of stress (SIG) and strain (EPST), organized as follows.
4-node quadrilateral for Lagrangian calculations with reduced integration.
The element has 4 components of stress (SIG) and strain (EPST), organized as follows.
4-node quadrilateral for Lagrangian calculations with full integration.
The element has 4 components of stress (SIG) and strain (EPST), organized as follows.
9-node isoparametric quadrilateral with curved sides. This is a special version of the Q9 element under test, that should avoid mechanisms.
Its use is not recommended for the moment.
The element has 4 components of stress (SIG) and strain (EPST), organized as follows.
3-node finite volume triangle for multicomponent flows.
4-node finite volume quadrilateral for multicomponent flows.
4-node quadrilateral for structural ALE calculations with full integration. Uses Godunov algorithm.
The element has 4 components of stress (SIG) and strain (EPST), organized as follows.
4-node quadrilateral MACRO spectral element.
The integration points coincide with the Gauss-Lobatto-Legendre points and are determined by specifying the MICRO spectral elements S24.
4-node quadrilateral MICRO spectral element This element is used only to specify ’internal’ nodes of an MS24.
2-node cable element.
This is a specialized element for the representation of cables in 2D space, in conjunction with the FUNE material (it resists only in traction, not in compression). When used with the VM23 material, it represents a bar (which resists both in traction and in compression). The element is large-strain.
The element has 4 components of stress (SIG), organized as follows: σ_{x}, σ_{y}≈ 0, τ_{xy}=0, σ_{z}≈ 0. The total strains (EPST) follow the same organization: є_{x}, є_{y}, γ_{xy}=0, є_{z}.
1-node debris particle element.
This is a specialized element for the representation of flying debris, as e.g. resulting from an explosion or an impact, by means of spherical particles. It may be used both in 2D and in 3D.
The various elements available in 3D are presented below.
num. Name Gibi Dev npt dof ngp Remarks 57 ADC8 CUB8 JRC 8 3 1 advection-diffusion brick 32 APPU POI1 CEA 1 6 1 support 130 ASHB —- CEA 8 3 5 assumed strain thick shell 79 BILL POI1 CEA 1 3 1 particle element (NABOR and SPH) 19 BR3D SEG2 CEA 2 3 1 bar 115 BSHR —- CEA 2 6 – bushing with trans. and rot. dof 114 BSHT —- CEA 2 3 – bushing with translational dof 144 C272 CU27 JRC 27 3 8 27-node cube 145 C273 CU27 JRC 27 3 27 27-node cube 155 C81L CUB8 JRC 8 3 1 8-node cube 156 C82L CUB8 JRC 8 3 8 8-node cube 62 CL32 QUA4 JRC 4 6 4 b.c.s for CQD4 63 CL33 QUA9 JRC 9 6 9 b.c.s for CQD9 18 CL3D QUA4 CEA 4 3 1 bound. cond. (4-node face) 78 CL3I TRI3 JRC 3 3 1 3-node b.c.s 99 CL3Q QUA4 JRC 4 3 1 4-node b.c.s 29 CL3T TRI3 CEA 3 3 1 bound. cond. (3-node face) 151 CL92 QUA9 JRC 9 3 4 9-node (3D) b.c. for C272 152 CL93 QUA9 JRC 9 3 9 9-node (3D) b.c. for C273 95 CLD3 TRI3 JRC 3 6 3 b.c.s for CQD3 96 CLD6 TRI6 JRC 6 6 4 b.c.s for CQD6 47 CMC3 TRI3 CEA 3 6 2 multilayer shell 12 COQ3 TRI3 CEA 3 6 1 triangular thin shell 14 COQ4 QUA4 CEA 4 6 4 quadrangular thin shell 40 COQI TRI3 JRC 3 6 15 triangular shell (small strain) 93 CQD3 TRI3 JRC 3 6 15 degenerated shell (Hughes-Liu) 91 CQD4 QUA4 JRC 4 6 20 degenerated shell (Hughes-Liu) 94 CQD6 TRI6 JRC 6 6 20 degenerated shell (Hughes-Liu) 92 CQD9 QUA9 JRC 9 6 45 degenerated shell (Hughes-Liu) 13 CUB6 CUB8 CEA 8 3 6 brick with 6 Gauss pt 30 CUB8 CUB8 CEA 8 3 8 brick with 8 Gauss pt 6 CUBB CUB8 CEA 8 3 8 brick based on B-bar method 11 CUBE CUB8 CEA 8 3 1 brick with 1 Gauss pt 133 CUVF CUB8 CEA 8 3 1 cube finite volume 81 CUVL CUB8 CEA 8 3 1 Van Leer cube 140 DEBR POI1 JRC 1 3 - debris particle 84 DKT3 TRI3 CEA 3 6 15 shell (Mindlin) 83 DST3 TRI3 CEA 3 6 15 shell (Discrete Shear Triangle) 80 ELDI POI1 CEA 1 6 1 discrete element 66 FL34 TET4 JRC 4 3 1 fluid tetrahedron 67 FL35 PYR5 JRC 5 3 1 fluid pyramid 68 FL36 PRI6 JRC 6 3 1 fluid prism 69 FL38 CUB8 JRC 8 3 1 fluid hexahedron 53 FLU3 CUB8 JRC 8 3 1 fluid brick 16 FS3D RAC3 CEA 8 3 1 F.S. connection (4-node face) 48 FS3T PRI6 CEA 6 3 1 F.S. connection (3-node face) 110 FUN3 SEG2 JRC 2 3 1 cable element 153 LIGR SUPE CEA 2* 6 - mechanism (articulated systems) 125 INT6 —- CEA 6 3 1 triangular prism interface element 126 INT8 —- CEA 8 3 4 hexahedron interface element 119 MAP3 —- CEA 4 3 – point on a triangular facet 120 MAP4 —- CEA 5 3 – point on a quadrangular facet 122 MAP6 —- CEA 4 6 – point on a triangular shell facet 123 MAP7 —- CEA 5 6 – point on a quadrangular shell facet 101 MC34 TET4 JRC 4 3 1 finite volume tetrahedron 102 MC35 PYR5 JRC 5 3 1 finite volume pyramid 103 MC36 PRI6 JRC 6 3 1 finite volume prism 104 MC38 CUB8 JRC 8 3 1 finite volume hexahedron 33 MECA SEG2 CEA 2 6 1 mechanism (articulated systems) 128 MOY4 —- CEA 4 3 – node to element mean connector 129 MOY5 —- CEA 5 3 – node to element mean connector 107 MS38 CUB8 JRC 8 3 1 spectral "macro" quadrilateral 54 PFEM POI1 JRC 1 3 1 particle finite element 28 PMAT POI1 CEA 1 3 1 material point 17 POUT SEG2 CEA 2 6 2 beam 20 PR6 PRI6 CEA 6 3 6 prism with 6 Gauss pt 27 PRIS PRI6 CEA 6 3 1 prism with 1 Gauss pt 134 PRVF PRI6 CEA 6 3 1 prism finite volume 82 PRVL PRI6 CEA 6 3 1 Van Leer prism 136 PYVF PYR4 CEA 5 3 1 pyramid finite volume 138 Q4MC QUA4 CEA 4 6 - multilayered quadrangular shell 90 Q4G4 QUA4 CEA 4 6 4 shell (Batoz) 111 Q4GR QUA4 CEA 4 6 5 idem Q4G4 (simplified : 1 pt) 112 Q4GS QUA4 CEA 4 6 20 idem Q4G4 (simplified : 4 pts) 35 QPPS QUA4 CEA 4 6 5 similar to Q4GR 113 RL3D SEG2 CEA 2 3 1 two-node spring 108 S38 CUB8 JRC 8 3 1 spectral "micro" quadrilateral 117 SH3D —- CEA 3 6 – node to shell connector 127 SH3V —- CEA 8 3 4 node to element connector 85 SHB8 CUB8 CEA 8 3 5 thick shell 89 SPHC POI1 CEA 1 6 1 particle element (thick shell) 139 T3MC TRI3 CEA 4 6 - multilayered triangular shell 51 T3GS TRI3 CEA 3 6 5 shell (Reissner-Mindlin) 21 TETR TET4 CEA 4 3 1 tetrahedron with 1 Gauss pt 135 TEVF TET4 CEA 4 3 1 tetrahedron finite volume 41 TUBM SUPE CEA 1* 3* 1 connection 3D-1D 116 TUYM SUPE CEA 1* 3* 1 connection 3D-1D
The specifications for these elements are given hereafter:
Solid element for elasto-plastic computations. This element developed at EDF ([882]) is free from volumetric locking and does not exhibit hourglassing. When the material becomes quasi-incompressible, one should decrease CSTAB coefficient to maintain the calculation stable.
This element is used especially with fluid materials. However, because of its under-integration, "hourglassing" phenomena may appear, if they are not prevented by the boundary conditions. Such phenomena may be contrasted by using the HOURG option (anti-hourglass artificial viscosity).
The element has 6 components of stress (SIG), organized as follows (for solid materials): σ_{x}, σ_{y}, σ_{z}, τ_{xy}, τ_{yz}, τ_{xz}. The total strains (EPST) follow the same organization: є_{x}, є_{y}, є_{z}, γ_{xy}, γ_{yz}, γ_{xz}. Note that, as concerns the shear strains, the engineering values γ and not the tensor values є are used, with γ_{ij}=2є_{ij}.
This element must be used with care. In order to obtain good results make sure to use a symmetric mesh (ex: British flag).
Solid element for elasto-plastic computations. This element should be used with caution, because being underintegrated it may lead to hourglassing. Use preferentially CUBB or CUB8 elements.
The element has 6 components of stress (SIG), organized as follows: σ_{x}, σ_{y}, σ_{z}, τ_{xy}, τ_{yz}, τ_{xz}. The total strains (EPST) follow the same organization: є_{x}, є_{y}, є_{z}, γ_{xy}, γ_{yz}, γ_{xz}. Note that, as concerns the shear strains, the engineering values γ and not the tensor values є are used, with γ_{ij}=2є_{ij}.
This element is recommended for computations on 3-D shells if the deformations are small. In reality, this element is composed of 4 triangular COQ3 plates which are superimposed and symmetrized.
Same remarks as for FS2D.
This element enables the modelling of complex profile beams submitted to a tension or bending stress. The default stability time step for this element is quite conservative (optimized for tubes?). Larger or even much larger values for different cross sections may be obtained by using the option DTBE (see H 20).
Same remarks as for CL2D.
This element is mainly used to model concrete rebars or any other beam submitted to a simple tension.
As it is the case of CUB8, this element is recommended for elasto-plastic computations.
The element has 6 components of stress (SIG), organized as follows: σ_{x}, σ_{y}, σ_{z}, τ_{xy}, τ_{yz}, τ_{xz}. The total strains (EPST) follow the same organization: є_{x}, є_{y}, є_{z}, γ_{xy}, γ_{yz}, γ_{xz}. Note that, as concerns the shear strains, the engineering values γ and not the tensor values є are used, with γ_{ij}=2є_{ij}.
This element may be used for fluids or for elasto-plastic computations.
The element has 6 components of stress (SIG), organized as follows (for solid materials): σ_{x}, σ_{y}, σ_{z}, τ_{xy}, τ_{yz}, τ_{xz}. The total strains (EPST) follow the same organization: є_{x}, є_{y}, є_{z}, γ_{xy}, γ_{yz}, γ_{xz}. Note that, as concerns the shear strains, the engineering values γ and not the tensor values є are used, with γ_{ij}=2є_{ij}.
This prismatic element is especially used for fluids (see CUBE).
The element has 6 components of stress (SIG), organized as follows (for solid materials): σ_{x}, σ_{y}, σ_{z}, τ_{xy}, τ_{yz}, τ_{xz}. The total strains (EPST) follow the same organization: є_{x}, є_{y}, є_{z}, γ_{xy}, γ_{yz}, γ_{xz}. Note that, as concerns the shear strains, the engineering values γ and not the tensor values є are used, with γ_{ij}=2є_{ij}.
Primarily, this element enables the modelling of rigid
missiles in connection with the keyword "IMPACT"
; but it
also enables the introduction of added masses.
Same remarks as for CL2D.
Solid element recommended for elasto-plastic computations (no hourglassing phenomena).
The element has 6 components of stress (SIG), organized as follows: σ_{x}, σ_{y}, σ_{z}, τ_{xy}, τ_{yz}, τ_{xz}. The total strains (EPST) follow the same organization: є_{x}, є_{y}, є_{z}, γ_{xy}, γ_{yz}, γ_{xz}. Note that, as concerns the shear strains, the engineering values γ and not the tensor values є are used, with γ_{ij}=2є_{ij}.
This element has one node and six degrees of freedom. It allows to use constitutive equations of type non-linear support in a chosen direction. See also page C2.108.
This element has two nodes with six degrees of freedom. It allows to use constitutive equations for mechanisms (articulations, etc.).
Connection 3D-1D. Consult the corresponding ‘liaison’ (connection).
Connection 3D-1D for moving meshes (ALE). Consult the corresponding ‘liaison’ (connection).
This element is used for the modelling of an eccentric layer in relation to the average plane defined by its 3 nodes. The layer is associated with an orthotropic behaviour in the given plane. Several CMC3 elements are supported by the same nodes, but they are differently eccentric; they represent a multilayer structure.
The geometric and mechanical characteristics of the element
(eccentricity, orthotropy associated to a local system)
can be defined either when CASTEM2000 generates the mesh (see option
CASTEM page A.30) or directly by EUROPLEXUS (see page C.95) in a normal
mesh generated by COCO or GIBI.
The local reference of the element is as follows: the first axis is
formed by side 1-2, the second is such that the 3rd node lies
in the half-plane (Y>0).
Same remarks as for FS2D.
3-node thick shell (Reissner-Mindlin) element with 1 integration point in the plane. It has the same local frame as COQ3. This element developed at EDF ([869]).
It is a predecessor of the Q4G family, uses the same approach for representing the shear strain and is thus the best suited among T3 shell elements to be combined with Q4G shell elements.
The element has 8 components of stress (SIG), organized as follows: σ_{x}^{m}, σ_{y}^{m}, τ_{xy}^{m}, σ_{x}^{b}, σ_{y}^{b}, τ_{xy}^{b}, τ_{xz}, τ_{yz}, where the first three components are the membrane contributions, the second three components are the bending contributions and the last two components are the transverse shear contributions (note that the order in which these last two components are given is opposite to what is usually found in 3D continuum elements, for example). The total strains (EPST) follow the same organization: є_{x}^{m}, є_{y}^{m}, γ_{xy}^{m}, є_{x}^{b}, є_{y}^{b}, γ_{xy}^{b}, γ_{xz}, γ_{yz}. Note that, as concerns the shear strains, the engineering values γ and not the tensor values є are used, with γ_{ij}=2є_{ij}.
This element is primarily aimed at the modeling of fluids or structures by using the method of particles and forces.
This point-like element has one node with six degrees of freedom. The element is developed at EDF ([873]) to model fragmentation of concrete structures. The discrete element mesh is generated by using a particular geometric padding technique (Jerier 2010) implemented into SpherePadder tool (free software under GNU GPL v2 license) and integrated as a plug-in into SMESH mesher of SALOME plate-form. The DE mesh is available in MED format only. Interactions between these elements allow to model cohesive nature of materials or contact.
Specific element (hexahedron) for Van Leer fluids in 3D.
Specific element (prism) for Van Leer fluids in 3D.
3-node shell element (Discrete Shear Triangle).
It is a thick shell element (Mindlin). Same local frame as COQ3.
The element has 8 components of stress (SIG), organized as follows: σ_{x}^{m}, σ_{y}^{m}, τ_{xy}^{m}, σ_{x}^{b}, σ_{y}^{b}, τ_{xy}^{b}, τ_{xz}, τ_{yz}, where the first three components are the membrane contributions, the second three components are the bending contributions and the last two components are the transverse shear contributions (note that the order in which these last two components are given is opposite to what is usually found in 3D continuum elements, for example). The total strains (EPST) follow the same organization: є_{x}^{m}, є_{y}^{m}, γ_{xy}^{m}, є_{x}^{b}, є_{y}^{b}, γ_{xy}^{b}, γ_{xz}, γ_{yz}. Note that, as concerns the shear strains, the engineering values γ and not the tensor values є are used, with γ_{ij}=2є_{ij}.
3-node shell element (Discrete Kirchhoff Triangle). It is a thick shell element (Mindlin). It has the same local frame as COQ3.
The element has 6 components of stress (SIG), organized as follows: σ_{x}^{m}, σ_{y}^{m}, τ_{xy}^{m}, σ_{x}^{b}, σ_{y}^{b}, τ_{xy}^{b}, where the first three components are the membrane contributions and the second three components are the bending contributions. The total strains (EPST) follow the same organization: є_{x}^{m}, є_{y}^{m}, γ_{xy}^{m}, є_{x}^{b}, є_{y}^{b}, γ_{xy}^{b}. Note that, as concerns the shear strains, the engineering values γ and not the tensor values є are used, with γ_{ij}=2є_{ij}.
8-node thick shell element obtained starting from the 8-node brick. The 2 faces of this element are formed by the nodes: 1, 2, 3, 4 for the first face and 5, 6, 7, 8 for the second face.
This thick shell (Mindlin-Reissner) particle element has one node with five degrees of freedom: 3 translations and 2 rotations.
4-node shell element (Batoz), with 4 integration points in the plane and 5 integration points through the thickness for plasticity.
There are 8 stress components: sigm-x, sigm-y, sigm-xy, sigf-x, sigf-y, sigf-xy, tau-xz, tau-yz.
It is a thick shell element with 4 nodes (BATOZ formulation) which accounts for the non-coplanarity of the four nodes. It is a complete but expensive version of Batoz’s element.
A local frame is defined at each Gauss point: the first vector is tangent to the line (csi=cst.) in the sense from node 1 to node 2, the second vector is the vector product of the first by the vector tangent to the line (eta=cst.) in the sense from node 1 to node 4. The frame is completed so as to be right-handed.
4-node shell element (BATOZ) with 1 integration point in the plane and 5 integration points through the thickness for plasticity.
It is a simplified version of Q4G4 with a single integration point in the plane. An incomplete anti-hourglass stiffness (only in rotation) is implemented; an adjusting coefficient for anti-hourglass can be set using the following syntax:
"OPTI" "HGQ4" hgq4ro
The default value of hgq4ro is 0.018.
The element has 10 components of stress (SIG), organized as follows: σ_{x}^{m}, σ_{y}^{m}, τ_{xy}^{m}, σ_{x}^{b}, σ_{y}^{b}, τ_{xy}^{b}, τ_{xz}, τ_{yz}, σ_{h}^{1}, σ_{h}^{2}, where the first three components are the membrane contributions, the second three components are the bending contributions, the next two components are the transverse shear contributions (note that the order in which these last two components are given is opposite to what is usually found in 3D continuum elements, for example) and the last two components are anti-hourglassing (pseudo-)stresses. The total strains (EPST) follow the same organization: є_{x}^{m}, є_{y}^{m}, γ_{xy}^{m}, є_{x}^{b}, є_{y}^{b}, γ_{xy}^{b}, γ_{xz}, γ_{yz}, є_{h}^{1}, є_{h}^{2}. Note that, as concerns the shear strains, the engineering values γ and not the tensor values є are used, with γ_{ij}=2є_{ij}.
This element is similar to Q4GR.
The element has 10 components of stress (SIG), organized as follows: σ_{x}^{m}, σ_{y}^{m}, τ_{xy}^{m}, σ_{x}^{b}, σ_{y}^{b}, τ_{xy}^{b}, τ_{xz}, τ_{yz}, σ_{h}^{1}, σ_{h}^{2}, where the first three components are the membrane contributions, the second three components are the bending contributions, the next two components are the transverse shear contributions (note that the order in which these last two components are given is opposite to what is usually found in 3D continuum elements, for example) and the last two components are anti-hourglassing (pseudo-)stresses. The total strains (EPST) follow the same organization: є_{x}^{m}, є_{y}^{m}, γ_{xy}^{m}, є_{x}^{b}, є_{y}^{b}, γ_{xy}^{b}, γ_{xz}, γ_{yz}, є_{h}^{1}, є_{h}^{2}. Note that, as concerns the shear strains, the engineering values γ and not the tensor values є are used, with γ_{ij}=2є_{ij}.
4-node shell element (Batoz), with 4 integration points in the plane and 5 integration points through the thickness for plasticity.
It is a simplified version of Q4G4 with 4 integration points in the plane.
The element has 8 components of stress (SIG), organized as follows: σ_{x}^{m}, σ_{y}^{m}, τ_{xy}^{m}, σ_{x}^{b}, σ_{y}^{b}, τ_{xy}^{b}, τ_{xz}, τ_{yz}, where the first three components are the membrane contributions, the second three components are the bending contributions and the last two components are the transverse shear contributions (note that the order in which these last two components are given is opposite to what is usually found in 3D continuum elements, for example). The total strains (EPST) follow the same organization: є_{x}^{m}, є_{y}^{m}, γ_{xy}^{m}, є_{x}^{b}, є_{y}^{b}, γ_{xy}^{b}, γ_{xz}, γ_{yz}. Note that, as concerns the shear strains, the engineering values γ and not the tensor values є are used, with γ_{ij}=2є_{ij}.
Two-node nonlinear spring element to model paraseismic supports ([883]). This element has no mass and can have a zero length when using RESG material.
The availability of the bushing element family allows to define generalized stiffness and damping between two nodes. The implemented model provides a first type of element, BSHT, with only translation degrees of freedom (available both in 2D and in 3D), and a second type, BSHR, with rotational degrees of freedom too.
All the characteristics of the bushing element are defined using "JOINT PROPERTIES" material type.
This element is used to connect a slave node to a master edge of shell. Three kinematic constraints are introduced on the translational and rotational degrees of freedom of the slave node. The displacements and rotations of the slave node are linearly interpolated between the two master nodes. These elements are defined in the topology but they work only through the "LIAISON" directive.
This element is used to connect a slave node to a master edge of element. It is the same as for the SH3D element except that there is no constraint on rotations. These elements are defined in the topology but they work only through the "LIAISON" directive.
This element is used in order to glue one slave node to a master face. The master face is triangular in the case of the MAP3 and quadrangular in the case of the MAP4. 3 kinematic constraints are introduced in order to impose the translation dof of the slave node. These elements can be used in order to glue 2 volumic meshes. These elements are defined in the topology but they work only through the "LIAISON" directive.
This element is used in order to glue one slave node to a master shell face. The master face is triangular in the case of the MAP6 and quadrangular in the case of the MAP7. 3 kinematic constraints are introduced in order to impose the translation dof of the slave node and 3 kinematic constraints are added on the rotational dof. These elements can be used in order to glue 2 shell meshes. These elements are defined in the topology but they work only through the "LIAISON" directive.
The INT6 (triangular prism) and INT8 (hexahedron) elements are pure displacement interface elements (also called cohesive elements) dedicated to the modeling of interlayers, separating "standard" structural elements. In the particular case of a composite model, these elements can be considered as representing a homogeneous resin layer ensuring the interlaminar stress transfer between adjacent plies. This approach is most often referred to as "mesoscopic" laminate modeling.
8-node thick shell element obtained starting from the 8-node brick. This element is identical as SHB8 but follows the assumed strain formulation. The 2 faces of this element are formed by the nodes: 1, 2, 3, 4 for the first face and 5, 6, 7, 8 for the second face.
4-node multilayered shell element which is a generalization of the Q4GS element. This element is also multi-material. The number of Gauss point in the thickness depends on the number of plies. The user has to define the total number of Gauss points in the thickness using the parameter NGPZ in COMP (resp. SAND).
3-node multilayered shell element which is a generalization of the DST3 element. This element is also multi-material. The number of Gauss point in the thickness depends on the number of plies. The user has to define the total number of Gauss points in the thickness using the parameter NGPZ in COMP (resp. SAND).
The element has 8 components of stress (SIG), organized as follows: σ_{x}^{m}, σ_{y}^{m}, τ_{xy}^{m}, σ_{x}^{b}, σ_{y}^{b}, τ_{xy}^{b}, τ_{xz}, τ_{yz}, where the first three components are the membrane contributions, the second three components are the bending contributions and the last two components are the transverse shear contributions (note that the order in which these last two components are given is opposite to what is usually found in 3D continuum elements, for example). The total strains (EPST) follow the same organization: є_{x}^{m}, є_{y}^{m}, γ_{xy}^{m}, є_{x}^{b}, є_{y}^{b}, γ_{xy}^{b}, γ_{xz}, γ_{yz}. Note that, as concerns the shear strains, the engineering values γ and not the tensor values є are used, with γ_{ij}=2є_{ij}.
3D cubic finite volume element. The finite volume is defined as cell centred. Several options for the calculation can be chosen with OPTI VFCC.
3D prism finite volume element. The finite volume is defined as cell centred. Several options for the calculation can be chosen with OPTI VFCC.
3D tetrahedral finite volume element. The finite volume is defined as cell centred. Several options for the calculation can be chosen with OPTI VFCC.
3D pyramid finite volume element. The finite volume is defined as cell centred. Several options for the calculation can be chosen with OPTI VFCC.
This element has several nodes with six degrees of freedom. The first node belongs to a shell and the following ones belong to a beam. It allows to use constitutive equations for following two mechanisms :
3 node triangular plate element.
This element can be used to model 3D plates or shells (by plane facet approximation). It is integrated through the thickness. The element can undergo large displacements and large rotations as a whole (rigid body), thanks to a co-rotational formulation, but is limited to small strains. In particular membrane strains should remain small (maximum a few %).
The element has 4 components of stress (SIG), organized as follows: σ_{x}, σ_{y}, τ_{xy}, σ_{z}≈ 0. The total strains (EPST) follow the same organization: є_{x}, є_{y}, γ_{xy}, є_{z}. Note that, as concerns the shear strains, the engineering values γ and not the tensor values є are used, with γ_{ij}=2є_{ij}.
8 node specialised element for compressible fluids.
The same remarks apply as for FLU1 in 2D. The element can be degenerated to represent a prism (6 nodes), a pyramid (4 nodes), or a tetrahedron (4 nodes) by suitable repetition of node numbers in the topology.
This element is used to represent a 2D (or 3D) continuum (usually a fluid) by means of the Particle Finite Element method (PFEM).
8 node brick for advection-diffusion problems.
This element is used to solve advection-diffusion problems in incompressible fluids with heat transfer according to JRC models.
4-node boundary condition for the CQD4.
These elements must be attached directly to the CQD4, i.e., they share the same nodes.
9-node boundary condition for the CQD9.
These elements must be attached directly to the CQD9, i.e., they share the same nodes.
4-node tetrahedron for compressible fluids. Is an alternative to the degeneratable FLU3 hexahedron.
5-node pyramid for compressible fluids. Is an alternative to the degeneratable FLU3 hexahedron.
6-node prism for compressible fluids. Is an alternative to the degeneratable FLU3 hexahedron.
8-node hexahedron for compressible fluids. Is an alternative to the degeneratable FLU3 hexahedron.
Boundary conditions of 3 nodes. Recommended for use with COQI triangular shell elements and in general with all 3D Ispra models. This element automatically recognizes the element to which it is attached and uses the most appropriate pressure discretization.
4-node quadrilateral degenerated shell element (Hughes-Liu).
The element has 6 components of stress (SIG), organized as follows: σ_{x}, σ_{y}, τ_{xy}, σ_{z}≈ 0, τ_{yz}, τ_{xz}. The total strains (EPST) follow the same organization: є_{x}, є_{y}, γ_{xy}, є_{z}, γ_{yz}, γ_{xz}. Note that, as concerns the shear strains, the engineering values γ and not the tensor values є are used, with γ_{ij}=2є_{ij}.
9-node quadrilateral degenerated shell element (Hughes-Liu).
The element has 6 components of stress (SIG), organized as follows: σ_{x}, σ_{y}, τ_{xy}, σ_{z}≈ 0, τ_{yz}, τ_{xz}. The total strains (EPST) follow the same organization: є_{x}, є_{y}, γ_{xy}, є_{z}, γ_{yz}, γ_{xz}. Note that, as concerns the shear strains, the engineering values γ and not the tensor values є are used, with γ_{ij}=2є_{ij}.
3-node triangular degenerated shell element (Hughes-Liu).
Similar to CQD4 but with a triangular shape.
The element has 6 components of stress (SIG), organized as follows: σ_{x}, σ_{y}, τ_{xy}, σ_{z}≈ 0, τ_{yz}, τ_{xz}. The total strains (EPST) follow the same organization: є_{x}, є_{y}, γ_{xy}, є_{z}, γ_{yz}, γ_{xz}. Note that, as concerns the shear strains, the engineering values γ and not the tensor values є are used, with γ_{ij}=2є_{ij}.
6-node triangular degenerated shell element (Hughes-Liu).
Similar to CQD9 but with a triangular shape.
The element has 6 components of stress (SIG), organized as follows: σ_{x}, σ_{y}, τ_{xy}, σ_{z}≈ 0, τ_{yz}, τ_{xz}. The total strains (EPST) follow the same organization: є_{x}, є_{y}, γ_{xy}, є_{z}, γ_{yz}, γ_{xz}. Note that, as concerns the shear strains, the engineering values γ and not the tensor values є are used, with γ_{ij}=2є_{ij}.
3-node boundary condition element for CQD3.
6-node boundary condition element for CQD6.
Boundary conditions of 4 nodes.
Recommended for use with 3D Ispra models. This element automatically recognizes the element to which it is attached and uses the most appropriate pressure discretization.
Finite-volumes: 4-node tetrahedron for multicomponent flows. This element is part of the models developed by the CESI team (formerly at ENEL, Milano) in collaboration with JRC. For more information on this element, see reference [135].
Finite-volumes: 5-node pyramid for multicomponent flows. This element is part of the models developed by the CESI team (formerly at ENEL, Milano) in collaboration with JRC. For more information on this element, see reference [135].
Finite-volumes: 6-node prism for multicomponent flows. This element is part of the models developed by the CESI team (formerly at ENEL, Milano) in collaboration with JRC. For more information on this element, see reference [135].
Finite-volumes: 8-node hexahedron for multicomponent flows. This element is part of the models developed by the CESI team (formerly at ENEL, Milano) in collaboration with JRC. For more information on this element, see reference [135].
Finite-volumes: 8-node hexahedral MACRO spectral element. This element is part of the models developed by the CESI team (formerly at ENEL, Milano) in collaboration with JRC.
The integration points coincide with the Gauss-Lobatto-Legendre points and are determined by specifying the MICRO spectral elements S38.
8-node hexahedral MICRO spectral element.
This element is used only to specify ’internal’ nodes of an MS38.
This is a specialized element for the representation of cables in 3D space, in conjunction with the FUNE material (it resists only in traction, not in compression). When used with the VM23 material, it represents a bar (which resists both in traction and in compression). The element is large-strain.
The element has 4 components of stress (SIG), organized as follows: σ_{x}, σ_{y}≈ 0, τ_{xy}=0, σ_{z}≈ 0. The total strains (EPST) follow the same organization: є_{x}, є_{y}, γ_{xy}=0, є_{z}.
1-node debris particle element.
This is a specialized element for the representation of flying debris, as e.g. resulting from an explosion or an impact, by means of spherical particles. It may be used both in 2D and in 3D.
This element can be used for precise modelling of continua. It can undergo arbitrarily large deformations. Since it is underintegrated, it is locking-free, but it may occasionally suffer from mechanisms if boundary conditions are too loose. In such cases, use of the C273 element (which, however, is more expensive) is recommended.
The element has 6 components of stress (SIG), organized as follows: σ_{x}, σ_{y}, τ_{xy}, σ_{z}, τ_{yz}, τ_{xz}. The total strains (EPST) follow the same organization: є_{x}, є_{y}, γ_{xy}, є_{z}, γ_{yz}, γ_{xz}. Note that, as concerns the shear strains, the engineering values γ and not the tensor values є are used, with γ_{ij}=2є_{ij}.
This is the fully-integrated version of the C272 element. Its use is only recommended when mechanisms might occur.
The element has 6 components of stress (SIG), organized as follows: σ_{x}, σ_{y}, τ_{xy}, σ_{z}, τ_{yz}, τ_{xz}. The total strains (EPST) follow the same organization: є_{x}, є_{y}, γ_{xy}, є_{z}, γ_{yz}, γ_{xz}. Note that, as concerns the shear strains, the engineering values γ and not the tensor values є are used, with γ_{ij}=2є_{ij}.
9-node boundary condition element for C272.
9-node boundary condition element for C273.
8-node hexahedron with reduced spatial integration (1 Gauss Point). This element can be used for precise modelling of continua. It can undergo arbitrarily large deformations. Since it is underintegrated, it is locking-free, but it may suffer from mechanisms. In such cases, use of the C82L element (which, however, is more expensive) is recommended.
The element has 6 components of stress (SIG), organized as follows: σ_{x}, σ_{y}, τ_{xy}, σ_{z}, τ_{yz}, τ_{xz}. The total strains (EPST) follow the same organization: є_{x}, є_{y}, γ_{xy}, є_{z}, γ_{yz}, γ_{xz}. Note that, as concerns the shear strains, the engineering values γ and not the tensor values є are used, with γ_{ij}=2є_{ij}.
This is the fully-integrated version (8 Gauss Points) of the C81L element. Its use is recommended when mechanisms might occur.
The element has 6 components of stress (SIG), organized as follows: σ_{x}, σ_{y}, τ_{xy}, σ_{z}, τ_{yz}, τ_{xz}. The total strains (EPST) follow the same organization: є_{x}, є_{y}, γ_{xy}, є_{z}, γ_{yz}, γ_{xz}. Note that, as concerns the shear strains, the engineering values γ and not the tensor values є are used, with γ_{ij}=2є_{ij}.
Some shell elements developed at Ispra may be defined as
a sandwich (an assembly) composed
of several layers, each one having its own material.
The usual hypothesis
that fibers (straight lines across the thickness of an
undeformed shell)
remain straight during deformation is retained. The fiber may or
may not be/remain normal to some ‘mean’ or ‘reference’ shell surface
depending on the theory (Kirchhoff or Mindlin) assumed, i.e. on
the fact that transverse shear strains are taken into account or not.
As a consequence of fibers remaining straight, the deformation assumes
a simple pattern through the thickness. In sandwich elements the
state of stress may be discontinuous at layer interfaces because the
different materials have in general different properties.
No detachment (delamination) of the various layers is modelled
at present.
These models are useful e.g. for representing reinforced concrete
structures, or other composite materials (sandwich structures).
For the moment, this feature is available for elements of
type ED01 in 2D and elements of type COQI, CQD3, CQD4, CQD6, CQD9,
T3MC, Q4MC, Q4GS, Q4GR, QPPS, T3GS, DKT3 in 3D.
In order to use these models, see the SAND directives in the
Geometry (page C.45) and in the Materials (page C.1110) Sections
of the manual.
When using sandwich elements, the number of layers and of
integration points through the thickness in each layer is specified
by the user and may therefore vary from test case to test case.
In order to facilitate the use of these elements, the following
rule has been chosen:
For sandwich elements, the numbering of the integration points proceeds along each fiber (through the thickness) first, and from the lower to the upper part of the fiber
The lower and upper element surfaces are defined by element numbering
and the right-hand rule, as usual in EUROPLEXUS. The above numbering
scheme is called ‘fiber-first’, as opposed to ‘lamina-first’
numbering schemes.
As an example, consider an element with two fibers, i.e. two
integration stations in the element’s plane (sometimes called lamina)
and 5 integration points through the thickness. Then, the points
numbered 1 to 5 belong to the first fiber, while points 6 to 10
belong to the second fiber. Furthermore, points 1 and 6 are the bottom
ones, 3 and 8 the middle ones and 5 and 10 the top ones, and so on.
For ease of reference, the precise numbering schemes for elements
susceptible of being multi-layered is given below.
The numbering scheme is fiber-first (i.e. identical) for both
the old (until August 1995) and the new (homogeneous or multilayered)
element.
The unlayered element used until August 1995
an unusual numbering rule
where the outer integration points were numbered first, then the
intermediate points and finally a (single) point in the mean surface
(see the Technical Note: “A Triangular Plate Element for the
Nonlinear Dynamic Analysis of Thin 3D Structural Components”,
reference [87]).
The element had 13 points altogether.
The new numbering rule is fiber-first, and is the same for both the
unlayered and the layered element. For the unlayered element, 3 fibers
of 5 points each (15 points altogether) are assumed, while in the
multilayer element the fibers are still 3 but the number of points
through the thickness may vary.
In the versions before August 1995,
(unlayered element) a ‘lamina-first’ numbering rule was
assumed. Along each lamina, points were numbered along the η
direction first, then along the ξ direction (these directions
as well as the lower and upper faces of the elements
are uniquely defined by the numbering of the element nodes).
The number of points through the thickness was chosen by
the user.
In the current version, for both the homogeneous and
the multilayer elements, integration points are numbered
fiber-first and of course the number of points through the thickness
is still variable.
Those element are a generalization of the Q4GS and DST3 elements. The number of total Gauss point through the thickness must be defined with the NPGZ parameter in the dimensioning section.