Previous Up Next

3  SPATIAL DISCRETIZATION (ELEMENT TYPES)

INT.80


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:

3.1  ELEMENT TYPES


Object:

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.


Remark:

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.

3.1.1  1-D ELEMENTS

The various elements available in 1D are presented below.

num.NameDevGibinpt dofngp Remarks
22TUBESEG2CEA211fluid only (rigid tube)
23TUYASEG2CEA272tube coupled with FSI
24CL1DPOI1CEA111fluid boundary condition
25BIFUSUPECEA1:971bifurcation junction
26CAVISUPECEA1:911cavity junction
31CLTUPOI1CEA171boundary condition with FSI
44ED1DSEG2JRC2111D/2D-3D structural coupling
146BRECSEG2CEA271pipeline rupture
147TUVFSEG2CEA211rigid tube (1D vfcc)
148TYVFSEG2CEA271tuvf coupled with FSI (1D vfcc)
149BIVFSEG2CEA211bifurcation junction (1D vfcc)
150CAVFSEG2CEA1:911cavity 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:


TUBE

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).


CL1D

This element allows to introduce the different boundary conditions or localised singularities, in a pipeline meshed by elements of type "TUBE".


CAVI

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.


BIFU

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.


TUYA

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”.


CLTU

Similarly to “CL1D”, this element further allows to introduce coupled boundary conditions of the fluid-structure type (e.g. a closed pipe end).


BREC

This element allows to model a pipeline rupture. Before the optional rupture instant, this element behaves like a bifurcation.


TUVF

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).


TYVF

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”.


BIVF

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.


Warning:

The BIVF element can be used only with 2 branches of fixed pipeline at the moment (tuvf element).


CAVF

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.


Warning:

The 1D finite volume element are under development and testing at CEA and EDF and should therefore be used with great care.


ED1D

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:

  1. The multi-D part of the model is meshed as usual and an 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.
  2. Each 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.
  3. All 1-D parts of the model are represented in a single 1-D model, for which a separate input data set has to be provided.
  4. When more than one 1-D part is present, each one of these will form a separate ’level’ in the 1-D model (see the EURDYN-1D manual for the definition of level).
  5. In setting up the 1-D model, the abscissa of each level should be oriented from the interface point toward the outside of the multi-D body. Thus, the interface node is always the first one (or the ‘left’ node, according to EDURDYN-1D conventions) of each level.
  6. Each ED1D element should be assigned a different VM1D material (see page C.220) and the "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:

        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.

        TF < TEND < FINTIM

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.

3.1.2  2-D ELEMENTS

INT.90

The various elements available in 2D are presented below.


num.NameGibiDevnpt dofngp Remarks
1COQUSEG2CEA232thin shell
2TRIATRI3CEA321triangle
3BARRSEG2CEA221bar (membrane only)
4PONCPOI1CEA121circular bar(axisym.)
5MEMBSEG2CEA221’virole’ in membrane (axisym.)
7CL2DSEG2CEA221boundary conditions
8CAR1QUA4CEA421quadrangle with 1 Gauss pt.
9CAR4QUA4CEA424quadrangle with 4 Gauss pt.
10COQCSEG2CEA231thin shell with shear
15FS2DRAC2CEA421F.S. coupling
28PMAT2DPOI1CEA121material point
38Q92QUA8JRC9249-node quadrilateral
39Q93QUA8JRC9299-node quadrilateral
42CL23SEG3JRC3223-node b.c.s
43ED01SEG2JRC2310beam/conical-shell
45TVL1TRI3CEA321Van Leer triangle
46CVL1QUA4CEA421Van Leer quadrangle
49Q92AQUA8JRC924Q92 on symmetry axis
52FLU1QUA4JRC421fluid quadrilateral
54PFEM2DPOI1JRC121particle finite element
56ED41SEG2JRC4310old version of ED01
58ADQ4QUA4JRC421advection-diffusion quadrilateral
64FL23TRI3JRC321fluid triangle
65FL24QUA4JRC421fluid quadrilateral
70CL22SEG2JRC2222-node b.c.s
71Q41QUA4JRC421ALE structural quadrilateral
72Q42QUA4JRC424ALE structural quadrilateral
73Q41NQUA4JRC421ALE structural quadrilateral
74Q42NQUA4JRC424ALE structural quadrilateral
75Q41LQUA4JRC421Lagr. structural quadrilateral
76Q42LQUA4JRC424Lagr. structural quadrilateral
77Q95QUA8JRC924test version of Q92
97MC23TRI3JRC321finite volume fluid triangle
98MC24QUA4JRC421finite volume fluid quadrilateral
100Q42GQUA4JRC424ALE structural quadrilateral
105MS24QUA4JRC421spectral "macro" quadrilateral
106S24QUA4JRC421spectral "micro" quadrilateral
109FUN2SEG2JRC221cable element
114BSHT2DSEG2CEA22-bushing with translational dof
118MAP2—-CEA32-Point on solid edge
121MAP5—-CEA32-Point on 2D shell
124INT4—-CEA422quadrilateral interface element
131T3VFTRI3CEA321triangle finite volume
132Q4VFQUA4CEA421quadrangle finite volume
140DEBR2DPOI1JRC12-debris particle
 

The specifications for these elements are given hereafter:


COQU

Reference element for all calculations with 2D thin shells.


TRIA

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.


BARR

This element is intended for the modeling of steel reinforcement in concrete structures, or of bars that work only in traction-compression.


PONC

This element should only be used to model circular steel reinforcement in axisymmetric concrete structures.


MEMB

This element is similar to COQU, but has a purely membrane behaviour.


CL2D

This element allows to specify a condition of absorbing medium or an impedance.


CAR1

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.


CAR4

This element is recommended for elastoplastic solids.

The element has 4 components of stress (SIG) and strain (EPST), organized as follows.


COQC

Simpler than "COQUE", it also enables to evaluate the shear, if this is not too large.


FS2D

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).


PMAT

This element is particularly aimed at modeling rigid projectiles, in connection with the directive "IMPACT". It can also be used to specify added masses.


TVL1

This element has been developed for Van Leer fluids.


CVL1

Similarly to TVL1, this element has been developed for Van Leer fluids.


BSHT

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.


MAP2

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".


MAP5

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".


INT4

The INT4 element is a quadrilateral pure displacement interface element (sometimes called cohesive 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.


T3VF

2D triangle finite volume element. The finite volume is defined as cell centred. Several options for the calculation can be chosen with OPTI VFCC.


Q4VF

2D quadrangle finite volume element. The finite volume is defined as cell centred. Several options for the calculation can be chosen with OPTI VFCC.


Q92

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.


Q93

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.


CL23

This element is mainly used to specify uniform pressure conditions acting on the boundaries of quadratic elements of type Q92, Q93 or Q92A.


ED01

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 γij=2єij.


Q92A

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.


FLU1

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.


PFEM

This element is used to represent a 2D (or 3D) continuum (usually a fluid) by means of the Particle Finite Element method (PFEM).


ED41

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.


ADQ4

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.


FL23

3-node triangle for compressible fluids. This is an alternative to the degeneratable FLU1 quadrilateral.


FL24

4-node quadrilateral for compressible fluids. This is an alternative to the degeneratable FLU1 quadrilateral.


CL22

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.


Q41

4-node quadrilateral for structural ALE calculations with reduced integration.

The element has 4 components of stress (SIG) and strain (EPST), organized as follows.


Q42

4-node quadrilateral for structural ALE calculations with full integration.

The element has 4 components of stress (SIG) and strain (EPST), organized as follows.


Q41N

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.


Q42N

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.


Q41L

4-node quadrilateral for Lagrangian calculations with reduced integration.

The element has 4 components of stress (SIG) and strain (EPST), organized as follows.


Q42L

4-node quadrilateral for Lagrangian calculations with full integration.

The element has 4 components of stress (SIG) and strain (EPST), organized as follows.


Q95

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.


MC23

3-node finite volume triangle for multicomponent flows.


MC24

4-node finite volume quadrilateral for multicomponent flows.


Q42G

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.


MS24

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.


S24

4-node quadrilateral MICRO spectral element This element is used only to specify ’internal’ nodes of an MS24.


FUN2

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: σx, σy≈ 0, τxy=0, σz≈ 0. The total strains (EPST) follow the same organization: єx, єy, γxy=0, єz.


DEBR

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.

3.1.3  3-D ELEMENTS

INT.100

The various elements available in 3D are presented below.


num.NameGibiDevnpt dofngp Remarks
57ADC8CUB8JRC831advection-diffusion brick
32APPUPOI1CEA161support
130ASHB—-CEA835assumed strain thick shell
79BILLPOI1CEA131particle element (NABOR and SPH)
19BR3DSEG2CEA231bar
115BSHR—-CEA26bushing with trans. and rot. dof
114BSHT—-CEA23bushing with translational dof
144C272CU27JRC273827-node cube
145C273CU27JRC2732727-node cube
155C81LCUB8JRC8318-node cube
156C82LCUB8JRC8388-node cube
62CL32QUA4JRC464b.c.s for CQD4
63CL33QUA9JRC969b.c.s for CQD9
18CL3DQUA4CEA431bound. cond. (4-node face)
78CL3ITRI3JRC3313-node b.c.s
99CL3QQUA4JRC4314-node b.c.s
29CL3TTRI3CEA331bound. cond. (3-node face)
151CL92QUA9JRC9349-node (3D) b.c. for C272
152CL93QUA9JRC9399-node (3D) b.c. for C273
95CLD3TRI3JRC363b.c.s for CQD3
96CLD6TRI6JRC664b.c.s for CQD6
47CMC3TRI3CEA362multilayer shell
12COQ3TRI3CEA361triangular thin shell
14COQ4QUA4CEA464quadrangular thin shell
40COQITRI3JRC3615triangular shell (small strain)
93CQD3TRI3JRC3615degenerated shell (Hughes-Liu)
91CQD4QUA4JRC4620degenerated shell (Hughes-Liu)
94CQD6TRI6JRC6620degenerated shell (Hughes-Liu)
92CQD9QUA9JRC9645degenerated shell (Hughes-Liu)
13CUB6CUB8CEA836brick with 6 Gauss pt
30CUB8CUB8CEA838brick with 8 Gauss pt
6CUBBCUB8CEA838brick based on B-bar method
11CUBECUB8CEA831brick with 1 Gauss pt
133CUVFCUB8CEA831cube finite volume
81CUVLCUB8CEA831Van Leer cube
140DEBRPOI1JRC13-debris particle
84DKT3TRI3CEA3615shell (Mindlin)
83DST3TRI3CEA3615shell (Discrete Shear Triangle)
80ELDIPOI1CEA161discrete element
66FL34TET4JRC431fluid tetrahedron
67FL35PYR5JRC531fluid pyramid
68FL36PRI6JRC631fluid prism
69FL38CUB8JRC831fluid hexahedron
53FLU3CUB8JRC831fluid brick
16FS3DRAC3CEA831F.S. connection (4-node face)
48FS3TPRI6CEA631F.S. connection (3-node face)
110FUN3SEG2JRC231cable element
153LIGRSUPECEA2*6-mechanism (articulated systems)
125INT6—-CEA631triangular prism interface element
126INT8—-CEA834hexahedron interface element
119MAP3—-CEA43point on a triangular facet
120MAP4—-CEA53point on a quadrangular facet
122MAP6—-CEA46point on a triangular shell facet
123MAP7—-CEA56point on a quadrangular shell facet
101MC34TET4JRC431finite volume tetrahedron
102MC35PYR5JRC531finite volume pyramid
103MC36PRI6JRC631finite volume prism
104MC38CUB8JRC831finite volume hexahedron
33MECASEG2CEA261mechanism (articulated systems)
128MOY4—-CEA43node to element mean connector
129MOY5—-CEA53node to element mean connector
107MS38CUB8JRC831spectral "macro" quadrilateral
54PFEMPOI1JRC131particle finite element
28PMATPOI1CEA131material point
17POUTSEG2CEA262beam
20PR6PRI6CEA636prism with 6 Gauss pt
27PRISPRI6CEA631prism with 1 Gauss pt
134PRVFPRI6CEA631prism finite volume
82PRVLPRI6CEA631Van Leer prism
136PYVFPYR4CEA531pyramid finite volume
138Q4MCQUA4CEA46-multilayered quadrangular shell
90Q4G4QUA4CEA464shell (Batoz)
111Q4GRQUA4CEA465idem Q4G4 (simplified : 1 pt)
112Q4GSQUA4CEA4620idem Q4G4 (simplified : 4 pts)
35QPPSQUA4CEA465similar to Q4GR
113RL3DSEG2CEA231two-node spring
108S38CUB8JRC831spectral "micro" quadrilateral
117SH3D—-CEA36node to shell connector
127SH3V—-CEA834node to element connector
85SHB8CUB8CEA835thick shell
89SPHCPOI1CEA161particle element (thick shell)
139T3MCTRI3CEA46-multilayered triangular shell
51T3GSTRI3CEA365shell (Reissner-Mindlin)
21TETRTET4CEA431tetrahedron with 1 Gauss pt
135TEVFTET4CEA431tetrahedron finite volume
41TUBMSUPECEA1*3*1connection 3D-1D
116TUYMSUPECEA1*3*1connection 3D-1D
 


The specifications for these elements are given hereafter:


CUBB

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.


CUBE

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): σx, σy, σz, τxy, τyz, τxz. The total strains (EPST) follow the same organization: єx, єy, єz, γxy, γyz, γxz. Note that, as concerns the shear strains, the engineering values γ and not the tensor values є are used, with γij=2єij.


COQ3

This element must be used with care. In order to obtain good results make sure to use a symmetric mesh (ex: British flag).


CUB6

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: σx, σy, σz, τxy, τyz, τxz. The total strains (EPST) follow the same organization: єx, єy, єz, γxy, γyz, γxz. Note that, as concerns the shear strains, the engineering values γ and not the tensor values є are used, with γij=2єij.


COQ4

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.


FS3D

Same remarks as for FS2D.


POUT

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).


CL3D

Same remarks as for CL2D.


BR3D

This element is mainly used to model concrete rebars or any other beam submitted to a simple tension.


PR6

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: σx, σy, σz, τxy, τyz, τxz. The total strains (EPST) follow the same organization: єx, єy, єz, γxy, γyz, γxz. Note that, as concerns the shear strains, the engineering values γ and not the tensor values є are used, with γij=2єij.


TETR

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): σx, σy, σz, τxy, τyz, τxz. The total strains (EPST) follow the same organization: єx, єy, єz, γxy, γyz, γxz. Note that, as concerns the shear strains, the engineering values γ and not the tensor values є are used, with γij=2єij.


PRIS

This prismatic element is especially used for fluids (see CUBE).

The element has 6 components of stress (SIG), organized as follows (for solid materials): σx, σy, σz, τxy, τyz, τxz. The total strains (EPST) follow the same organization: єx, єy, єz, γxy, γyz, γxz. Note that, as concerns the shear strains, the engineering values γ and not the tensor values є are used, with γij=2єij.


PMAT

Primarily, this element enables the modelling of rigid missiles in connection with the keyword "IMPACT"; but it also enables the introduction of added masses.


CL3T

Same remarks as for CL2D.


CUB8

Solid element recommended for elasto-plastic computations (no hourglassing phenomena).

The element has 6 components of stress (SIG), organized as follows: σx, σy, σz, τxy, τyz, τxz. The total strains (EPST) follow the same organization: єx, єy, єz, γxy, γyz, γxz. Note that, as concerns the shear strains, the engineering values γ and not the tensor values є are used, with γij=2єij.


APPU

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.


MECA

This element has two nodes with six degrees of freedom. It allows to use constitutive equations for mechanisms (articulations, etc.).


TUBM

Connection 3D-1D. Consult the corresponding ‘liaison’ (connection).


TUYM

Connection 3D-1D for moving meshes (ALE). Consult the corresponding ‘liaison’ (connection).


CMC3

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).


FS3T

Same remarks as for FS2D.


T3GS

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: σxm, σym, τxym, σxb, σyb, τxyb, τxz, τyz, 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: єxm, єym, γxym, єxb, єyb, γxyb, γxz, γyz. Note that, as concerns the shear strains, the engineering values γ and not the tensor values є are used, with γij=2єij.


BILL

This element is primarily aimed at the modeling of fluids or structures by using the method of particles and forces.


ELDI

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.


CUVL

Specific element (hexahedron) for Van Leer fluids in 3D.


PRVL

Specific element (prism) for Van Leer fluids in 3D.


DST3

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: σxm, σym, τxym, σxb, σyb, τxyb, τxz, τyz, 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: єxm, єym, γxym, єxb, єyb, γxyb, γxz, γyz. Note that, as concerns the shear strains, the engineering values γ and not the tensor values є are used, with γij=2єij.


DKT3

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: σxm, σym, τxym, σxb, σyb, τxyb, 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: єxm, єym, γxym, єxb, єyb, γxyb. Note that, as concerns the shear strains, the engineering values γ and not the tensor values є are used, with γij=2єij.


SHB8

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.


SPHC

This thick shell (Mindlin-Reissner) particle element has one node with five degrees of freedom: 3 translations and 2 rotations.


Q4G4

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.


Q4GR

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: σxm, σym, τxym, σxb, σyb, τxyb, τxz, τyz, σh1, σh2, 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: єxm, єym, γxym, єxb, єyb, γxyb, γxz, γyz, єh1, єh2. Note that, as concerns the shear strains, the engineering values γ and not the tensor values є are used, with γij=2єij.


QPPS

This element is similar to Q4GR.

The element has 10 components of stress (SIG), organized as follows: σxm, σym, τxym, σxb, σyb, τxyb, τxz, τyz, σh1, σh2, 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: єxm, єym, γxym, єxb, єyb, γxyb, γxz, γyz, єh1, єh2. Note that, as concerns the shear strains, the engineering values γ and not the tensor values є are used, with γij=2єij.


Q4GS

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: σxm, σym, τxym, σxb, σyb, τxyb, τxz, τyz, 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: єxm, єym, γxym, єxb, єyb, γxyb, γxz, γyz. Note that, as concerns the shear strains, the engineering values γ and not the tensor values є are used, with γij=2єij.


RL3D

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.


BSHT and BSHR

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.


SH3D

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.


SH3V

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.


MAP3 and MAP4

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.


MAP6 and MAP7

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.


INT6 and INT8

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.


ASHB

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.


Q4MC

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).


T3MC

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: σxm, σym, τxym, σxb, σyb, τxyb, τxz, τyz, 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: єxm, єym, γxym, єxb, єyb, γxyb, γxz, γyz. Note that, as concerns the shear strains, the engineering values γ and not the tensor values є are used, with γij=2єij.


CUVF

3D cubic finite volume element. The finite volume is defined as cell centred. Several options for the calculation can be chosen with OPTI VFCC.


PRVF

3D prism finite volume element. The finite volume is defined as cell centred. Several options for the calculation can be chosen with OPTI VFCC.


TEVF

3D tetrahedral finite volume element. The finite volume is defined as cell centred. Several options for the calculation can be chosen with OPTI VFCC.


PYVF

3D pyramid finite volume element. The finite volume is defined as cell centred. Several options for the calculation can be chosen with OPTI VFCC.


LIGR

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 :


COQI

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: σx, σy, τxy, σz≈ 0. The total strains (EPST) follow the same organization: єx, єy, γxy, єz. Note that, as concerns the shear strains, the engineering values γ and not the tensor values є are used, with γij=2єij.


FLU3

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.


PFEM

This element is used to represent a 2D (or 3D) continuum (usually a fluid) by means of the Particle Finite Element method (PFEM).


ADC8

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.


CL32

4-node boundary condition for the CQD4.

These elements must be attached directly to the CQD4, i.e., they share the same nodes.


CL33

9-node boundary condition for the CQD9.

These elements must be attached directly to the CQD9, i.e., they share the same nodes.


FL34

4-node tetrahedron for compressible fluids. Is an alternative to the degeneratable FLU3 hexahedron.


FL35

5-node pyramid for compressible fluids. Is an alternative to the degeneratable FLU3 hexahedron.


FL36

6-node prism for compressible fluids. Is an alternative to the degeneratable FLU3 hexahedron.


FL38

8-node hexahedron for compressible fluids. Is an alternative to the degeneratable FLU3 hexahedron.


CL3I

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.


CQD4

4-node quadrilateral degenerated shell element (Hughes-Liu).

The element has 6 components of stress (SIG), organized as follows: σx, σy, τxy, σz≈ 0, τyz, τxz. The total strains (EPST) follow the same organization: єx, єy, γxy, єz, γyz, γxz. Note that, as concerns the shear strains, the engineering values γ and not the tensor values є are used, with γij=2єij.


CQD9

9-node quadrilateral degenerated shell element (Hughes-Liu).

The element has 6 components of stress (SIG), organized as follows: σx, σy, τxy, σz≈ 0, τyz, τxz. The total strains (EPST) follow the same organization: єx, єy, γxy, єz, γyz, γxz. Note that, as concerns the shear strains, the engineering values γ and not the tensor values є are used, with γij=2єij.


CQD3

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: σx, σy, τxy, σz≈ 0, τyz, τxz. The total strains (EPST) follow the same organization: єx, єy, γxy, єz, γyz, γxz. Note that, as concerns the shear strains, the engineering values γ and not the tensor values є are used, with γij=2єij.


CQD6

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: σx, σy, τxy, σz≈ 0, τyz, τxz. The total strains (EPST) follow the same organization: єx, єy, γxy, єz, γyz, γxz. Note that, as concerns the shear strains, the engineering values γ and not the tensor values є are used, with γij=2єij.


CLD3

3-node boundary condition element for CQD3.


CLD6

6-node boundary condition element for CQD6.


CL3Q

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.


MC34

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].


MC35

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].


MC36

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].


MC38

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].


MS38

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.


S38

8-node hexahedral MICRO spectral element.

This element is used only to specify ’internal’ nodes of an MS38.


FUN3

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: σx, σy≈ 0, τxy=0, σz≈ 0. The total strains (EPST) follow the same organization: єx, єy, γxy=0, єz.


DEBR

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.


C272

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: σx, σy, τxy, σz, τyz, τxz. The total strains (EPST) follow the same organization: єx, єy, γxy, єz, γyz, γxz. Note that, as concerns the shear strains, the engineering values γ and not the tensor values є are used, with γij=2єij.


C273

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: σx, σy, τxy, σz, τyz, τxz. The total strains (EPST) follow the same organization: єx, єy, γxy, єz, γyz, γxz. Note that, as concerns the shear strains, the engineering values γ and not the tensor values є are used, with γij=2єij.


CL92

9-node boundary condition element for C272.


CL93

9-node boundary condition element for C273.


C81L

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: σx, σy, τxy, σz, τyz, τxz. The total strains (EPST) follow the same organization: єx, єy, γxy, єz, γyz, γxz. Note that, as concerns the shear strains, the engineering values γ and not the tensor values є are used, with γij=2єij.


C82L

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: σx, σy, τxy, σz, τyz, τxz. The total strains (EPST) follow the same organization: єx, єy, γxy, єz, γyz, γxz. Note that, as concerns the shear strains, the engineering values γ and not the tensor values є are used, with γij=2єij.

3.2  SANDWICH (MULTI-LAYER) ELEMENTS

INT.110


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.

3.2.1  LOCATION AND NUMBER OF THE INTEGRATION POINTS


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.


ED01 element


The numbering scheme is fiber-first (i.e. identical) for both the old (until August 1995) and the new (homogeneous or multilayered) element.


COQI 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.


CQDx elements


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.


Q4MC and T3MC elements


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.


Previous Up Next