ConFem Documentation
ConFem Documentation : Keywords for ConFem Input Data : Element Section

10.3 Element Section

$\rightarrow $ https:://concrete-fem.com

The section keyword *ELEMENT has as options

TYPE=<element type>

is mandatory and specifies the element type

ELSET=<name>

is mandatory groups a set of elements of same type into a unit with name <name> which is reference to by other keywords

BONDLAW=<name>

is optional and indicates the element set as embedded in a continuum and connects it to a bond law specified in the material section (optional)
 

implemented for element types T2D2, T2D3, T3D2, T3D3, B23, B23E only, see the following list

 

automatically transforms the above elements into element types T2D2E, T2D3E, T3D2E, T3D3E, B23I, B23EI – which cannot be specified explicitly but only implicitly by the BONDLAW-option

 

automatically generates bond elements

 

of type B2D2E related to T2D2,B23I,
 

of type B2D3E related to T2D3,B23E,
 

of type B3D2E related to T3D2 and

 

of type B3D3E related to T3D3



The data lines describe the following element data

<element number>,

<1st node number>,

<2nd node number>

....



Values have to be separated by commas. The number of nodes which have to be specified depends on the element type. Nodes have to be specified in a counter clockwise direction sequence regarding plate, slab and shell elements.

The whole of these lines form an element set which is referred to by the name specified above. The particular element set is closed with a new section keyword. More element sets may be created starting with the section keyword *ELEMENT.

The following element types can explicitly be specified currently:

   

number

ndof indices

Book Section

internal type index
   

of nodes

see Section 7

  

T1D2   

1D truss / bar

2

1

2.3

1

T2D2   

2D truss / bar

2

1,2

2.3

1

T2D3   

enhanced 2D truss / bar

2+1

1,2 + 1

8.5

1

T3D2   

3D truss / bar

2

1,2,3

-

1

T3D3   

enhanced 3D truss / bar

2+1

1,2,3 +1

-

1

B21   

2D Timoshenko beam

2

1,2,6

4.3.1

11

B21E   

2D enhanced Timoshenko beam

3

1,2,6

4.3.1

11

B23   

2D Bernoulli beam

2

1,2,6

4.3.2

10

B23E   

2D enhanced Bernoulli beam

3

1,2,6

4.3.2

10

CPE3   

2D continuum plane strain

3

1,2

-

2

CPE4   

2D continuum plane strain

4

1,2

2.3

2

CPS3   

2D continuum plane stress

3

1,2

-

2

CPS4   

2D continuum plane stress

4

1,2

2.3

2

C3D8   

3D continuum

8

1,2,3

-

3

SB3   

2D slab

3

3

9.5.2

20

SH3   

3D continuum based shell

3

1,2,3,4,5

 

21

SH4   

3D continuum based shell

4

1,2,3,4,5

10.1-4

21

S1D2   

1D spring

2

1

2.3

99

S2D6   

2D spring

2

1,2,6

-

98



The section keyword *ELEMENT has no own sub-keywords.

1D elements

1D elements are T1D2 and S1D2. Both allow to provide an additional elective – not mandatory – float value following the element number and the two node numbers spanning these elements.

T1D2
This value specifies a uniaxial tensile strength for the respective element to be used with the material model *ELASTICLT, see Section 10.4..In case it is given it overrides the tensile strength specified with the definition of *ELASTICLT. Its major purpose is to specify a stochastic field along T1D2 elements.

S1D2
This value specifies a multiplier for the quantity $t$ in a *SOLID SECTION definition, see Section 10.5. Its major purpose is to consider the length of T1D2 elements connected by the respective S1D2 element to define a bond flow from a circumference definition. The multiplier is chosen with 1 in case it is not explicitly specified.

Embedded elements

Using an option *BONDLAW=<name> transforms the respective element into the same element but connected to an underlying continuum of CP*-elements by a bond law, see the option definitions above.

This bond law has to be defined in the Material section, see Section 10.4, with the sub-keyword *BOND and the same name as defined with the respective options.

Enhanced truss elements

Enhanced truss / bar elements (T2D3, T3D3) include an additional node with a longitudinal displacement degree of freedom only, see Book 8.5. This improves the behavior when the elements are used as embedded elements with the BONDLAW-option. Such an improvement is generally not given with a standalone setup and elements T2D2, T3D2 are recommended therefore.

The additional node has to be defined in the input data *NODE-section and included as 3rd node after the 1st node l.h.s and the 2nd node r.h.s. This 3rd node is not shared by other elements and may have coordinates 0.0, 0.0, 0.0. Anyway, 1st and 2nd node need correct coordinates.

Enhanced beam elements

Enhanced beam elements (B21E,B23E) include an additional node with a longitudinal displacement degree of freedom only, see Book 4.3.1/2. This improves the interpolation behavior with cracked reinforced concrete cross sections.

This node has to be defined in the input data *NODE-section and included as 2nd node in between the 1st node l.h.s and the 3rd node r.h.s. This 2nd node is not shared by other elements and may have coordinates 0.0, 0.0. Anyway, 1st and 3rd node need correct coordinates.

Continuum elements with Strong Discontinuity Approach (SDA)

Continuum elements (CP*3,CP*4,C3D8) are generally – this is also still under construction and may not work seamlessly under all conditions – enabled to regard discontinuous displacement fields according to the Strong Discontinuity Approach, see Book 7.7.

This is coupled to a limited tensile strength of materials and currently implemented for material type *ELASTICLT, see Section 10.4. Continuum elements are extended to corresponding SDA-elements (CP*3 to CP*3S, CP*4 to CP*4S, C3D8 to C3D8S) when some material specific condition is fulfilled. This introduces – on the element level – additional degrees of freedom for the discontinuity geometry which are connected to a traction-separation law defined by the respective material. The corresponding data are described in Section 12.3

Shell elements SH4

Every shell node has a local 3D right-handed cartesian coordinate system, see Fig. 4 and Section 10.1 of Book. It is defined through a director more or less normal to the shell surface. A director defines the cross sectional planes which are assumed to remain straight during a deformation. The other two cartesian system directions define the axes of the rotational degrees of freedom.

\includegraphics[scale=0.70]{Figures/C8_ShellKinemat1}
Figure 4: Nodal shell coordinate system



Furthermore, the node directors co-determine the relations between global and local coordinates in shell integration points. In particular – regarding an integration point –, they co-determine the Jacobian matrix and thus the director of the integration point.

Another local 3D right-handed cartesian coordinate system is used with each integration point director as local $n$-direction. The local $\alpha $-direction is generally derived by the cross product of the director and the global $y$-direction, i.e. it aligns to to the global $x-z$-plane. The local $\beta $-direction is derived from the cross product of the director and and the local $\alpha $-direction.

The material behavior is described with respect to this integration point coordinate system, see Book 10.3. In particular, stress directions and directions of derived normal forces, bending moments and shear forces relate to this coordinate system. The components of $\bf {V}_\alpha ,\, \bf {V}_\beta $ – measured in the global system – are appended to the shell element output, see Section 12.3. This indicates how moments, forces and stresses are acting. The orientation angle of a reinforcement layer – acting uniaxially within the shell surface by definition – refers to $\bf {V}_\alpha $. The orientation angle is measured counterclockwise with the director $\bf {V}_n$ as rotation axis.

$\rightarrow $ https:://concrete-fem.com

ConFem Documentation