9.14    Nodal Link Element

 

            The link element is used to connect two nodal points either in translations or rotations in any direction.  The element is defined by two nodes and a single directed axis, by a linear/nonlinear extensional stiffness and damping along the axis, or by a linear/nonlinear rotational stiffness and damping about the axis. The element is essentially a spring or damper which can have either axial or rotational stiffness and damping.  There is no limit to the number of links which can be established between two nodal points to produce the desired effects.

 

            By default a linear spring is assumed.  If nonlinear, a piecewise linear behavior is assumed. The nonlinear spring capabilities of the element are illustrated in Figure 9.14.1a.

 

 

Figure 9.14.1a  Nonlinear Link Element

 

where F = force or moment, and  = displacement or rotation.  The nonlinear curve is assumed piecewise linear and is prescribed by defining various load_levels Fi , and corresponding spring_coefficients Hi  up to 5 load_levels and corresponding spring coefficients can be used.  The element may be prescribed to be elastic or hysteretic, as shown in Figure 9.14.1b. 

 

 

Figure 9.14.1b  Nonlinear Link Element

 

NODAL_LINK

 

 

            Element_name = NODAL_LINK     Kinem = kinem, etc...

                  < material data >

                  < output requests >

                  < connectivity data >

 

 

 

 

9.14.1     Element Group Control Information

 

            Must follow the element name (same data record), and define the control parameters in the following form:    KINEM = kinem, etc...

 

Note    Variable Name                          Type     Default    Description

 

            Kinem                                      integer         [0]       Link condition code

                                                                                                = 0 Translation

                                                                                                = 1 Rotation

 

            Number_of_material_sets       integer         [1]       Number of material sets

 

            File_name                                 string       [none]    File name (optional).  Name must be
                                                                                                enclosed in quotation marks.

 

            Input_format                              list            [*]       Input format

                 keywords / list

 

 

 

9.14.2     Geometric / Material Properties Data (Numat sets)

 

Note       Variable Name                       Type     Default    Description

 

• Keywords Read Method

               Material_set_number            integer       [1]        Material set number  Numat

 

               Modulus_coefficient               real        [0.0]       Spring coefficient H0

 

               Damping_coefficient              real        [0.0]       Damping coefficient c

 

 (1)          Damping_exponent                 real        [0.0]       Damping exponent

 

               Reference_axis

                    n_x                                      real        [0.0]       Component in x_direction

                    n_y                                      real        [0.0]       Component in y_direction

                    n_z                                      real        [0.0]       Component in z_direction

 

               Material_type                        string    [elastic]    Material type selection

                    elastic / hysteretic

 

               Load_level_i                           real        [0.0]       Load level i (i  5)

               Spring_coefficient_i                real        [0.0]       Spring coefficient i (i  5)

 

               Tensile_strength                      real        [0.0]       Tensile failure strength

                                                                                                (only active if  > 0)

 

               Compressive_strength             real        [0.0]       Compressive failure strength

                                                                                                (only active if < 0)

 

• List Read Method

               Geometric data must follow in the form:

                    < n, spring (n), damp (n), n_x (n), n_y (n), n_z (n),
                           mat_type (n), load_level (i,n), spring_coeff (i,n), i = 1, 5 >

                    < terminate with a blank record >.

 

 

Notes/

(1)   The damping coefficient is computed as:

C =

            where  = relative velocity between node 1 and node 2; c = damping_coefficient and

            = damping_exponent.

 

EXAMPLE

DEFINE_ELEMENT_GROUP /

      name = "group_name" /

      element_type = nodal /

      element_name = nodal_link /

      number_of_output_sets = 2 /

      kinem= 1 /

      number_of_material_sets = 1

 

            material_set_number = 1 \

                  modulus_coeff = 1.3+4 \

                  n_x=0.00  n_y=0.00  n_z=1.00 \

                        material_type = hysteretic \

                        load_level_1 = 15.0 \

                        spring_coeff_1 = 5.e+3

 

      Nodal_connectivity

            1          1          1          2

 

      Field_output

            1          0          1          2

 

 

 

9.14.3     Element Nodal Connectivity Data

 

            Consult Section 11 for details; for this element  NEN = 2.

 

 

 

 

9.14.4     Output History Requests

 

FIELD_OUTPUT

 

 

            FIELD_OUTPUT       n,     ng,     ntemp(1),     ntemp(2),    etc...

                  < etc..., terminate with a blank record >.

 

 

Plots of various element response components may be obtained.  Each component requested is plotted versus time.  Plots of this type are useful in providing quick information concerning the time history behavior of important data.  The total number of components to be plotted must equal Number_output_sets, which is defined on the element group control command (see Section 9.1).

 

Note          Variable           Default                  Description

 

(1)                  N                    [0]                      Element number  1 and  Numel

 

(2)                 NG                   [0]                      Generation increment  0

 

(3)           NTEMP(1)             [0]                      Component number  1 and  2

 

               NTEMP(2)             [0]                      Component number  1 and  2

 

 

Notes/

(1)        Element components history output data must be input for elements at which the time history of one or more components is to be plotted. Records need not be read in order.  Terminate with a blank record.

 

(2)        Element components history output data can be generated by employing a two record sequence as follows:

 

                                    Record 1: L,LG,LTEMP(1),LTEMP(2)

                                    Record 2: N,NG,NTEMP(1),NTEMP(2)

 

The output time history requests of all elements

 

                                    L+LG, L+2*LG,..., N-MOD(N-L,LG)

 

(i.e., less than N) are set equal to those of node L.  If LG is blank or zero, no generation takes place between L and N.

 

(3)        Two different  component numbers may be plotted as described above.  The corresponding component numbers and output labels are:

           

              Component Number          Description          Output Label

 

                             1                Displacement /Rotation         DELT

                             2                       Force/Moment                FORC

 

 

 

 

Notes . .