4.2 Example 2: Link modeled with beam elements

This example models a simple flexible link component using three-dimensional beam elements.

To perform the analysis for the link modeled with beam elements:

Enter the following command to extract the input files from the compressed archive files provided with the Abaqus release:
```
abaqus fetch job=adams_ex2
```
Enter the following command to execute the Abaqus analysis:
```
abaqus job=adams_ex2
```
Enter the following command to execute the Abaqus Interface for MSC.ADAMS and translate the results file generated in the Abaqus analysis to a modal neutral file for use with ADAMS/Flex:
```
abaqus adams job=adams_ex2
```

The primary difference between the beam model and the solid model is that the beam model uses only 10 B31 elements (11 nodes). Because the beam elements have both displacement and rotational degrees of freedom at their nodes, no multi-point constraints are needed to connect the link to other MSC.ADAMS components. The rest of the model is essentially identical to the solid model of the link.

The first eight nonzero frequencies for the unconstrained model are shown in Table 4–3.

Table 4–3 Nonzero frequencies for the beam link model that are used by ADAMS/Flex.

Frequency, Hz
205
555
610
1070
1618
1742
1775
2568

These frequencies are close to those of the solid model of the link. Although the computational cost in Abaqus is much less for this model than for the solid model, the computational costs in MSC.ADAMS for the two models are very similar because both models have 32 modes (12 constraint modes and 20 fixed-interface vibration modes).

The Abaqus input file for the beam model, adams_ex2.inp, is shown below.

*HEADING
Link modeled with B31 beam elements
**  ----------------------------------------------
**
**               NODE DEFINITION
**
*NODE, nset=nall
**
         1,0.000000000E+00,0.000000000E+00,0.000000000E+00
         2,5.000000000E-02,0.000000000E+00,0.000000000E+00
         3,1.000000000E-01,0.000000000E+00,0.000000000E+00
         4,1.500000000E-01,0.000000000E+00,0.000000000E+00
         5,2.000000000E-01,0.000000000E+00,0.000000000E+00
         6,2.500000000E-01,0.000000000E+00,0.000000000E+00
         7,3.000000000E-01,0.000000000E+00,0.000000000E+00
         8,3.500000000E-01,0.000000000E+00,0.000000000E+00
         9,4.000000000E-01,0.000000000E+00,0.000000000E+00
        10,4.500000000E-01,0.000000000E+00,0.000000000E+00
        11,5.000000000E-01,0.000000000E+00,0.000000000E+00
**
**  ----------------------------------------------
**
**               ELEMENT DEFINITION
**
*ELEMENT,TYPE=B31
         1,1,2
         2,2,3
         3,3,4
         4,4,5
         5,5,6
         6,6,7
         7,7,8
         8,8,9
         9,9,10
        10,10,11
**
**  ----------------------------------------------
**
**               ELEMENT PROPERTY DEFINITION
**
*ELSET,ELSET=PROP1
1,2,3,4,5,6,7,8,9,10
**
*BEAM SECTION,ELSET=PROP1,SECTION=RECT,MATERIAL=STEEL,TEMP=GRAD
3.000E-02,1.000E-02
0.000E+00,0.000E+00,-1.000E+00
,
**
**  ----------------------------------------------
**
**               MATERIAL DEFINITION
**
*MATERIAL,NAME=STEEL
*ELASTIC
 2.069999944E+11, 3.000000119E-01,
*DENSITY
 7.800000000E+03,
**
*NSET,NSET=RETNODES
1, 11
**
**  ----------------------------------------------
**
*STEP
*FREQUENCY,EIGENSOLVER=LANCZOS
20,
*BOUNDARY
RETNODES, 1,6
*ELEMENT MATRIX OUTPUT, MASS=YES, ELSET=PROP1
*NODE FILE
U
*END STEP
**
**  ----------------------------------------------
**
**               SUBSTRUCTURE GENERATION
**
*STEP
*SUBSTRUCTURE GENERATE, TYPE=Z1, RECOVERY MATRIX=YES, 
 MASS MATRIX=YES, OVERWRITE
*RETAINED NODAL DOFS, SORTED=NO
RETNODES, 1,6 
*SELECT EIGENMODES,generate
1,20
*SUBSTRUCTURE MATRIX OUTPUT, STIFFNESS=YES, MASS=YES,
 RECOVERY=YES
*END STEP