Since this is a transient dynamic analysis, it is natural to consider how the results compare with those obtained using direct integration of the equations of motion. Direct integration can be performed with either implicit (ABAQUS/Standard) or explicit (ABAQUS/Explicit) methods. Here we extend the analysis to use the explicit dynamics procedure.
A direct comparison with the results presented earlier is not possible since the B33 element type and critical damping are not available in ABAQUS/Explicit. Thus, in the ABAQUS/Explicit analysis the element type is changed to B31 and Rayleigh damping is used in place of critical damping.
Copy the Dynamic model to one named explicit. All subsequent changes should be made to the explicit model.
To modify the model:
Delete the modal dynamics step.
Replace the remaining frequency extraction step with an explicit dynamics step, and specify a time period of 0.5 s. In addition, edit the step to use linear geometry (toggle off Nlgeom).
This will result in a linear analysis.
Rename the step to Transient dynamics.
Create two additional history output requests. In the first, request displacement history for the set Tip-a; in the second, request reaction force history for the set Attach.
Add mass proportional damping to the bracing section properties. To do this, double-click BracingSection underneath the Sections container in the Model Tree; in the section editor that appears, click the Advanced tab.
In the Damping region, enter a value of 15 for alpha and 0 for the remaining damping quantities.
These values produce a reasonable trade-off in the values of critical damping at low and high frequencies of the structure. For the three lowest natural frequencies, the effective value of 
is greater than 0.05, but as was shown in Figure 7–11, the first two modes do not contribute significantly to the response. For the remaining modes, the value of is less than 0.05. The variation of as a function of natural frequency is shown in Figure 7–13.
Repeat the above step for the main member section properties.
Redefine the tip load at set Tip-b. Specify CF2 = –10000, and use the amplitude definition Bounce.
Change the element library to Explicit, and assign element type B31 to all regions of the model.
Create a new job named expDynCrane, and submit it for analysis.
When the job completes, enter the Visualization module to examine the results. In particular, compare the tip displacement history obtained earlier from ABAQUS/Standard with that obtained from ABAQUS/Explicit. As shown in Figure 7–14, there are small differences in the response. These differences are due to the different element and damping types used for the modal dynamic analysis. In fact, if the ABAQUS/Standard analysis is modified to use B31 elements and mass proportional damping, the results produced by the two analysis products are nearly indistinguishable (see Figure 7–14), which confirms the accuracy of the modal dynamic procedure.
