Neat Tricks in Pro/ENGINEER Wildfire 3.0
by Romeo Ridel

Design Animation in Pro/ENGINEER Wildfire 3.0

This technical tip will help you create some useful visual effects using the Pro/ENGINEER Design Animation module.

Since all the components involved in a mechanism or any packaged assembly are non-deformable throughout the entire range of motion, it may be necessary at some point to model pulleys, belts, chains, cables (or, any combinations) and see them animating in a proper way.

The idea behind this method is to make use of the Pro/MECHANISM joints connecting different segments of the component about to be animated. In other cases, simply defining a connection between two or three design animation bodies will do the trick.

For instance, if you need to model a rope (or cable) mechanism in which pulleys are involved the followings methods can be used:

• Split the cable part (which is currently a single long component) into individual segments and connect them to each other using “Slider” Pro/MECHANISM joints. This will create a telescopic-like component (Figure 1). This operation automatically creates independent design animation bodies, which allows us to move them either using servomotors or > Dyn Drag functionality.
  
  
• Once the Pro/MECHANISM joints are completed, define a “Gear” connection to simulate the pulleys. This type of connection is velocity ratio-based and will help ensure the animation is created properly. (Figure 2)
  
  
• The last step is to either define the servomotors or organize the > Dyn Drag snapshots in the animation timeline. The final animation is presented in Figure 3.

We will use another example for the animation of belts (or chains). This method can also be used for different components that move following a precise trajectory. The animation preparation follows an identical step-by-step approach as above:

• Split the belt part in as many segments as desired. The smaller the segments the smoother the motion.
  
  
• Place the very first component using a “Default” joint. This is the slot curve or, the trajectory that all other components have to follow.
  
  
• Place the second component (first segment of the belt) using a “Planar” joint. This will restrain the motion about the plane normal to the direction of motion. Also, for the same component, follow the trajectory using a “Slot” joint (in Pro/ENGINEER Wildfire 3.0, this is available in “Assembly” mode). (Figure 4)
  
  
• The follower point is placed right in the center of the belt segment.
  
  
• Connect all the other segments using “Pin” (to allow the rotation) and “Slot” (to follow the trajectory) joints (Figure 5)
  
  
• Either use servomotors or > Dyn Drag snapshots to animate the mechanism. The outcome can be seen in Figure 6.

Using Pro/ENGINEER Mechanica and Pro/ENGINEER Expert Framework (EFX) Integration

This technical tip is based on a functionality implemented in Pro/ENGINEER Wildfire 2.0. It is the integration between Pro/ENGINEER Mechanica and Pro/ENGINEER Expert Framework Extension, which can be very handy for analyzing structures built out from standard section profiles.

The integration is based on the shared cross-sectional libraries (or the “Profiles”, see Figure 7) of Pro/ENGINEER Mechanica and Pro/ENGINEER Expert Framework. Therefore, there can be a seamless transfer of information from one to the other.

Profiles become idealizations once transferred to Pro/ENGINEER Mechanica. In other words, the cross-sectional properties are assigned to 1-D finite elements (i.e., the BEAM elements). These BEAM finite elements require less computation time and disk storage space. Thus, a quick FEA solution in a very short amount of time without complicating designers with any mesh controls, aspect ratios, etc.

These next steps will walk you through the process of sharing Pro/ENGINEER Expert Framework profile libraries with Pro/ENGINEER Mechanica and also the procedure on transferring the model to Pro/ENGINEER Mechanica for analysis:

• Identify Pro/ENGINEER Expert Framework’s load point and adjust the available libraries’ naming convention as seen in Figure 8.
  
  
• After you complete this operation, all framework assemblies designed with Pro/ENGINEER Expert Framework contain information for structural analysis in Pro/ENGINEER Mechanica.
  
  
• After you complete a certain design using Pro/ENGINEER Expert Framework, create a Pro/ENGINEER simplified representation. For example, TEST_EFX. Use “Substitute” and “By Rep” as a rule as seen in Figure 9. The “By Rep” is Pro/ENGINNER Mechanica.
  
  
• Click > Apply from the simp rep dialog box. The simplified representation removes the solid geometry of the profiles and keeps a datum curve that has the assigned cross section information of the beam for Pro/ENGINEER Mechanica.
  
  
• Access > Applications > Mechanica > Structure and notice that the datum curves are now 1-D finite elements with the ENGINEER Expert Framework cross-section profile already assigned to them (Figure 10). Now we can define the loads and constraints, and run the Pro/ENGINEER Mechanica analysis.