SolidWorks 2011 Assemblies Bible - Matt Lombard [9]
The bottom line for the method of mating to base parts is that it is unreliable through changes. Of the methods that are presented in this book, this is the most common yet least reliable method. This is not the fault of the software, but of the method. The reason this faulty method is the most popular is because it is the easiest, and requires the least planning.
When SolidWorks first appeared on the market in the mid-1990s, it became very popular not only because it was inexpensive but also because it was much easier to use compared to products such as Pro/ENGINEER. Pro/ENGINEER taught methods for putting parts and assemblies together that were tedious but worked better through changes.
As an example of where you might use this kind of assembly, think of a robotic arm. Figure 1.1 shows an assembly that was created with bottom-up techniques and was assembled with face-to-face mates.
FIGURE 1.1
Mechanical parts using mates to locate and enable motion
But if you were to create, say, a scale model of a car, as shown in Figure 1.2, the method of independently designing each component, especially something like body panels, and then mating them together wouldn't make much sense. Other methods in the other types of assemblies shown later in this chapter will help with this type of design.
FIGURE 1.2
Considering how you would design the parts of a scale model car
It would be difficult or impossible to design the body panels of the car such that they fit together well and looked smooth next to one another using the bottom-up with mates method.
Driving an assembly with sketches and planes
One way to avoid the potential pitfalls of mating to a base part is to replace the changeable faces and edges with items that are more stable. The stability hierarchy listing items from the most to the least stable looks like this:
• Assembly or part origin
• Assembly or part standard planes
• Reference geometry (plane, axis, point)
• Reference geometry from inserted parts (from using the Insert⇒Part command)
• Sketch lines and midpoints
• Sketch endpoints
• Surface model faces
• Solid model faces
• Edges and vertex points
• In-context items
• Reference geometry
• Faces
• Edges
An easier way to remember this without memorizing the list is that the more parents something has, the less reliable it is as a reference. This becomes more applicable if external references are involved, such as inserted parts or an in-context situation. Edges created by fillets or chamfers are lower on the list of stable references than other edges.
There is no clear answer to the question, “Is this reference stable enough?” It is entirely possible for you to be completely successful using in-context edges for all your model references. In order for that to happen, you would have to plan your model very well and avoid any big topological changes (changes to the number or function of faces) to the model.
Cross-Reference
Chapter 10 covers in-context modeling in more depth, and Chapter 19 covers inserted parts.
When you are building a part, selecting references from near the top of the previous list can be challenging, especially when faces and edges are so easy to use. You need to evaluate how much editing and rework you think you will generate when changes that you haven't necessarily planned on have to be made. Much of this ties into the design intent discussion from the SolidWorks 2011 Parts Bible.
Now consider the two examples mentioned in the last assembly modeling method — the robot arm and the model car. You could design the robot easily