Solid Thinking: Things You Might Not Know About Assemblies15 Mar, 2005 By: Greg Jankowski Cadalyst
Little-known facts can add up to big improvements in productivity and design accuracy
One of the key advantages of designing with SolidWorks is the ability to create a virtual prototype. When an assembly is created, it can be made so it looks and acts like the real assembly before parts are ever made. The advantage to using the virtual prototype is that the components can be checked to see if they fit together and will move freely. This is much better than spending the time and money on early physical prototypes only to find out a part does not fit.
The assembly components are attached to one another using mates. These mates should be functional. If the assembly can move or rotate, there are ways to simulate this motion. For more advanced motion studies and analysis, there are additional software packages (COSMOSMotion) that can be used to create dynamic, detailed studies of the forces, acceleration, and interferences throughout the range of assembly motion.
An under-used feature in SolidWorks is interference detection. Figure 1 shows an example assembly where the shatter is too large for the gears and bearing. One consideration is that all interferences may not actually be bad. For example, a press fit is a designed interference.
Figure 1. Example assembly shows interference 1.
To accommodate these special cases and make interference checking more useful, a number of enhancements have been made to this feature:
- The top level assembly or individual assembly or individual assembly components and subassemblies can be selected. On a very large assembly, it may be easier to check just the area changed or under review.
- Interferences can be marked so they will be ignored. To do this select the inference shown in the Results area, right-click and select Ignore. To show the ignored interferences, select Show Ignored Interferences within the PropertyManager. Figure 2 shows the results from the figure 1 assembly. Interference 1 is not ignored and is shown in blue. Interference 2 is ignored (and shown) and is displayed in white.
- There is also an option to treat a coincident -- that is, parts touch one another, but don't interfere -- either as an interference or not. One way to handle this may be to run the interference check first without the coincident option selected to find the items that actually interfere with one another, fix or ignore those interferences, then do one additional check on the coincident interferences to make sure none of those are unexpected.
- The Component View option will change the name from Interference 1, Interference 2, to the actual component name.
- The visibility of the interference is also controllable. The interfering part can be made transparent (default) and the actual interference volume is shown in red. This helps to quickly visualize the actual interference. The interferences are shown one at a time, or you can hold down the Shift key and select multiple interferences.
- The subassemblies can be treated as individual parts or you can treat the assembly as one part.
Figure 2. Interference PropertyManager shows the analysis from the assembly in figure 1.
Interference checking is an important feature to use on the assembly before parts are actually made. One additional point to keep in mind is that if a lid on the assembly can swing open from 0 to 60 degrees, the assembly should be made so the lid can be checked at 0 and 60 degrees using a angular mate. Mistakes made in the virtual prototype are checked and much easier to fix than after prototype or productions parts are made. Even simple design changes should be checked to see if they interfere with another assembly component.
Create Drawing from Assembly
Another useful feature is the ability to create a drawing directly from the assembly. Once the assembly is created, just select the Make Drawing from Part/Assembly icon as shown (figure 3).
Figure 3. Make Drawing from Part/Assembly icon.
A predefined template can be defined to automatically produce views based on the predefined views in the template. Figure 3 shows the assembly from figure 1 after selecting the Create Drawing function. By using the Make Drawing from Part/Assembly feature in conjunction with a template creating predefined views, you can make the drawing shown (figure 4) with just a few mouse clicks.
Figure 4. Drawing created from a predefined template.
When trying to determine how an assembly is structured, a quick tool that can be used is Assembly Statistics. Just like part or drawing statistics, the assembly statistics can help to gain a quick understanding as to the complexity and structure of the design. The Drawing, Parts and Assembly Statistics features display different information based on the current document type. Certain information is only pertinent to a specific type of document. For example, the number of top-level mates is important to an assembly, but is not relevant to a part, and has limited applicability to a drawing.
Figure 5. Assembly statistics from the assembly shown in figure 1.
For an assembly, the key values will be the number of assembly components -- the size of the assembly -- and how many top-level mates exist within an assembly -- how long it will take to solve the assembly mates. For flat assembly, all assembly components and their mates are solved when the assembly is opened.
One technique that is useful for performance, collaborations and reusability of an assembly is to use subassemblies:
- Create the assembly using a structure that is the same as the final design. This allows for the subassemblies to be opened separately and also turned off, using configurations, when working on the main assembly. This structure also follows the concept of the virtual prototype. Design the part as if it will be manufactured. It will also make creating assembly documentation easier.
- One advantage of a subassembly is that is can be replaced with three mates. To replace all the individual assembly components would require much more work as each component could have three mates each and be related to other sub-assemblies.
- This method also limits the number of top-level mates within the assembly. When SolidWorks opens an assembly, all the mates defined at the top level are evaluated and solved at the same time. The mates contained inside the subassemblies are not solved by default. To solve subassembly mates, flexible assemblies can be used.
These tips can help make your assemblies better and easier to create. Some of these tips may seem small, but little things add up to help improve productivity and accuracy.
About the Author: Greg Jankowski
In her easy-to-follow, friendly style, long-time Cadalyst contributing editor Lynn Allen guides you through a new feature or time-saving trick in every episode of her popular AutoCAD Video Tips. Subscribe to the free Cadalyst Video Picks newsletter, and we'll notify you every time a new video tip is published. All exclusively from Cadalyst!