SolidWorks 2011 Parts Bible - Matt Lombard [172]
• Create a simplified configuration when building very complex parts or working with large assemblies.
• Model with symmetry in mind. Use feature patterns and mirroring when possible.
• Use link values or global variables to control commonly used dimensions.
• Do not be afraid of configurations. Control them with design tables where there are more than a few configs, and document any custom programming or automated features in the spreadsheet for other users.
• Use display states when possible instead of configurations.
• Use multi-body modeling for various techniques within parts; it is not intended as a means to create assemblies within a single part file.
• Cosmetic features — fillets, in particular — should be saved for the bottom of the design tree. It is also a good idea to put them all together into a folder.
• Use the Tools⇒Options⇒Performance⇒Verification on Rebuild setting in combination with the Ctrl+Q command to check models periodically and before calling them “done.” The more complex the model, or the more questionable some of the geometry or techniques might be, the more important it is to check the part.
• Always fix errors in your part as soon as you can. Errors cause rebuild time to increase, and if you wait until more errors exist, troubleshooting may become more difficult.
• Troubleshoot feature and sketch errors from the top of the tree down.
• Do not add unnecessary detail. For example, it is not important to actually model a knurled surface on a round steel part. This additional detail is difficult to model in SolidWorks, it slows down the rebuild speed of your part, and there is no advantage to actually having it modeled (unless you are using the model for rapid prototype or to machine a mold for a plastic part where knurling cannot be added as a secondary process). This is better accomplished by a drawing with a note. The same concept applies to thread, extruded text, very large patterns, and other features that introduce complex details.
• Do not rely heavily on niche features. For example, if you find yourself creating helices by using Flex/Twist or Wrap instead of Sweep, then you may want to rethink your approach. In fact, if you find yourself creating a lot of unnecessary helices, then you may want to rethink this approach as well, unless there is a good reason for doing so.
• File size is not necessarily a measure of inefficiency.
• Be cautious about accepting advice or information from Internet forums. You can get both great and terrible advice from people you don't know, along with everything in-between. Sometimes even groups of people can be dead wrong. Get someone you trust to verify ideas, and as always, test them on copied data to determine if they're effective.
If you are the CAD Administrator for a group of users, you may want to incorporate some best practice tips into standard operating procedures for them. The more users that you manage, the more you need to standardize your system.
Cross-Reference
Best practice development is covered at length in the SolidWorks Administration Bible (Wiley, 2009).
Using the Skeleton Approach
The term Skeleton in Pro/ENGINEER has a different significance than the way it is being used here. SolidWorks does not have any feature or function named “skeleton.” The term just refers to a technique and a set of sketches, planes, axes, and reference points used to lay out the major faces and features of a part.
The SolidWorks Help files, tutorials, and training curricula have encouraged users in some respects to take a “fast and loose” approach to modeling, which is great for initial modeling speed but not so good for design for change. The main consideration seems to be the simplest way to do something, or how it could be done rather than how it should be done. This mentality fit well with the initial several releases of the SolidWorks software, which at that time was marketed as being simple and fast.
The software has progressed immensely since those days.