SolidWorks Part Modeling: Basic Best Practices by Brian McElyea
Best practices are simply ways of bringing about better results in easier, more reliable ways. By incorporating some best practices into your SolidWorks modeling routine, you can streamline your design work and focus on your design instead of driving SolidWorks. Below you will find some of the best practices that I use when creating part models in SolidWorks.
Start with a good template
Creating templates is one of the first things you should do before starting production work (or when starting a new project, if required). The part template provides the foundation that all your models will be built upon. This is especially important if working with other SolidWorks users on the same project; it will ensure consistency across the project.
The template can determine which units and drafting standards are used, and also contains any project-specific custom properties that are desired. I like to keep all metadata associated with part and assembly files (such as standard tolerances and most of the other data that gets read into drawing title blocks) in the respective files themselves. This way, all information related to that particular file is embedded in the custom properties, and the file can stand on its own if, for example, you are dimensioning the part in the file itself.
.png)
.png)
.png)
Model parts about the origin
By always starting your part models at the part’s origin, you're starting at a known reference that is readily accessible in other environments (i.e., other parts, assemblies, and drawings). This also creates consistency, which is a good thing--especially if you are working with other SolidWorks users.
Sure, you can create your models anywhere you like and fix a point in space, but if the initial sketch is not related to the part’s origin, you should be aware of potential issues that may reveal themselves as the design evolves. For instance, if you have features that you want to be symmetrical, you may have to create additional reference geometry in order to mirror.
The only time I overlook this is when doing top-down modeling (working in-context in an assembly). When creating a new part in-context, the part origin is located at the assembly origin. In my experience, that is generally a good thing when creating parts in this manner.
Use symmetry whenever possible
Using symmetry wherever possible is a way to simplify your sketches, allowing changes to be more easily made. This can actually be accomplished in two ways: at the sketch level (using either the Mirror Entities or Dynamic Mirror Entities commands) and at the feature level (using the Mirror command). To enable symmetric sketch geometry creation on the fly, use the Dynamic Mirror command.
.png)
Name dimensions for reference
If you are going to be using Equations or building Design Tables, make things a little easier on yourself (and your co-workers) by naming your dimensions as you create them. This is an especially handy tip when modeling configurations of a commercial part from a specification where the dimensions in a table correspond to alphabetical dimensions on a schematic.
Use equations
If you have a dimension that should always be some fraction or multiple of another, then model it that way! Equations in SolidWorks have gotten much better in the last several releases.
You can also create conditional situations using more complex equations and VBA. For instance, if you wanted to create a dimension whose value depends on a range of values for another dimension, you can use the Visual Basic Immediate If (IIf) function. The IIf function takes the form of IIf(eval,then,else). To put it in SolidWorks format:
“D2@ Sketch1″ = (IIf (“D1@Sketch1″>6 AND “D1@Sketch1″<12, 8, 4))
In this circumstance, “D2@Sketch1″ would evaluate to 8 for values of “D1@Sketch1″ between 6 & 12, and 4 for all other values.
Create mate references
If you are creating a part that will be used in multiple assemblies, such as a library or commercial-off-the-shelf (COTS) part, consider adding a Mate Reference or two. This will allow you to drag in these parts and quickly apply mates. And if you name the references, your part can be automatically mated when placed in the assembly.
Apply cosmetic fillets and chamfers last
By not adding any critical features (such as cosmetic fillets and chamfers) until the end of the feature tree, you decrease the amount of rebuild time for the part.
Adding cosmetic features last will also make it easier to create simplified configurations of your models for analysis or to speed up assembly performance, as they will be easy to find at the end of the FeatureManager tree and there will be no dependencies to other geometry that may cause issues when they are suppressed.
Use fillet features instead of sketch fillets
There are some instances where a sketch fillet makes sense. But in my experience, I have found that in most cases, a fillet feature will result in a more robust model and also makes troubleshooting easier. Using fillet features also allows you to group fillets based on the fillet radius when appropriate, and can allow the model to be simplified easier.
Use library features
If you find yourself (or your co-workers) constantly reusing the same feature(s), such as connector holes or sheet metal louvers, consider creating a Library Feature. This will allow you to drag and drop the feature onto your model. You can set up the Library Feature to take user input, and you can have configurations, such as shell sizes for connectors.
Conclusion
These tips highlight just a few of the best practices you can incorporate into your workflow to help you model parts more efficiently and help to communicate your design intent. By incorporating some (or all) of these suggestions, my hope is that you will become a better and more efficient SolidWorks user.
***
Brian McElyea is a senior mechanical engineer at Intuitive Research and Technology Corporation. He is a Certified SolidWorks Professional (CSWP), president of the Redstone Arsenal chapter of the North Alabama SolidWorks User Group (NASWUG-RSA), and writes about SolidWorks at CADFanatic.com.
