Using SolidWorks to Create a Helical Pattern

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SolidWorks has many different flavors of pattern features that can aid you in your design process. On top of the extensive capabilities available in the traditional linear, circular and mirror patterns, we can also create patterns utilizing data from curves, sketches and tables. New in 2013, we are even able to vary both spacing and feature dimensions in the linear pattern tool!

One of the very few things not offered as a built-in feature, however, is the helical pattern. Before you go about creating countless sketches, features, and reference planes to achieve the coiling pattern you need, you may want to read this article for some helpful hints in attaining that same pattern by using some of the useful features that are already available in the software.

In order to create the helical pattern we are looking for, we need to have a way to tell SolidWorks to follow a helical path while dropping the necessary instances (or copies) where we need them. The Curve Driven Pattern feature already does a very good job at accomplishing this, while giving us with the options we need to maintain the feature orientation to the cylindrical body. Using the Helix and Spiral feature to provide the ‘curve’ for our curve driven pattern, we are able to achieve the geometry we need without breaking a sweat.

 

  1. The first step is to prepare to create the helix. In order to do this, you will need a sketch that contains only a circle with the diameter you wish the helix to be. I’ve chosen to first model a cylinder as my base and then I placed my new sketch on one of the flat end faces. By using Convert Entities to copy the circular edges of the base feature, we can be confident that the diameter of the helix will update automatically if someone chooses to change the size of the model in the future.Using SolidWorks to Create a Helical Pattern
  2. Next, you’ll want to find the Helix and Spiral command in the Curves drop-down on your CommandManager. You can also access this command by going to Insert > Curve > Helix/Spiral. Here you can chose to define your helix by either pitch and revolution, height and revolution, or pitch and height. Once you’ve entered your parameters, make sure your helix is turning in the correct direction and that it starts at a point which makes sense for you application. In this example, I’ve chosen to define my helix with the pitch and height parameters. I chose a rather large pitch in order to maintain a gradual slope around the cylinder. I’ve lined up the start of my helix with the Front Plane. This is not necessary, but it may help you to visualize your helical pattern while you create it.Using SolidWorks to Create a Helical Pattern
  3. Once your helix is created, it is time to model the geometry necessary to complete the seed of the desired pattern. This can be done before the helix is created, however, I decided to do it after in order utilize the convenience of Convert Entities in the first step. The geometry of your seed does not need to be geometrically related to that of your helix. As you can see, I’ve created a cut into the cylinder and added some holes and fillets.Using SolidWorks to Create a Helical Pattern
  4. The final step is to create your Curve Driven Pattern. This feature can be found in the CommandManager under the Linear Patterns drop-down. It can also be found in Insert > Pattern/Mirror > Curve Driven Pattern. Once in the PropertyManager, the first thing you’ll be asked is to provide SolidWorks with the curve that will guide your pattern. Then you can choose how many instances you require and whether you would like your pattern to be equally spaced or spaced at a specific interval. The most important thing of all is to make sure you choose your alignment method to be Tangent to Curve. Then you must select the curved outer surface of your cylinder as your normal face.Using SolidWorks to Create a Helical Pattern

Whether you chose to create this pattern with features, faces, or solid bodies, it does not matter. If you create your pattern with equal spacing, you may wish to skip the last instance, depending on how you originally modeled the height of your helix in comparison to the length of the cylinder.

Using SolidWorks to Create a Helical Pattern

Et voila! If you follow my steps, you should come up with a successful helical pattern. If you wish to go more in depth, you may choose to explore the use of global variables and equations to derive relationships between the helix geometry and the curve driven pattern parameters in order to truly satisfy your design intent.
 

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Laura Weismantel is an Applications Engineer at CAPINC, a SolidWorks Value Added Reseller with locations across New England. She is a regular contributor to their CAPINC University blog.

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CAPINC was founded on one core principle: Provide the best solutions and services to assist our customers in designing and developing better products. CAPINC provides premier solutions and services in New England to assist our customers in accelerating their design and development process for better mechanical products. Our award winning technical support team is comprised of industry experts with hundreds of years of combined practical experience in mechanical design, design validation and analysis, product data management, and technical communication. We are the award winning 3D solutions partner offering SolidWorks software and training, and the entire Stratasys line of 3D printers and production systems. For more tech tips and blog tutorials check out CAPINC's blog and videos.
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