The following blog is the process on how to add snap hooks into your plastic injection molded part. The snap hooks feature can really save you a lot of time by creating the initial geometry of the snap hooks and the fitted groves that they go into. The snap hooks feature will also save a ton of time if there are any revisions needed down the road. By using this command in SOLIDWORKS will make design changes quick and easy.
In order to use the snap hooks feature, it is a good idea to first set up your 3D sketch. The reason you will create a 3D sketch is to help with the positioning of your snap hooks inside the snap hooks command. The use of 3D sketch points will allow you to easily position where you want the snap hooks to lie. We want to insure that these 3D sketch points will be along the same plane in 3D space, so in order to position the sketch points along the same plane I inserted a plane around the maximum point of curvature of the remote (refer to the first image). Once my plane was positioned I went inside the 3D sketch, where I added two sketch points with two relations each. The first relations that I added were coincidence to the edge of the remote for both sketch points. Secondly, to insure that the sketch points were on the same plane I used the on plane relation to make sure the two points would line up properly.
At this time, I have the points of placement created for my snap hooks, so I entered into the snap hooks feature. I had to do a separate snap hooks feature for each of the two 3D sketch points, being that I wanted two snap hooks in my model with different locations. The process, once in the command, is select one of the 3D sketch points as the point of placement for the snap hook. Next, I used the top plane to define the vertical direction of the snap hooks. I needed to also define the direction of the hook so I used the right plane to insure that it was facing outwards from my solid body. Through this process, use the preview in your graphics window and the reverse directions check boxes in the command to get the proper orientation. Lastly, inside the snap hooks command it asks for the dimensions to define the geometry of the snap hooks, continue to fill these in as necessary for your individual design intent.
Once done creating my two snap hooks I can now proceed to create the snap hook groves. It is necessary to create the snap hooks before the grooves because SOLIDWORKS requires the snap hooks to already have been created in order to make a complementing grove for it to fit into. The snap hook groove feature is very easy to use; the first thing it asks you to select the snap hook that you would like to create the matching groove for. Next, you simply select the body that you would like to add the groove to. From here you can edit the geometry of the snap hook grooves if you have specific geometry to match your design intent, otherwise SOLIDWORKS will automatically match the dimensions to fit the snap hook you selected. So, just like that you have a matching snap hook and groove to hold your two plastic injection molded parts together. Also, at any time you can get right back into the feature and change the geometry or placement of the hooks.
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A video using this technique can be found here.