Snap hooks, also referred to as snapfits, are a type of integrated plastic fastener common to injection molded parts. And similar to the lip/groove feature discussed last month, they provide a good way of mating plastic components together without the need for additional hardware fasteners such as screws and bolts.
The snap hook system consists of two parts. The first part (the male part) is generally a cantilever beam with a hook on the end, and the second part (female) is the receptacle, or groove, into which the cantilever and hook will fit. The cantilever undergoes some displacement as it traverses the receptacle, and once it is mated, the cantilever relaxes to provide a tight fastening. If you want to know more about the mechanics, mathematics and guidelines for designing such a system, there is an excellent guide from Bayer MaterialScience that can be found here.
Figure 1. A snap fit profile and cross-section. (Image courtesy of Bayer MaterialScience.)
Let’s assume that you understand the mechanics of how snap-fit fasteners work (maximum permissible deflection, mating force, stress and strain, etc.) and that you wish to design a system in SOLIDWORKS.
As with last month’s tutorial on the lip/groove feature, we will start off with two halves of a box. I have created one box, and to save time, I will just mirror that body above the top plane so that we now have a hollow enclosure. When our snap-fit fasteners and groove are complete, we will have designed a snap-fit system for mating these components together.
Figure 2. The bottom half of the enclosure.
Figure 3.The full enclosure.
For now, we can hide the top half of the enclosure as it will just get in the way. In the design tree, right-click the body that represents the top half of the box, and click the Hide icon. It will then disappear from the viewing area.
The first step is to define some sort of reference point where we will locate the snap hook once we have evoked the snap hook feature. To do this, I select the right plane (or front plane—it’s a square box, so it doesn’t matter. We just want to define the midpoint of the inner edge).
Once the plane is selected, I click the 3D Sketch option from the ribbon at the top of the screen, and I sketch a point on the midpoint of the inner top edge. I constrain the point so that it lies on the point, and at the midpoint of the edge.
Figure 4. Defining reference points with a 3D sketch.
Now that the reference point is defined, we can go ahead and begin with the snap hook creation feature.
Snap Hook Feature
The next step is to invoke the fastening feature wizard.
We can do this by going to the top menus, selecting INSERT > FASTENING FEATURE > SNAP HOOK.
This will open a section in the left-hand pane that is divided into two parts. At the top portion, we can see a section titled Snap Hook Selections (see Figure 5), and it is in this section where we will locate our hook on the model body. Beneath that section is a 2D representation of the hook geometry titled Snap Hook Data. First, we will position the hook on the model using the Snap Hook Selections options.
The first box allows us to select a position for the location of the hook body (the cantilever part). Click the box, then go into the main graphic area and select which face you will be using and where exactly on that face you want the hook body to appear. I select the reference point that we created in the previous step. This is lying on the top most face. The middle of the hook’s width is snapped onto the reference point, so the hook will lie right in the middle of the box width.
The next box in the selections pane allows us to define the vertical direction of the hook. I have selected the top plane, so the vertical direction will point upward. Please feel free to mess around with these settings to get a feel for them.
The third box allows us to define the direction of the hook itself (the horizontal direction, if you will). I want my hook to face away (outward) from the center of the box so as to create a flush exterior finish, so I select the exterior face that is adjacent to the hook (face <1>).
You can see a summary of these actions in Figure 5, and I have labeled the face and points for easy reference.
Figure 5. Snap Hook Selections.
Snap Hook Data
Now that the hook is located on the box, we can begin to change the hook dimensions according to our design requirements.
If you go back to the Snap Hook section in the left hand pane and scroll down below Snap Hook Selections, you will see a 2D illustration of the hook profile and a view of the hook from the front (the wide part).
Here we can input dimensions for the depth at the top of the hook, the length of the main hook body (I have made it 20mm), the width at the root (3.43mm) and so on.
Those of you who are familiar with hook design may notice a glaring omission in the input boxes. There is no option here to select the angle of inclination. This is very important in snap hook design as it affects the mating friction and also the mating force. If you want to figure out your angle of incidence, you will have to use some trigonometry here. Just imagine the hook as a right triangle and you can vary the sides accordingly to give you the required angle.
Now that the hook is positioned and the dimensions are as required, we can move onto the next step. Click the green tick icon and close the snap hook pane.
Snap Hook Groove
Now that the hook is complete, we can begin to construct the groove into which the hook will reside when the two halves of the box are mated together. First, we need to unhide the top half of the box that was hidden earlier in this process. Right-click on the top half of the box in the design tree and click the show icon. The top half of the box will appear in the main graphics window.
Invoke the Snap Hook Groove feature by going to the top menu and selecting INSERT > FASTENING FEATURE > SNAP HOOK GROOVE. This will open the Snap Hook Groove selection pane on the left-hand side of the screen. This section is a lot easier than the Snap Hook portion, because we are just going to select the existing hook and the software will basically do the rest.
Click the first box in the Feature and Body Selections section. This will allow us to select the hook. We can do this from the design tree, where it is labeled in this instance as Snap Hook 1.
The next input box below that allows us to select the body into which we will make the actual groove. Naturally, we select the top half of the box.
And that is pretty much it. If you rotate your model, you can see there is now a groove on the inside face. For all intents and purposes, you now have a snap hook and groove system.
You will note, however, that there is another 2D drawing of the hook in the Snap Hook Groove pane, along with a few more input boxes. These boxes allow you to design in some offset, which allows the hook greater clearance. By default, mine has a 2mm offset to the gap height. This will allow my hook to engage a little bit sooner than required (and in reality, this will allow a loose fitting of the top half to the bottom half of the box—it will wiggle around a bit). For a good measure, I just add 0.25mm to the width clearance. I’m actually going to 3D print my box and my fasteners, so I want a little bit of extra clearance, just in case.
While you are playing around with these values, you will see the groove change in real time in the graphics window, and you will see a wireframe ghost image of the snap hook itself, so you can get a visual idea of what is going on.
Figure 8. Wireframe of hook plus groove.
When you are happy with the groove design, just press the green tick and the Snap Hook Groove pane will close. Congratulations—you have created a Snap Hook and Groove system.
But wait…a single snap hook by itself is not very useful in this context, right? Correct. When fastening two halves together, you are going to need more than one fastener. Otherwise, it’s not so much a fastener, but more of a hinge. And not a very good hinge at that.
Replicating the hook and groove is very easy. It’s just like copying any other feature.
I click the Features tab in the top ribbon menu, and click Mirror. In the Mirror pane, I select the front plane as my mirror plane and simply select the hook and the groove from the design tree (or the graphics window), and Bob’s your uncle. We now have two hooks, two grooves and a sturdy fastening. We can mirror this feature as many times as we like and along any plane.
Figure 9. Mirroring the hook and groove feature.
So, there you have it. You are now well on your way to creating plastic enclosures. Of course, many enclosures don’t rely exclusively on snap hooks—they also combine the snap hook system with lips and grooves. Luckily, there is a tutorial on that as well, so why not have a look at last month’s tutorial on the lip/ groove feature, combine it with snap hooks and give it a go.