Lip and Groove Design Made Easy

Lips and groves are prominent parts of our everyday lives, and they work on a very simple premise. Take a lunchbox, for example. A lunchbox consists of two parts, the base (where you put your sandwiches) and the lid. The lip is built into the mating edge of the lid, and the groove is built into the edge of the box’s base. When you push them together, not only do they help to align the assembly, but they also help to seal it and keep it closed, stopping your lunch from falling out all over the place.

image001Figure 1.A lip, groove and sandwich in a lunch box. (Image courtesy of Global Baby.)

Of course, it’s not just lunch boxes that feature lip and groove mating. Your smartphone likely has one, too, as does your laptop power supply enclosure. In fact, wherever two plastic shells need to be mated to create a flush enclosure, there is a good chance that there is a lip and groove aligning and mating the two components together.

In this tutorial, we are going to take a look at the lip and groove feature in SOLIDWORKS, which provides an easy method for creating lip and groove parts in your designs. It’s a fairly easy tool to use, and once you have mastered it, you can greatly reduce the time needed to incorporate these features into your designs. 

Make a Box

Okay, so the first step is to make a box or container of some kind. The box will need to have two components—a base and a lid. I won’t go into describing how to make a box in this tutorial. Let’s just say that knowing how to make a model of a hollow container is a prerequisite for using the lip and groove feature!

The important thing to note is that the lip and groove feature only works in part mode. It will not work in assembly mode. So, you can either build your box as two separate bodies in part mode, or else you can build the base first and import the lid as a separate body into the same part document.

In Figure 1, I have opted to design both the lid and base in the same document.

In the figure, you will notice that I have added some internal ribs to the base of the box. This is not an accident, and you will see why I have done this later.

image003Figure 2. Generic box and lid with internal ribs.

Now that you have your container model opened in part mode, you will need to access the lip and groove feature.

The feature can be accessed from the menus at the top of the display:

Insert> Fastening Features> Lip/Groove

This sequence will open the feature selection window up on the left-hand pane.

image005Figure 3. Accessing the lip and groove feature.

Figure 4. The Lip/Groove pane.

From here, you will see a number of options. In the first section, you will see two input selection boxes for Body/Part Selection. This is where you will select which body you want the lip to appear on, and which body you wish to apply the groove to. I have selected the part named “Base” to apply the groove to, but your design may differ. The third selection box in this section allows you to select the groove’s cut direction. Generally speaking, you will want the cut to be in a downward-facing direction, so pick a downward-facing edge as a reference point. In my example, I have selected one of the longest edges of the internal ribs. Note that If all the selected faces on which to create the lip and groove are planar and have the same normal face, the default direction will be normal to the planar faces.

After defining your parts to apply the lip and groove, and after defining the direction, you can scroll down the Lip/Groove pane to the next section, which is called “Groove Selection.”

The first box allows you to select the faces on which you wish to cut your groove. In my example, I have selected the topmost face of the base. Beneath that is the box that will allow you to define the inner or outer edge where you will cut the groove. I have selected the inside edges of the topmost face, which I defined in the previous box.  Below these two boxes,you will see two check boxes.

image010Figure 6. Examples of jump gaps cleared and jump gaps selected.

One check box is for “Tangent Propagation,” which allows you to extend the groove cut to tangent edges (I left this unchecked because my edges are planar),while the next check box allows you to “jump gaps.” I have checked this box. Remember the vertical ribs on the inside of the box? By checking the Jump Gaps box, SOLIDWORKS will cut a groove behind the ribs and create a receptacle for the lip to slot behind them.

image011Figure 6. Defining the groove.

After inputting the definitions for the groove, scroll down a little more on the Lip/Groove pane and you will seethe “Lip Selection” area. The options here are exactly the same as the groove section because—wait for it—a lip is basically a geometrically mirrored groove.

When you click the Lip Selection box, the body with the groove will disappear from the main window and the lid section will become visible. You will repeat the same procedure you used for the body with the groove except for one difference: if your groove is on the inner edge, then you will need to cut your lip into the outer edge of this part. And, conversely, if the groove is on the outer edge, then you will need to apply your lip to the inner edge of this body in order for the full assembly to mate together.

So now your lip and groove geometry is defined, you have specified which edges are to be cut away on each body, and you are free to move on to the next section.

Figure 7. Lip and groove parameters.

Scroll down to the last section in the left-hand Lip/Groove pane and you will be greeted with a cross-sectional drawing of a lip and groove, with input boxes pointing to each part of the lip and groove. This is where you will define the custom dimensions for your lip and groove. Although it should be noted, that as long as there are no conflicts in your geometry, you should have the default values applied already and you can actually click on the “Show Preview” check box to see what your design will look like. If you are happy with the default settings, then you can click the green check mark at the top of the Lip/Groove pane, and you will see the lip and groove applied to your model in the main window.

If you are not happy with the default settings, then you can change the values in the white boxes manually. For example, maybe your lip isn’t tall enough. In that instance, you will want to look at the drawing, locate the input box corresponding to lip height, and change the value. SOLIDWORKS will then create a deeper cut and create a taller lip. Altering these values will alter the tolerances and hence the fit of the mate where it comes to manufacture.

Finally, there are three check boxes at the bottom of the pane: Link matched values, Show preview and Maintain existing wall faces.

The Link matched values option will equate certain parameters to each other, ensuring that when scaled they remain relative to each other.

Checking the Maintain existing wall faces option will maintain the draft version when possible and extend the existing wall face to the top of the lip,if you create a lip on a model wall that has a draft version.

So, there you have it. The lip and groove feature is pretty easy to use and saves a lot of time when you are designing enclosures. I have used it a few times, and it’s especially good for 3D-printed enclosures. Just remember to make the thickness of your lip at least three filaments wide for a more sturdy and rigid lip.

image015Figure 8. Close-up of groove (left) and lip (right).

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