Solidworks Plastics Features: Lip/Groove

The Solidworks Lip/Groove feature is one I haven’t used a lot, but it does save me time when I do use it. When I don’t choose to use it, it’s usually because my lip/groove does not go all the way around the part, or it is so simple it’s easier to create it some other way. Let’s take a look at the Lip/Groove feature.

I get a little chuckle out of the SW icon, as it’s kind of incorrect. But if you stopped to admire every mistake, you wouldn’t get much done.

Lip & Groove can work in two different modes. The easiest mode is where you just put a lip or a groove on a part, and then put the opposite feature on the other part. That’s easy enough, but kind of manual.

The more elegant way to handle Lip/Groove makes it less elegant to model the rest of the part, but let’s go through it anyway, and you can decide.

You start by selecting the body for the groove (blue) and then the body for the lip (pink). If you only have one body in your model, you’ll still get the option to pick two.

The third (purple) box is for the direction of the lip/groove. Be careful with this. If you pick an edge that has draft on it, you may not get the direction you want. You’ll be better with a plane, planar face or an axis. The Lip/Groove direction should match the direction of pull for the draft.

The groove selection box will automatically hide one of the bodies for you so you can pick faces or edges from the other body. That’s a nice touch. If you have round corners make sure to select Tangent Propagation. If your edges are not tangent, you will have to manually select all the edges where you want to apply the lip/groove.

If you have gaps in the lip/groove, make sure to click Jump Gaps. That part may give you some issues, but give it a try anyway. If it doesn’t work, you may have to run the command twice to get all the way around the part.

Notice that when you switch to the Lip Selection, it will switch bodies for you automatically again. Very nice.

For the Parameters, all of the appropriate numbers should be in there. If you need something other than what this feature gives you, you might have to add it manually.

The H dimension can be considered a reveal. If you use this dimension, the edges for the groove should be on the inside, and the lip on the outside.

This will leave two features in your FeatureManager – one for the lip, one for the groove. Remember that when you want to edit, because it makes a difference which one you edit. It would have been better if you could edit them both in one place, but it’s a relatively minor criticism for this kind of feature.

Oh, and from personal experience, don’t try to run this command when you’re in Section View. You won’t be able to select all the little bits you want to get.

I think it’s a pretty nice feature if all you need is a fairly basic lip/groove. I don’t usually model in such a way that I have two finished bodies in a single part, but you might make the exception for this. And then there are the cases where you would have more than two parts to put lips/grooves on. In that case, you’d have to run the command again.

Almost regardless, using this feature is better than doing it manually, especially if the parting line for your parts is non-planar.