Sweep Like a Boss

The sweep tool has been changed over the years to contain many different options. Let’s take this time to go over all the features of the sweep, new and old. We will talk about the minor details that every sweep should contain and how powerful the tool actually is.

A sweep is essentially just a profile and a path, where the profile is “extruded” along the path. Most users believe that the profile and path must be touching but it does not necessarily have to. See the screenshot below.

The profile simply mimics the path whether it is touching or not. Putting the profile directly on the path is where a specific detail comes into play. It is a general rule of thumb to draw the path before the profile for a specific reason, the pierce relation. The pierce relation is a critical component to a successful sweep and is highly recommended even on the simplest geometry. A pierce relation locks a specific point to the path geometry but allows some degrees of freedom needed by a sweep.

It is also recommended to place your profile at the end of the path otherwise it will only go one direction on the path. But bidirectional sweep is now available in SW 2016 so you don’t have to worry about placing your sketch on the end of your path.

To create a pierce relationship using the same model as above, we will CTRL select the center of the circle and the closest line in the path sketch. From there, the properties dialog will come up and only give us the option for a pierce relation. See below.

Now that our profile sketch is fully defined we can create the sweep.

Our sweep looks great but as I create this sweep I notice something else, a circular profile? The circular profile is new to 2016 so that if you know you will be creating a circular sweep like we have here we don’t have to draw the circle on the end! Let’s give it a shot by deleting out our sketch containing the circle and see what the options are for this.

As we see above, when doing this, we have the option to change the diameter of the circle and this is exactly what we are looking for. Also, we have the option to make it a thin feature so that it can be a hollow tube. This certainly can save some time for those that are used to drawing the circle on the end, making the pierce relation and dimensioning it. This new feature does all of it!

Earlier I was talking about how powerful this tool can be, and I have constructed some interesting sketches to create an abstract bottle design. Check it out!

This is where the sweep tool can be extremely powerful. I will show you what happens when using a guide curve and how altering the settings can change the outcome by a significant amount. Here is what the sweep will look like if the guide curve is not used.

Now this isn’t any different than what we just did, but adding in the guide curve changes the model quite a bit.

I selected the spline as the guide curve and it certainly is more abstract now. On a side note, if you noticed the “Open Group” in the property fields, it is because I put the path and guide curve in the same sketch and used the selection manager to select them. If you are unsure about the selection manager take a look at the blog I did awhile back Why haven’t you been using the Selection Manager.

Going back to the geometry it certainly is a very strange shape, but what if we want to change the way it looks a bit? Well, there are options! In expanding the options group box, we see a couple things.

Mainly what we are looking for is the Profile Orientation. There are two options: Follow Path and Keep Normal Constant.

The Follow Path option essentially keeps the profile perpendicular or normal to the path itself. Keep Normal Constant keeps the profile normal to the sketch plane used. Essentially it keeps the profile orientation constant but moves it around on that plane to follow the path. We already have seen what the Follow Path looks like, but let’s see what the Keep Normal Constant looks like.

Clearly these two options in this case make a big difference with how it looks. These are basically the major options to look at, and the two variations of the part using the sketches we created. Depending on what the end result should be, the sweep could have given me exactly what I wanted and is significantly quicker than modeling a bunch of sketches to use a loft.

For our last example, we will be using a different option called Profile Twist. Profile Twist can be controlled by multiple factors, but I am just going to use the amount of revolutions in this scenario. It is significantly easier and quicker than modeling a helix and sweeping it.

As you can see, I modeled 5 circles and a straight line. Using the Profile Twist option of “Specify Twist Value” and 1 revolution, it looks like what you see above.  If you did not use this option, you would have to create a helix, sweep it and then do a circular body pattern around an axis that you need to create as well. This can reduce the amount of time by just doing everything in a single sweep feature.

The Sweep tool has added a lot of new features throughout the years and is getting better and better. Hopefully I showed the flexibility of this tool and how much quicker it is than doing the alternatives in certain cases.

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