The Loft command is, in my opinion, one of the most powerful functions available in a solid modelers. Many people dismiss this command early on since it's not only one of the more difficult commands to use, but it's also difficult to visualize. People don't like to model things they can't visually imagine.
Lofts can also be prone to problems, depending on the type of sketches you make. Oftentimes, the sketches will have to be similar in terms of shape, or you'll end up with undesired edge lines and paradoxical monstrosities. For instance, these two sketches...
...will loft together to make this:
Although the computer can create this part file in virtual space, it's actually a paradox and can't exist in reality. This is because it has a couple two-dimensional surfaces that have "infinitely small" (two-dimensional) depth. Additionally, on both the right and left side of the part, you can see some edges that lead to a straight perpendicular edge on the other sketch. This might be okay if you're just making an example part that isn't meant to be realistic, but otherwise you'll want to avoid this.
Basically what this means is you have to exercise caution for the sketches you plan to loft together. If the basic shape contains more ending points (convergences between lines, of any type) then you're likely you end up with more edge lines than you want to imagine, which will be unavoidable unless you change the design. The loft command is powerful but at times it may yield the wrong type of image than the one you want, due to how it works.
Compound Lofting:
The loft command can be used to connect two single sketches together, however it has other purposes too. It can also be used to link a series of sketches together, yielding a smooth, contoured shape that connects multiple points on each sketch. In high school, the term I used to describe this was compound loft. Solidworks has a special name for it (chain loft) which I only learnt later on in my own travels, but I think my name sounds like it's worth more money :)
Essentially, what you want to do when creating a chain like this, is to visually cut the model up into different slides and modeling a sketch at each cut. When the cuts are joined together, they form the finished model you had to begin with. This is in line with sectional drawing. The difference is, though, that using the parametric modeler to connect the loft planes all together essentially creates a multitude of infinitely small cutting places in between the sketches you make. The sketches get connected to one-another using splines, and surfaces arer created around them. If you take the individual sketches you make and loft them one-to-the-next, the outcome will be blockey and edgey since the sketches don't get splined together.
This feature can and is used to create any assortment of contoured 3d surfaces in realtime that, if planned correctly, can indeed be realistic to the model you've made in CAD. A large percentage of the freeform shapes parts use is created using a compound loft series, be it for marker milling, plastics molding, or whatever. I will describe some of this process quickly in both SW and Inventor below.
Solidworks:
To begin with, you need to have a series of sketches planned out that you will loft together. For a quick example I used these simple sketches below:
It may be difficult to see but the sketches are different in small ways, including the length of lines and the centerpoint of circles.
Select the Loft boss/base command and you will be prompted with the loft command's options. There is a tab below named "loft tools:" and three options presented within. Enable the chain loft option to ensure you can select more than two sketches for the loft.
Select your three sketches in order and a preview 3d shape will appear. Depending on the shape of the sketches, the preview shape might not be correct. This usually happens if the program can't figure out which points to connect to form the lofted surfaces. For my example sketches I want there to be a smooth transition between all the sketch points, which are all more or less in line with one-another. In the picture below, the incorrect points are selected (which would create some funky paradoxal 3d surface).
Those loft points are incorrect so I use the mouse to drag-and-drop them to where they need to be. The preview shape now looks like this:
That looks good to me, so I complete the command and am presented with the finished loft part.
This particular example part file obviously isn't anything useful in reality, but it gives you an idea of the process.
Inventor:
Like the SW section, you need to begin with several sketches that will be connected and form the loft. Again, the sketches don't appear to be too different in shape, but take the time to notice the small differences between them.
Click the Loft command in the sketch menu, and you're presented with the Loft window. Select all the sketches in order...
Again, the program will attempt to pick out the points to connect for the lofted shape. The above picture shows everything correct except for one of the bottom edges, which crosses with another of the edges. To adjust this, move to the "transition" tab, disable the "automatic mapping" option, then use the mouse to move the incorrect edge to the correct point. You can also select it from the list and delete it, then manually put in a new one based on the desired sketch points you want.
Once a working loft can be extrapolated by the program, a preview shape will appear...
That's exactly what I want to appear, so I finish the command and am presented with the finished loft:
Examples:
Both the quick examples above aren't useful to anybody in reality, so I'd like to go ahead and add length to this page by showing some of the advanced compound lofts I've performed in the past. Some of these parts involved adding to the model whereas some are subtracting (subtracting is used, as always, if you're trying to replicate how parts are actually "milled"...material is removed from the model, never added).
A simple loft command can be used to show the porting on an Ion bolt, for instance. It's used here in this model of a Warrior bolt I made.
Lofted together yields the type of shape that was removed from the bolt for air to pass through. There's also an extrusion (seen in both the above sketches). This profile, multiplied 6 times around the long axis of the bolt, yields the finished model:
To demonstrate an extreme case of sleek 3d milling, I'll now demonstrate what I did to recreate the external surface of a Shocker NXT body. This part file is copyrighted but I removed the dimensions from the sketches prior to making screenshots, so this will work.
To start, the body is supposed to be milled in such a way that the side surface is a rotating cut all alongside the length of the body. This could be recreated using a coil, but the axis would essentially have to be an arc (or dare I say...spline) which Inventor obviously doesn't like to do. At this stage in the production of the body, the bottom is milled however the top is not. To complete this form, I made several key sketches across the length of the body, to be lofted together and remove material from the slug hexagonal shape. Additionally, I decided to pull a double whammy and finish the top "rounded" part of the body as well as the side coiling surface, both using the same loft command.
The Loft command window looks like this. I manually assigned the sketch points to avoid confusion on the computer's part.
When complete, the model looks like so. Pay special attention to the way the coiled surface follows the oblique line around the side of the body.
Finished body looks like this:
This also shows how you can sometimes cheat the program and use the same lofting command for two unrelated surfaces. The upper "rounded" section of the body is essentially a straight extrusion, but it can be lofted together by creating multiple identical arcs (as I did above). Like I said, double whammy!
Another example, using the "add to" compound loft. This profile is used on the Invert Mini foregrip housing. The foregrip has a curved front as well as curved sides (the curve changes as you go higher on the foregrip) and the top is rounded off at the front. This is a compound loft dream in the making (and it was, for me anyway).
The loft feature.
Some of the curves initially didn't like to join up properly, so I had to tweak it a bit. This involved adjusting the height of the key sketches, which also involved adjusting their dimensions and general shape ever so slightly. This foregrip would be more accurate to model if I had chosen, say, a dozen different planes to sketch. However, had I done that, it would have taken a LOT more time to get the smooth contours between the planes correct.
Anyways, here is the finished lofted surface, plus I mirrored it around the XY to show the actual foregrip shape (not half of it, as above).
Top view of the front contours: (I changed the colors to highlight the hidden lines). The second pic is a perspective view.
Okay, last example....the Invert Mini body. This helps to demonstrates using the loft command on different planes. I started out with an extruded square of material, from which I removed material to achieve the desired shape. Most of the body was put together by using compound lofted surfaces, but I'll highlight two of them in particular.
The first is the back of the body. It's round, dips down in the middle, then ends at a staggering oblique plane behind the feedneck.
Loft window...
Finished:
The front of the body was similar, a series of circles/arcs, except I had to use more of them and they had to be staged on different planes. One of the sketches was the finished cut from the above loft (behind the feedneck).
Loft window below. Inventor correctly extrapolated all the necessary work edges for me, so no manual work was needed.
Here's the finished loft command, with most of the other external milling also finished.
Here's a wide of the finished body.
Obviously that isn't perfectly exact to the real thing, but for demonstrational purposes of my own...shrug it's damned close enough for me! When parts are actually machined like this, the programmer will often elect to manually adjust the countours of the tooling bits to maintain a slightly different shape (for instance, a perfect circle around the feedneck, which didn't happen correctly in my model). This removes a bit from the "theoretical" lofted features but makes it look prettier in reality, which we all like.