How does this sound? Two ways to shape the shapes you love to shape using SolidWorks to get those lovely, lovely shapes. Now, before this sinks too much further into a gurgling mire of Suessville shenanigans, lets take a look at some interesting methods to form and fit and fit and form points of lofts and lofts of points… rrrrrrrrrrgh.
Lofting to a Point
A couple weeks ago we took a quick look at lofting a profile to a point using a centerline. INSANE yes? You can take a look at that to get the idea of how it all works, but basically all you need is a profile, a path and a point. Using the point as one of the profiles, allows you to easily get a very fine point. Adding a path (and/or centerline) gives you even more power and allows you to make some very interesting shapes. Well take those concepts and show two methods to amaze your mind.
A Loft to Point through a Surface
This, my friends, is an incredibly fun way to add a little bit of shape to your surface. It’s a little difficult to see it from screen shots, so I’ve included a short video to help ya get the idea of what it is and how it’s created. Here’s the video along with the steps to make it happen.
- Create a profile with endpoints below surface
- Create a path for the profile with an endpoint below the surface
- Loft the profile to the point, using the path as a Guide Curve in the Loft Properties
- Trim excess lofted surface using Surface trim (Insert, Surface, Trim)
- Knit surface (Insert, Surface, Knit)
- Fillet surface with Face Fillet (Insert, Surface, Fillet/Round) setting Options to curvature continuous
Lofting Your Profile Trick
The method here is to start and end your loft below the surface so you’re able to use that surface as a trim tool. Of course, depending on what your profile needs to look like, you may start all or some of it behind another surface.
A Loft to Point on a Surface
This is another fun way to shape a profile. Among other things, it could be used to emboss conical curves on a surface or to shape a part against a surface. It uses the Spline on Surface command. Here’s a video of how it works and the steps to make it happen.
- Create a path on the surface using Spline on Surface command (Tools, Sketch Entities, Spline on Surface)
- Create a plane on the path endpoint (select endpoint and centerline guide, the Insert, Reference Geometry, Plane)
- Create a profile on the plane
- Loft the profile to the point, using the path as a Centerline Parameter in the Loft Properties
Lofting Your Profile Trick
As I said, this uses the Spline on Surface command. This is a great tool to use if you need to ‘wrap’ something around a surface or rather, shape an object to a certain surface. When using solids, you could even cut into the surface.
To keep the loft separate from the surface you used to guide the loft, simply deselect Merge Results in the Loft properties (it’s near the bottom).
These are just a couple ways to get some nice shapes in SolidWorks. I’d be interested to know if anyone uses these methods or has any tips they can throw in. If so, hit the comments!
