Welcome to the latest blog series from SOLIDWORKS. Each month, our new “Stump the Chump” post will delve into common questions and/or challenges that our users encounter on a regular basis and will present various ways to solve them. While we have a large team of seasoned CAD veterans at SOLIDWORKS who can answer user questions, we also have the most passionate and best CAD user community in the world. So in this blog series, we will share advice, tips and suggestions in response to real questions posted by YOU in the SOLIDWORKS User Forums.
We will scour the SOLIDWORKS User Forums for questions and challenges that are relatively common among our users. If after reading this “Stump the Chump” post, you have an alternative answer or simply have additional questions, feel free to add it to the comments section below. So without further ado, here’s the first question:
Question: Sweep along a curve. Can the sketch profile dimension change as a function of the length of the sweep curve?? Like the diameter of a sketch circle, which becomes bigger and bigger as the square root of the length of the path?
User Answer: Depending on how complex your profile and sweep path curve are, you may be able to use a guide curve (or curves) to drive the dimension of the profile. In this quick example the 0.5 radius circle is the profile sketch, and the end diameter is determined by the guide curve, the size of which is driven by an equation linked to the length of the sweep path.
In this example, I replaced the 3-point arc guide curve with a freeform spline.
If you need the profile to change a lot, a loft might be more appropriate. Don’t forget, you can use guide curves to refine the shape of a loft too. If you can post more details, and/or an example of what sort of shape you’re trying to get, someone can probably give you some more detailed advice.
Follow-up question: Thanks so much for your help. I am 90% home…
If I try to have the length of the sweep curve in the sketch as one dimension, then I make your suggested equation to make the circle diameter driven by this length of the sweep curve. But, then I get only a constant diameter through the whole sweep – the last value. How do I get the parameter throughout the sweep, starting as zero and ending as the length of the sweep curve?
User Answer: You will need to use a loft, from a point to a circle. You can’t just reduce a circle profile to zero in diameter in SOLIDWORKS. A mathematician might see a point and a zero diameter circle as the same thing, but SOLIDWORKS doesn’t. A circle has to have a diameter, even a really small one. So if you need a point at one end, you’ll need to make a loft with a centerline.
Below: Sketch1 is the curve that is used for the center line, and to locate the end point. Sketch3 is just a sketch point, placed coincident to the end of the curve in Sketch1. Sketch2 is a circle, centered on the other end of the curve in Sketch1. We set the diameter of the circle equal to the length of the curve so it would be parametric. If you know the length of your curve, and you know it’s not going to change, you could just put the dimension on the circle and not bother with the equation. You don’t say if your curve is a simple arc like we’re using here, or something more complex. With the arc, as we have it set up here, you can’t go much beyond 113° without having the loft turning in on itself and failing. The shape of your curve and the end diameter will determine what you can get away with. Also note that the loft gets bigger uniformly as it follows the centerline. If you want a more complex transition from point to end diameter, you will need to add guide curves, more profiles, play with the start and end constraints, or a combination of some, or all, of the above.
SOLIDWORKS Expert Weigh-In: Another way to approach this problem is to create the sweep using an equation-driven curve. The blue circular profile (shown below) is swept along the green sweep path and the diameter of the profile is controlled by the equation-driven curve.
Watch the video below to see how it’s done.
Thank you to Mogan Fons for the question and to Logan Pegler and Erik Bilello for providing solutions in the SOLIDWORKS User Forum. If you have a question that you would like to pose to the greater SOLIDWORKS user community or to provide tips and tricks to your peers, our User Forums are a great resource. Access the SOLIDWORKS User Forums here.