Join Gabriel Corbett for an in-depth discussion in this video Use the Curve Driven Pattern tool, part of SOLIDWORKS Tips & Tricks.
- [Voiceover] In this movie, I'm going to be showing you how to use the curve-driven pattern. Now, the curve-driven pattern is a very powerful tool and it allows us to lay out a bunch of holes along a pre-defined path. My first example's gonna be this one over here, and you can see I've got a piece of tube or bar that's been bent into this shape. And I'd like to have some holes that kinda follow that same profile. Now because this is a sweep, I already have a pre-defined path. So I go over here to the Sweep number one, I choose this path, now that's right in the center of that. Now if we didn't have a path directly in the center of your part, you might create a sketch on the top surface, maybe an offset into your convert amenities along that outside edge, and use that as your path.
But in this case I already have the path, so let's go ahead and just use that. So choose the path, and then the feature you'll wanna pattern is this one here, which is Cut-Extrude1. I'm gonna go ahead and control select both of those and come up here to Linear Pattern and directly below that is Curve-Driven Pattern. Okay, as soon as I have that, notice I have that path pre-defined over here, I've got the amount of holes I'd like to put in here, and notice I'm gonna switch the direction, so notice it comes all along this edge here, and I can update or change the amount of holes. And notice they're equally spaced, which is really handy.
If you change and turn that off, I can then have these so they kinda follow along that path with however many I'd like. You can also change the spacing to your liking. I have a couple options down here as far as tangent curve or offset curve, in this case it doesn't really matter, 'cause we're directly on top of the curve or the patterning profile that we're putting the holes on, so you'll see some examples of that in the coming examples. The features or faces, this case here, I'm choosing just that hole, but you can pattern multiple features at the same time, or faces, you can even choose individual bodies to pattern along.
Just like any other patterning type of tool, I can also skip certain instances of it, just by clicking on the little pink dots, it just turns those ones off. And you can turn them back on by choosing the orange dots and turning those back on. And once you have it all set up, go ahead and click on the green check mark and there's our curve-driven pattern. Now the next example is gonna be this line right here. Now you don't always have to have a curve, it can be a straight line, that works just fine. But I'd like to pre-define a certain amount of holes along this line segment right here.
So the first thing I wanna do is get into that sketch. So click on that, Edit Sketch, and notice I've got it pre-defined five inches from the edge here and I've got an equal relationship on both edges here. So if I change this value here to two, notice both sides change so I always have this line segment directly in the center there with an equal spacing on either side. This is gonna be a prime example of when you wanna put a bunch of holes in the center of your part, you don't want them going off the edge of the part. So once I have it pre-defined, let's go ahead and change it to three inches, and then exit out of that. Now I wanna start a sketch directly on top of that, so click over here, click on Sketch, I'm gonna choose a circle command, and I'm gonna zoom in here, and I'm gonna start that circle right on that hole.
Add a dimension, let's say it's one inch. And then go up here to Features, do an Extruded Cut, and let's go ahead and extrude it all the way through the part. Click on OK, and there's our hole. Now go back to Linear Pattern, directly below that is Curve-Driven Pattern, my direction's going to be this line segment right in the center. And notice as soon as I do that it puts these holes along that, and what I'm really looking for in this case is equal spacing. So I'm putting a hole in the beginning and I have a hole at the very end, and I have however many instances I'd like across that line segment between the two.
If I change the values of these lines at the end, that's automatically gonna smush those together or stretch them out. So I'm gonna define that a little bit less, let's say there's gonna be 12, and then click on OK. And just that easily I was able to create an equally spaced set of holes across the line segment. This is very handy and a lot easier than the other alternative way to do the same thing. Okay, my last example here is gonna be this little pin that's been extruded up. I'm gonna go ahead and choose the pin itself, then I come over here to Linear Pattern, directly below that is Curve-Driven Pattern, and my directions are just gonna be this outside edge.
So I choose that, and I just wanna show an example here of what the different types of curve methods are. Notice I have the part already selected, and I'm gonna go ahead and choose the, oh, hold on. Click on the top. Don't choose the part itself, we don't want that, but I do want to show you that, if I'm using this Transform Curve, what it's doing is it's pushing all these parts down below the curve. Notice the spacing here, it's just pushing all of them kind of below that curve, and that's not really what we want. So what we want to do is offset the curve. Notice that pushes everything on the inside of it, and that's a lot more what we're looking for.
You can also switch between tangent to curve and align to seed, but in this case, it doesn't really make any difference. Once everything looks pretty good, just go ahead and click on the green check mark, and there you have it. So the curve-driven pattern, a very useful tool, you can use it with all types of different features, whether they're a extruded boss, a cut hole, a body itself, or a surface, and a lot of different ways you can use it it's gonna save you a whole lot of time. That's the curve-driven pattern, check back next week for more tips and tricks. Thanks.