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Patterning is one of the most efficient and powerful commands in SolidWorks. Features, bodies, or surfaces can be patterned and there's no limit to the number of instances. To get started we first need to select a feature or set a features that we'd like to pattern. Next we need to select the first direction and the number of instances in that pattern. Then, the spacing. If we want a pattern in one direction, we're done. However, if we'd like a grid pattern, like a set of holes or a vent for instance, we might want to select a second direction. Directions are chosen by selecting any edge or line that goes in the direction we want, the pattern to go in.
On the screen here, I've got a rectangular block, and I've got one hole, Extrude Cut 1 already set up. First thing's first, let's go ahead and choose that feature, and then come up here to the top of the screen, under Features, and click on Linear Pattern. My direction one is my first direction I'd like to go in, and that needs to be any linear edge. So in this case here, let's choose this bottom edge here. It could be that edge, it could be that edge, it could be that edge. Doesn't really matter, pick one. Choose that edge. Now you can see there's a little arrow, and a little blue line showing that pattern direction.
Next, let's choose the features to pattern. Well the feature to pattern is in the tree, and it happens to be that Cut Extrude 1. Notice it gives you a little preview of what's going on here. But it looks like the spacing's not correct, so let's go back up here to the Spacing and increase that a little bit. And you can see as I move, or increase the value, the preview moves on the screen. Let's go ahead and make that 1.2, and if we want to type it in we can set in type in 1.25. Now, we can control how many of these we want. So, let's zoom out a little bit, and then increase that number so it goes all the way across the part.
Now, if that's all we want, we just click on the green check mark and say okay, we're done, and there's that new pattern. But what happens if we want holes all the way across the part? Let's go back to Linear Pattern 1, open the Feature, and this time let's click on Direction 2. For Direction 2, I'm going to choose this edge here, so the holes are going that way. Choose how many we'd like, and I'm going to put two at first, and then I'm going to adjust that spacing. It looks like 1.4 will work just fine, and let's go ahead and increase the amount that we have in the pattern. Go one too many, you can see they'll cut off the edge, so we might want to bring that back one more.
And we can also adjust the spacing here so it fills it a little bit better. Once you have something that looks good, go ahead and click OK. But before we do that, I want to make sure that I point out that, we can also come down here to Skip Certain Holes. So go down here, as soon as you expand out, notice all these little pink dots that show up. Any one of those little pink dots you push, it will turn that instance off of that hole. So you can pick them at randomly, doesn't really matter, turn a few off, and they show up down here in this box, by the grid pattern.
If you want to bring one back, go ahead and click on it and delete if from that box which then brings it back in the view over here. When you're happy with what you have, click on OK, and there's all our holes. Patterning can be a huge time saver and the pattern features are easily adjusted. Patterning can be done in the Sketch Mode, however, that creates a large complicated sketch that's much harder to work with. I always recommend keeping your sketches as simple as possible, and Patterning and Mirroring bodies and features versus Sketches. The results will be the same and there are no rules. However, Feature Level Patterns are so much easier to work with.
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