Join John Helfen for an in-depth discussion in this video Create rectangular feature patterns, part of Autodesk Inventor 2018 Essential Training.
- Let's look at how we can create a rectangular pattern of a feature. On the screen, you can see a model I've created to get started with. And in the browser, you can see we have a couple of features. We have Extrusion 1, which is our base feature. And we have Extrusion 2, which is a hole that's cut through. Now, I want to start off by mentioning a little information about patterns in general. And I talked about this in the sketch version of this as well. And that is that I generally try to keep all my patterns at the part level. Let me show you why I do that.
If we look at Extrusion 2 in the browser, and we click the plus symbol next to it, you can see that we have a sketch that defines the position of our first hole, or our extrusion, which is our hole. And if we were needed to, we could have in that sketch patterned that hole to create the pattern we're about to create. The reason I don't do that typically is because once the feature is created, in order to edit it, I'm going to have to find it in the browser, I'm going to have to expand it, I'm going to have to edit the sketch in order to be into a position where I can actually change the pattern itself.
If we do this at the part level, however, the pattern will actually show up in the browser as a feature, making it one level closer to edit. It just makes you more efficient. So, generally I try to do my patterning at the part level. It doesn't mean there aren't going to be cases where you do need to do it in the sketch, but I think you'll be more efficient doing it at the part level. Let's go ahead and look at how we can do that. If we go to the 3D Model tab under the Pattern panel and select "Rectangular," you'll see the Rectangular Pattern dialogue. Now, in the upper left-hand corner, there's a couple basic options.
The first one is to pattern individual features, and the second is to pattern a solid. Patterning solids is something that's beyond an essentials course. It's good to know that it's there, but we're not going to cover it. Instead, we're going to stick with what most people will do, and that's pattern individual features or a group of features. We're already in the feature selection mode, and right now we really only have one feature we could pattern. And we're going to go ahead and select that, and that's this hole. And you can either select it in the graphics window, or you could select it in the browser. Either is perfectly acceptable. Now, if there were additional features like a fillet or a keyway cut through here, we could add those as well.
But since there's not, we'll stick with what we have, and we'll select the Direction mode. Once we do that, we can select our first direction for patterning. I'm going to use the horizontal line at the top of the model. And when I do that, you can see that there is a preview and it's facing the opposite direction, and it's hanging off of the part. We can fix that with the Flip button here in the dialogue box. Now, this is just a toggle. Each time you click on it, it simply flips the arrow and changes the direction of the pattern. But the button to the right of that is a little more advanced.
It's going to turn this into a midplane pattern. What that means is when it's selected, you'll notice it's also just a toggle. When we toggle it on, you get an arrow in both directions. When it's toggled off, you're in a single direction. Now, it might not look like anything's changed. But if we bump this up to three occurrences or instances, you'll see a new one is added. And it's added off of the part, or in the opposite direction. What Inventor's doing is using the original feature that we selected as the middle of the pattern, and each time you increase this, it's adding one to each side of the model.
We don't want that, so we're going to uncheck this or toggle it off. And you'll see, it takes that third instance and moves it on to the model. Let's go ahead an bump that up to five. And you'll see that we don't quite reach the end of the model, so I'm going to change the spacing from one inch to 1.25, and what that means is you're going to end up with a distance of 1.25 inches between each occurrence in this pattern. There'll be 1.25 inches between the first instance and the second. There'll be an additional 1.25 inches between the second and third, and so on.
Now, we'll look at the spacing options in the next movie, but at this point, if we wanted to, we could select "OK" and we would create a single pattern in a single row. I wanted to point that out because you don't have to use this second direction every time. In this case, we're going to, but if you wanted to, you could simply select "OK" and stop there. Let's go ahead and select the second direction. And this time, let's select the vertical edge on the left. Here you can see the arrow is pointing down, and we still have the toggles to flip things and add midplane, but we're going to leave it as it is and we're going to bump it up to three occurrences.
Now you can see, not only is it just doing the one feature, but it's actually patterning the entire row that we created, which is exactly what we want. However, we need to bump this value up a little bit. The spacing value here needs to be set to 1.5. If we select "OK," you can see that our pattern is created. I'll double-click the middle mouse button to center it. And we have all our holes created. In the browser, we now see the rectangular pattern. And this is what I was mentioning earlier. Rather than having to expand an extrusion, edit a sketch in order to edit a pattern, now we have this pattern feature at the top level in the browser.
If we click the plus symbol, you can see that we have some information here. We have the feature that was extruded, and we have the individual occurrences that happened to be created during this pattern. We could simply double-click on the pattern to return to the dialogue box and make changes to that. And that's much more efficient than digging down into a sketch. So I just wanted to bring that up so you could see that. I'm going to go ahead and cancel this. And let's take a look at these occurrences. These occurrences are important because in certain cases, you're going to create a pattern but there might be a need to remove one of those items.
If you simply right-click on one of the occurrences, you can choose to suppress it, and it's removed from the model. It's just a temporary option, you can always return and right-click and select "Suppress" and turn it back on. But it's nice to know these are available. And they're easily reachable in the browser at the feature level.
- Reviewing interface changes
- Projecting and importing geometry
- Working with Autodesk AnyCAD
- Understanding part modeling
- Building parts with placed features
- Working with partial chamfers