Join John Helfen for an in-depth discussion in this video Creating rectangular feature patterns, part of Inventor 2014 Essential Training.
Now that we've learned how to create sketched and placed features, it's time to explore how we can pattern those features. Now we've already seen patterning previously in this course and that was at the sketch level. In the sketch creation process, we do have the ability to pattern sketch geometry in the same way we can pattern features and we have similar capabilities. We have a rectangular pattern, a circular pattern, and a mirror pattern, or a mirror feature. We're going to focus on the rectangular pattern in this movie, but before we get there I do want to call out the fact that while we have the ability to create sketched patterns, I typically try to keep my patterning at the part level, like what I'm going to show you here, and the reason for that is generally just design efficiency.
While I'm making changes to the design, I don't want to have to dig into the browser too deeply in order to make edits to my pattern. In the browser, you can see that we have Extrusion 1, which is the base rectangle, and we also have an Extrusion 2 which is this hole. And we could have, for example, when creating this sketch, patterned this hole, in a rectangular fashion, and created geometry that would work for our design. The problem is, is when we get to a point where we need to change that pattern if you pattern in the sketch, you first have to edit the sketch in order to be in a position where you can edit that pattern.
If we create the pattern at the part level, then just like Extrusion 1 and Extrusion 2, the feature will actually show up in the browser making it just one step closer to being able to be edited, and we'll just make things a little bit more efficient during the design process. Now that you know that, let's go ahead and look at the rectangular pattern. Rectangular pattern can be found in the pattern panel on the 3D model tab here at the top. And when we get into this dialog box, you can see there's a bunch of different options and we're going to explore most of these for this course.
We'll start out by talking about the two buttons here on the left. The top one which is the default option is the pattern an individual feature or group of features. The second option, which we're not going to cover in this course because it's a little more advanced, allows you to pattern a solid and what that means is when you get to more advanced features that may include certain surface modeling elements or work features, you can pattern a solid. And as it's patterned, it will join into one single solid. But I don't think it's something for an essentials course.
So we'll stick with what I think most people are going to do in most cases, which is just an individual feature pattern. Next we'll look at the fact that when we launch this dialog box, Inventor already placed us in the feature selection mode. You can see this because the arrow is red, indicating that Inventor needs some type of input for this portion of the dialog box, and it's depressed, meaning that's the active command. What I can do now is hover over the model and select any feature. And you will notice when I select that hole, Extrusion 2 is highlighted in the browser.
It is important to know that you can select either from the browser or from the model, because they are pointing to the same geometry. There's going to be cases where it might be easier to find something in the browser or find it in the window, and either one is perfectly okay depending on your design needs. The other item to mention around selecting features is you can select more than one feature. Right now we have only this extrusion selected, but if we had to fill it on the top of this hole or for example, maybe had to key cut through with this hole, we could select multiple features and pattern those at the same time.
I'm going to go ahead and stick with the single extrusion that we have selected, and we can look at the direction options we have. What's important to know about the directions is that you're not going to have to use both of them every single time. If I wanted to for example, create a pattern directly across the top of this part, I could choose a single direction. Let's go ahead and click that now, and I'll go ahead and select this top model edge, and you'll notice a preview is enabled. I could continue filling in the values for this dialog box, without selecting direction too, and go ahead and create a pattern in a single row.
In this case, we're going to look at both directions. But it's important to know that you don't have to use both every single time. As you can see on the screen, the preview for our pattern is showing that the pattern is going in the wrong direction, and we can use this flip option to the right of the direction arrow to toggle that to the opposite direction, and it is just a toggle. Selecting on it each time just flips the direction of the pattern over. And once you see the preview is in the right location, you can be done with that option. Next, what we'll look at is the button just to the right here, and that's the midpoint option.
I'm going to go ahead and check that. And at first you may think nothing's happened, but if I uncheck it you'll notice here on the preview, with that unchecked we only have a single arrow. If we check it, we get an additional arrow and what that means is Inventor is going to pattern in both directions. If I bump the number of instances up to three, you can see that we now have a mid plane pattern that shows one hole on one side, one hole on the other and the original hole is the mid-plane.
It's the middle of the pattern and it allows you to pattern in both directions. That's not what we're going to do here, so I'm going to go ahead and uncheck that. Now what you'll notice is because we didn't change the number of instances, Inventor has taken those, that same number of instances and moved them into a single direction which leads us to the next step. The next step is defining the spacing between the instances of the pattern. By default, Inventor has selected one inch, and it has selected a spacing option of just default spacing.
And what that means is, there is going to be an inch between each instance of this pattern. So for between Hole 1 and 2 there's one inch and between Hole 2 and 3, there's another inch. We'll explore the other options in the next movie. And right now, we're going to go ahead and add a second direction to this. But before I do that, I'm going to go ahead and bump this up to five instances, and I'm going to set the spacing to 1.25. And now you can see, we have five instances patterned evenly between both edges of this part.
There's a half inch on this side, and half inch left over on this side. I'm going to go ahead and select Direction 2 and this time, I'm going to select the vertical edge and we're going to set our instances to 3. So now rather than simply adding three new items, it's actually adding additional rows, making an array of the features. I'm going to go ahead and set this to 1.5 as the distance and I'll leave spacing set to its default spacing option. When you click OK, you can now see that we have a pattern of holes evenly distributed throughout this model.
I'm going to go ahead and turn on my edges here in the navigation bar with the Visual Styles button. I'm going to set it to Shade it with Edges, so you can see this a little more clearly. If you don't have this button, you can select the Visual Styles from the triangle dropdown at the bottom of the menu to turn it on. Now that we've created the pattern, you can see in the browser that we have a rectangular pattern feature listed and if we ever need to edit that, we can simply double click on the icon and bring up the original creation dialog box, and make edits to it just like any other feature in Inpattern.
The other thing you'll notice is if you hit the plus symbol, you have a link to the feature that was patterned and you have instances or occurrences of every single hole in the pattern. And the reason I wanted to call this out, is there's going to be certain times when you want to may want to suppress or remove temporarily, one of these occurrences. If for example, we wanted to remove this hole, we can right click on it and select Suppress. And we haven't deleted it, we've just temporarily turned it off. And you can leave it like that forever, but if during the design process you find out you do need that hole, you can always right click on it again, uncheck the suppress option to bring it back.
Now before we move to our next movie, I want to call out one thing that may have gone unnoticed in this video. And that's the fact that while we've created this pattern, we really haven't built too much intelligence into this pattern. And what I mean is if we go back to Extrusion 1 and double click Sketch 1 to edit it, we can make a change to this model underneath. I'm going to double click on the 6 value and set it to 8, and click Enter. And when I finish this sketch, the model's going to update, but the pattern is not going to update which is actually what we told it to do.
We told the pattern to use a spacing of 1 inch between each of these and I just set the value to 1.25 because I knew it would work out to be evenly centered on this part. In a lot of cases, that's going to be perfectly acceptable based on your designs, but in the next movie, we'll look at how we can add some intelligence to this so that as the part underneath changes, the pattern will update appropriately.
The course was created and produced by John Helfen. We're honored to host this training in our library.
- Customizing Inventor's menus
- Drawing rectangles, arcs, splines, and slots
- Moving, copying, and rotating geometry
- Trimming, splitting, scaling, and stretching geometry
- Creating work planes
- Projecting and importing geometry
- Creating extrusions, revolves, sweeps, and lofts
- Adding holes to a part model
- Creating rectangular feature patterns
- Creating iParts and iFeatures
- Using constraints to position parts
- Creating drawing views
- Setting dimensions