Join John Helfen for an in-depth discussion in this video Pattern and mirror sketch geometry, part of Autodesk Inventor 2018 Essential Training.
- [Voiceover] We can now explore how we can modify geometry with sketch patterns. On the screen, I have a blank Part. I'm going to right-click and select New Sketch, I'm going to select the XY plane to sketch on, and then I'm going to start with the Circular pattern. I'll right-click and select Circle, start at the center of the sketch and left-click, and then drag a circle out, we'll say 1.25 inches. Next, we're going to right-click and select Line. We'll start by clicking the center of the circle and dragging directly up .5 inches, entering that into the Heads-Up Display.
.5, and then hit Enter on the keyboard. Next, we'll right-click and select Center Point Circle, and create a circle on the end of that line. We'll enter .125 as a diameter. You can right-click and click OK to exit the command, and we're now ready to move forward. We can start a Circular Pattern by going to the Sketch tab under the Pattern panel, and selecting Circular in the center here. When the dialog comes up, you can see that Inventor has automatically selected the Geometry arrow, and it's red.
This indicates that Inventor doesn't have everything it needs to move forward. What it wants us to do is select geometry. So, I'm going to go ahead and select this circle, and the arrow updates to white. It doesn't mean you have to stop selecting geometry. We could continue selecting. It simply tells us that it has at least enough information to move forward. The next area is the axis. It is a red arrow, meaning it still needs selection. We'll select that, and then we'll select the center of the circle. And by default, Inventor starts with six instances at 360 degrees, or a full revolution.
You can make changes to these by simply updating the dialog box. Setting it to five updates the geometry so you that can see it. If we went and set this angle to 90, you would see that we have five instances, the starting geometry and then four additional items, where the centers are exactly 90 degrees apart. I'm going to go ahead and set this back to 360, and bump this back up to six. Clicking OK will create that geometry. Now, what's important here is, now that the sketch has been patterned, any of these elements in this sketch, for example this one down at the bottom, if we left-click on it and then right-click, our scene is a single entity.
We have the option to now delete the entire pattern, suppress this element, or edit the pattern. If we edit the pattern, we're placed back in the Circular Pattern dialog, and we can continue where we left off. I'm going to go ahead and cancel that, and this time, I'm going to left-click on the bottom left circle, right-click, and now we have the option to suppress an element. This comes in handy when you have a general shape, but there might be one or two items that are out of place or removed from this. Next, we're going to look at the rectangular pattern.
We're going to slide that off to the side, right-click in the Graphics window, and select Two-point Rectangle. And here, what we'll do is we'll start a point down in the lower left, and we'll drag a rectangle that is one inch, we'll hit Tab on the keyboard, and then we'll go one inch in the other direction as well, and hit Enter. We now have a one by one rectangle, or square, and we're going to right-click and select Center Point Circle. And here we're going to go ahead and place this in the lower left-hand corner, and we'll set it to .125, and hit Enter.
Next, we're going to right-click and select OK to get out of that command, and we can look at creating a rectangular pattern. The Rectangular Pattern command is also in the Pattern panel, here at the top. Just like the previous dialog, you see a lot of arrows here that are red, meaning they need information. It starts with the geometry. In this case, we're going to pattern the circle here. By selecting it, the arrow updates to white, meaning it's ready to move forward, and we can select a direction. The first direction I'm going to select is bottom horizontal line, and you can see it creates the first instance off to the right.
If you want it off to the left, you can simply hit the Flip command here in the dialog box, and you can change the direction of that specific item. Next, we're going to update the distance from one to .25, which is a little more appropriate for this design. Next, we'll bump this up to four, and you'll see we've run a little close to the outer edge. And that's fine, in this case, we're not super concerned with that. What's really important here is now we have the ability to create patterns quickly.
We can also select a second direction. If we select the red arrow, we can now select this vertical line, and if we zoom out, you can see that we're creating additional geometry in that direction. We'll use the Flip command to switch to the opposite side, and we'll bump this to four, and we'll drop the distance down to .25 again. You can now see that we have a pattern of four by four, at a quarter-inch apart, and by selecting OK, you can see that we have that geometry created.
Now, because this is out of center, we can see how a Mirror would actually work. Let's go ahead and mirror this geometry real quick, just so you can understand how Mirror works, and it's very similar to the steps we've already taken. We'll go back to the Pattern panel and select Mirror, we'll select the geometry we want to mirror by (unclear) left-clicking and dragging across it, and then we can pick a mirror line. If we select this bottom horizontal line and then hit Apply, you can see that a lot has happened.
First, let's go ahead and hit Done in the dialog. All of those constraint icons were symmetry icons. What that means is Inventor has automatically mirrored this, and added symmetry constraints to each of these circles so that their corresponding partner on the opposite side of the mirror is exact. Now, if we zoom in and we double-click on this dimension and change it from .125 to .2, you'll see that all of the circles update in the pattern. If you drop down to .1, they also update again, without expanding outside of the rectangle.
At this point, you can get out of the sketch and begin modeling this component.
- Reviewing interface changes
- Projecting and importing geometry
- Working with Autodesk AnyCAD
- Understanding part modeling
- Building parts with placed features
- Working with partial chamfers