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As we continue to learn about editing sketch geometry, in this movie, we're going to focus on the patterning commands. I'm going to start by creating a new part file by selecting New on the toolbar, selecting standard.ipt as my template, and clicking Create. Now that we're in a part file we need to create a new sketch. I'm going to go ahead and click create 2D sketch and select one of the origin planes to sketch on. I'm going to begin by creating a basic circle at the center of the sketch. I'll left click to locate it's center point, move my cursor and in the heads up display I'm going to enter one inch.
And hit enter to create the circle. Next I'm going to create a basic line, from the center of the sketch, up to about a quarter inch. The dimension doesn't really matter exactly in this case, but. Actually, let's go ahead and increase that to 0.375. I just double-clicked on the dimension to edit it, and now you can see it's a little bit closer to the edge. And we'll finish up this starting geometry by right-clicking, selecting Circle, and creating a circle on the end of that line.
In this case, I'll make it 0.125 in diameter, and hit Enter to create the circle. I now have a basic circle, and what I'm going to do is use the circular pattern command in the sketch to pattern this geometry around the circle. We can go to the Pattern panel and select Circular Pattern and we're presented with a dialog box that has our settings and by default, we're into a selection mode. This is very similar to the move, copy and rotate commands where I can select specific geometry that I want to pattern.
I'm going to select this line and the circle as what I want to pattern and then I can select the axis that I want to pattern around. I'm going to left-click to select the axis command, and in this case I'm going to select the center of the circle. By default, Inventor uses six items, and patterns it in a 360 degree pattern. If you only want four, you can simply change the number in the pattern updates and that's the case for any of these. So we'll go head back to six, and you can also adjust the degrees in which the pattern is going to take place.
For example, I could do 60 degrees and in this case you can see that they're all bunched up. So, if we were only going to go 60 degrees it might be make more sense to use three for example. So you can use these values to adjust your pattern to your specific need. I'm going to back and set this to 6, and I'll return and set the angle to 360s, or a full revolution, and I'll hit OK to create the pattern. Now a couple of things are important to know here.
The pattern is going to be defined by this original geometry, and it will act as a single unit. Even though you can select the individual pieces of geometry, if you right-click on one of them, you'll find that you have an option to delete the pattern, suppress an element within the pattern, or edit the pattern, which essentially brings back up the dialog where you can start again. Or continue where you left off. The Suppress command can come in quite handy. If you right-click on one of the pieces of geometry in the sketch, or in the pattern, you have the ability to suppress specific elements.
This can come in handy where you want to have offset patterns, but generally most of the geometry is in that type of pattern, like a circular pattern. Next, we're going to look at the Mirror command. We're going to continue by creating one more piece of geometry so this component is not as symmetrical which will make it a little bit easier to see the mirror command work. I'm going to go ahead to the rectangle command, but instead of using two-point rectangle, I'm going to click the arrow next to it and select 3 point rectangle. And I'm going to select the point, any point up near the top of the circle.
I'll point directly across from it, and I can drag up to define the length of the rectangle. Next, what I'm going to do is right click on this line across this. Circle, and convert it to construction. The reason I do this is that, if you zoom in a little bit, you can see that this line crosses that circle, so that if you use these profiles to exclude. Part of that circle might be cut off by that line, so by turning it to a construction line, inventor is going to ignore that line when it's creating geometry in a 3D space.
Now that I have this in place, we can look at the Mirror command. The Mirror command is also found in the Pattern panel. And works in a very similar fashion. If I select the geometry I can then go to a Mirror Line and select that line. And when I click Apply. You see that, that geometry is mirrored. Now I'm going to go ahead and click Done, a I'm going to right-click and select Undo. Because there's one more item that I want to make sure that everybody's aware of. If, for example, we needed to mirror this but we didn't want to use this line on the geometry, you can also draw construction geometry.
For example, I can draw a line here. Finish that and covert it to construction by right-clicking and selecting Construction. Now you don't have to do that. Because it's just floating out in space and doesn't create a closed loop, Inventor will ignore it for the most part. But it is generally a good practice if it's not going to be part of the sketch. That's being turned into geometry in the 3D space to use a Construction mode. Now if i go back to the Mirror command and select the geometry I want to mirror, I can use the Mirror Line as construction geometry to essentially create an offset mirror.
It's just one of those items that I want to make sure everybody's aware of because it can come in handy. Now that we have some other geometry created we can look at the rectangular pattern command. That's found in the pattern panel as well and works in a very similar fashion to the circular pattern. If we select our geometry, which is the default tool that shows up in the dialog box, I can then select a specific direction. I can either select the construction geometry we created or any of the geometry within the sketch.
Once you select that, you can see that we have two instances. An inch apart. You can set this number to as many as you need. For example, let's do 3 at an inch and a half apart. What you'll also notice, is we have these double arrows. Which, if your hove over it, says flip. All that does is just changes the direction. From one side to the other within this command. You'll also notice that what we've done at this point is done a linear array in a single direction.
We also have the ability to select a second direction. If we select that, and that select a vertical line, you can see that we're starting to get a more complex pattern. Let me go ahead and change this to 2 inches. Well, that's not even enough, let me go 4 inches. And now, what I've got is two instances of these patterns four inches apart. Again, you can go ahead and change this to three, for example. And now we have three patterns, and just like with the other direction, you can use the flip command to toggle the direction of that to create the array.
I'm going to go ahead and hit OK, and we now have these pieces of geometry pattern. In a rectangular pattern. Just like we had before, you can right-click on specific pieces of the geometry to suppress them, or you can delete the pattern as a whole to go back to the original geometry. Again, once you've done the pattern, it's important to remember that if you're going to delete a pattern, that you will keep the original geometry.
But that's not the case in a mirror. In case the, the mirror, you'll need to select that geometry and hit Delete to remove it.
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