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In this video, we're going to be exploring how to create slots in Inventor. On the screen, you see a basic flange that includes three arced slots. This is the complete part, which you can find in the exercise files. I've also created a version that we can start with, that does not include slots. To begin, we need to create a new sketch on the face where we want to create our slots. I'm going to select the top face of this plate, and use the Heads-Up Display to create a new sketch. If I return to the home view, you'll notice that the sketch was created directly through the center of this part.
To clean up the display so that I can see the sketch more clearly, I'm going to right click in the Graphics window, and select Slice Graphics. Or press F7 on our keyboard. What that does is temporarily removes the solid model in front of the sketch, so that you can clearly see what you're working on. Again, F7 on your keyboard will toggle that on and off. Now that we're in the sketch environment, we can go to the draw panel, and look at the different variations of slots we can make. We have three version of a straight slot, and two versions of an arc slot.
I'm going to go through creating, one of each of the straight slots, just so you can see that they're all essentially going to create the exact same slot. The only difference will be that the input that you've selected to create the slot will differ. In this case, we'll start with the center to center slot. I'll left click to place my starting point, and I'll left click again to locate my second center point. That is essentially the centers of the circles on the end of each slot. The third option is to simply define the width of the slide.
The second option is to select the overall length of the slide. Rather than the center to center distance, I'm going to use those same points, what used to be the center point, and I'll left-click to locate the first starting point. I'll then move over and use the Heads-Up Display to align me to the center of the other slot. And when I left click, you'll notice that my slot can have a width defined, but now, I'm in line with this center point directly.
The final version of this is to create a center point slot. That allows me to create for example, a slot on an angle very easily. And I can select the center point. And as I drag, it extends in both directions. I can then left click to locate my final location. And I can then define the overall width of the slot. So you get the same basic shape. It's just different inputs that you select, in order to create that shape. I'm going to go ahead and select all these items and hit delete on my keyboard to remove them. Because what I really want to talk about here is the arc to slot that we're going to create on this feature.
Before we do that, we need to think a little bit about what we're trying to accomplish here. I want this arc to slot to be located directly between this circle and the outer circle. I could go and measure the diameters and do the math to figure out exactly what this diameter is supposed to be but, there's an easier way to do it with construction geometry. Since I know that I always want it to be centered, what I'm going to do is create a line that starts at the top of the circle here, and ends at the top of the outer circle. What I have now is a line that is exactly the distance between the outer circle and the inner circle, and the mid-point of this line is going to be exactly where I want this arc to lie.
Before I create the slot, I'll select this line, I'll right-click, and I'll change it to Construction. All this does is makes it so that Inventor ignores the line during the extrude process, but it allows me to use it to position sketch geometry. I can now go back to the Slot command. And select Center Point Arc. And, I can select the center point I want to start the arc on, and I can then move up to the midpoint of this line, and you'll see that it snaps into place at the midpoint. I can left click to locate that, and as I move my cursor, you'll notice that I'm now able to define the angle I want that slot to be positioned at.
In this case, I'm going to go ahead and enter 60 degrees. And now when i move my mouse I can define the overall width of the slot. Here I'm going to enter .375, and hit Enter on my keyboard. I now have the geometry I need to create the feature, now in the original part you saw, we had 3 of these, and I could continue sketching, or I could use the array in the sketch. But what I'm going to do is finish this sketch, extrude this feature by right clicking and selecting Extrude from the marking menu. And extrude this slot.
Rather than joining material, I'll set it to cut material away. And rather than extruding to 1 inch, I'm going to set the termination to be through all. I'll click the check box to accept that feature. And you can now see I have one of the slots created. So, rather than drawing it in a sketch, I'm going to use the pattern feature here at the part level, to select the slot we just created, and then create a circular pattern around a rotation axis. In this case the center boss.
Rather than six elements, I'm going to set this to be three elements, and now I have three slots evenly distributed over a 360 degree range.
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