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Now that we've learned how to create the eye feature, let's go ahead and look at how we can place the eye feature. We're going to do this by starting with a blank part. We'll click New on the toolbar, select standard.ipt as the template and click Create. Now to begin, we're going to need a base feature. In the previous movie when we were authoring the part, the holes were placed on a flat plate. That was the base feature. So let's go ahead and create that. I'm going to go ahead and right click into graphics window and select create new sketch. And I'm going to select a plane to sketch on in the graphics.
Next I'm going to right click in the graphics window and select two point rectangle. And I'll left click on the center point to locate the starting point of the rectangle. From there, I'm going to use my head's up display. I'm going to enter three as my value for my length. I'm going to hit tab on my keyboard and I'm going to enter two for the height. And then I'll hit enter on the keyboard to create that, and I'll finish the sketch to return to the modelling environment. If you click home, you can zoom out and see all of the items you just created.
And we're ready to extrude this. So now I can right click in the graphics window Extrude. And I'm going to enter a value of .125. And his Enter on the keyboard to create the base feature. We now have Extrusion one, which is our base feature in the browser. And we're ready to place our iFeature. The eye feature can be placed from the Manage tab under the Insert panel here at the top, Insert Eye Feature. And by doing that, it's going to bring up the dialog box, and I'm going to go back to the location where we saved our eye feature.
And this is in the exercise folder. And you can see iFeature one. And I'm going to select that by left clicking on it. And you can see the insert iFeature dialog box. Now, when we were authoring the iFeature, there were a couple of prompts that were added. And there was a couple different items in the dialogue box that were set up. There was positioning, and there as sizing. Here in the dialogue you can see that position is highlighted, and is looking for the same plane that we would have selected had we drawn all of this information on our own.
So it's looking for a flat sketch plane. You can select the face that we want this on. You can select the edge. You can select the other edge as well, and any flat face at this point would be valid. And we're going to simply left click on the one we want. After doing so you can see that we have the sketch page selected and we now have the ability to move this around on this face by selecting the arrow and then moving our mouse. So if you want to position it a little more close to where you think it's going to be located You can do that, or if you click the arrow and then move your mouse, you can change the angle.
So, it is possible to position this at any location and in any angle you want, depending on your designs. I'm going to locate it there and go back to the dialogue box because you can manually override that with an exact value here as well in the dialogue box. I'm going to go ahead and set it back to zero because I want to keep it in it's original position and I'm ready to continue by hitting the next button. Now you can see the additional prompts that we had and the different items for sizing. We had the ability to change the length between the two holes and we have the ability to change the whole diameter.
And here you can see when we select one of these, the prompts that were entered into the authoring tool when we created this iFeature. If we select the second one, it says enter how old I am. And I could change this to three, for example, if, for example, I knew the iPart that we were going to attach to it was longer, but in this case, I'm going to go ahead and leave the values as they were. And continue on by hitting Next. The final item is to decide whether you've positioned it where you want, and that's final, or whether you want to activate the sketch immediately to begin editing.
Either one is completely fine. If you choose not to activate the sketch, you can simply double click the sketch in the browser to edit it. Since I know that I don't have exact positioning set, I'm going to go ahead and select Activate Sketch immediately. And when I hit finish, is going to automatically rotate me into a normal view of the sketch and begin editing the sketch. You can see here that I didn't have to create the whole centers, this construction line or this dimension for this item.
What I do have to do, however, is locate this. Because if I left click and drag this is free floating anywhere. But you can see here that using eye features might not be appropriate when you're going to just simply place two poles. But you never know, if you place this over and over and over and over again. In the end, it would save you significant amount of time to not have to click to create each of these items in the sketch plane and all of that information. If you could just use an iFeature to do that. But, what's nice here is I can right-click in the graphics window General Dimension, and I can use this sketch to locate this specifically where I want.
In this case I'll go ahead and enter .5 from the edge, and I'll left click on the construction line and then left click on the horizontal line to enter, let's see, .375. By doing that I've perfectly located this item, and when I hit finish sketch you can see I've placed the eye feature. It shows up in the browser, and you can see the sketch here that drives it. At any time, you can go back and double click this sketch, and make edits to it. If I finish that sketch, you can also go back and right click on this, and select Edit iFeature to return to the creation dialogue box where you could edit the lengths just like you did when you were creating it.
I am going to go ahead and cancel that, but hopefully you can see how iFeatures can speed your design process if you have features that you are creating over and over again.
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