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Now that we've learned how to create sketch geometry, it’s time to talk a little bit about construction geometry within the sketch. Construction geometry, is very similar to standard sketch geometry, with one little twist, and I'll show you what I mean as we move along. To begin, we're going to start by creating a new part by clicking the New button in the tool bar. Next, we'll select standard.ipt as our template and select Create to launch the new file. Now that we are in a new part file, we can begin by creating a new sketch.
We'll select Create 2D Sketch from the Sketch panel. From the origin geometry, we'll select a plane to sketch on, and we are now in the sketch environment and ready to create geometry. The easiest way to see construction geometry, is to let Inventor create it for you, and we'll do that, to start, by creating a specific type of rectangle. Rather than the two point rectangle, which is the default in Inventor, we're going to use the arrow next to the button and select Two Point Center Rectangle. This will allow me to define a rectangle by selecting a center point and one of its corners.
I'll hover over the center point and left click to locate the center. And as I move my mouse, you'll notice that geometry is being created. The outer lines are solid. And the inner lines that are crisscrossed are dotted. If I left-click to locate the corner, you can see the actual geometry being created. The green lines are indicating standard sketch geometry, while the dotted yellow lines are displaying construction geometry. Essentially, any piece of sketch geometry can be converted to a piece of construction geometry.
All you have to do is simply right click on a standard piece of geometry, and you'll see an option to select Construction or Centerline. In this case, we're going to use Construction. Both of them act very similar, and are turned on and off in the exact same way. By selecting Construction, you can now see that that top line has been converted from a Standard Piece of Geometry to a Construction Geometry. I'm going to do that one more time. I'll right click on that same line again, but this time, you'll notice that the Construction Option has a check box in it, indicating that this is currently in Construction Format.
Selecting it a second time returns it to standard sketch geometry. And that's the same for any kind of sketch geometry you create. Next, I want to point out why ,construction geometry is so important. In this case, we're using the sketch geometry that Inventor has automatically created to be able to define the center point of this rectangle. But, more importantly, if we finish this sketch, and apply an Extrude command to this. Which is actually part modeling, which we don't need to understand exactly yet. But it is important to understand where we're going so that you understand why construction geometry is so important.
If I right click in the graphics window and select Extrude, you'll notice something happens. Inventor has automatically selected, the outer rectangle, which was indicated by the green lines in our sketch, and extruded it to a specific depth. I'm going to go ahead and cancel this by clicking the red x in the heads up display And, return to the sketch editing environment, by double clicking the sketch in the browser. You can see we're now back in the sketch environment and what I'm going to do is convert one of these pieces of construction geometry to standard geometry.
I'll right click on it and select Construction. And, you'll now see that it's green, just like the outer lines. This time, if we finish the sketch, right click in the graphics window, and select Extrude, you'll see that Inventor hasn't selected a profile. And the reason for this is it's entered us into the profile selection portion of the command. But, since we've converted that construction geometry to standard geometry, Inventor now can use that line to interpret the closed profiles that are created by these shapes.
I now have two triangles that when selected will actually create the exact same shape we saw before, but we've done it by selecting two separate profiles. This comes in very handy when you become more proficient with sketching so that you can use construction geometry to help locate your standard sketch geometry, but you can also use it to understand the different ways to create profiles as you get more involved with design. I'll go ahead and cancel this command, and we'll go back into the editing environment by double-clicking the sketch in the browser.
And I'm going to right click on that piece of geometry and convert it back to construction. The other way we can create construction geometry, is by simply drawing any sketch item. For example, if we draw a line. Or, if we draw a rectangle, and finally, if we draw a circle, any of these pieces of sketch geometry can be converted, by either right clicking on em individually and selecting Construction. Or using a window to select the geometry and then right click and select Construction and you can change multiple items at once.
The final way you can create construction geometry, is if you know you're going to create several pieces of construction geometry at one time. You can go to the Format panel in the Sketch tab, and toggle on Construction. By doing this, any geometry created is automatically in a construction format. This comes in handy when you know you're going to be creating some construction geometry all at once. But I personally don't use it, because it's very easy to finish your construction geometry, perhaps take a break or walk away and then come back, and start creating geometry again, not remembering that you have construction enabled.
Which means you're going to probably have to go back, and select that geometry, right click, and convert to an alternate type of format anyway. It's a matter of preference. They all work exactly the same, so it's up to you as the designer to select which works best for you.
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