Join John Helfen for an in-depth discussion in this video Construction geometry, part of Autodesk Inventor 2018 Essential Training.
- [Voiceover] We're now ready to look at Construction geometry. We're going to start by creating a new blank part, by clicking New Part in the dashboard. We now have a blank part and we need to start a sketch. I'm going to right click on the Graphics window and select New Sketch, and select the x y plane in the origin planes. This gives us a sketch to begin with. And really the easiest way to see Construction geometry created, is to let Inventor do some of that work initially for you. To do that, we're going to create a rectangle but rather than use a two point rectangle, we're going to go to the Sketch tab, under the Create panel and click the drop down below Rectangle.
This will expand to show all the rectangles and slots we can create, and we're going to look for the Two Point Center Rectangle. What this is going to do is create a rectangle by defining a center of the rectangle and one of its corners. During that process, Inventor's going to create Construction geometry to do this. We're going to hover over the centerpoint of the sketch and left click, and as we move the mouse you can see that our rectangle is being created and there's some Construction geometry represented by the dashed lines, also being created.
If we go ahead and left click to place the other corner of the rectangle, our geometry's created. I'll go ahead and right click and select OK to get out of the command, and now you can see our geometry. The green lines around the outside are standard sketch geometry. Those would be like any other geometry you've sketched in any way you've learned already. The yellow dotted lines, however, are Construction geometry. Now what Inventor has done, is use these Construction geometry lines in order to find the center of this rectangle. If you draw a line from corner to corner on both sides, the intersection point is the center of this rectangle.
So what Inventor's done is created a coincident constraint between the midpoint of the Construction geometry and the centerpoint, in order to locate this rectangle. Now we can go ahead and change any regular geometry to Construction geometry. If you, for example, right click on the horizontal line at the top, in the marking menu, you'll see Construction and Centerline. Both of these work exactly in the same way. If you left click and select Centerline, you can see that the geometry's updated to reflect a centerline.
It's slightly different because the centerline can be used in other types of features, but it works in the same way. Selecting Centerline again will return it to standard geometry, and we can even do that one more time and select Construction, and this time you get the yellow dotted line. Let's go ahead and turn that back into standard geometry and let's finish this sketch. Because what I want to do now is show you how this construction geometry affects the overall part modeling. You've seen how it can help you locate centerpoints of rectangles, you might use it in other ways as well.
But, when we right click and select Extrude, and you don't need to understand the Extrude process yet, we'll look at part modeling in a little bit. But what's important here, is how the sketch geometry affect part modeling. What happened, is you can see Inventor automatically selected the one closed profile it had, which is the large green rectangle. If I hit Escape, and we return to editing this sketch by double clicking the sketch in the browser, let's see what happens when we take one of the Construction geometry lines and convert it to standard.
By right clicking on it, and unchecking Construction, this line now is green like the outer lines. This time, if we finish sketch and we right click and select Extrude, Inventor doesn't select the overall rectangle. And that's expected, because previously, it was ignoring the Construction geometry when trying to infer what was a closed loop or a closed profile. This time, it's seen this diagonal line as a separator between the two. So, if I select the bottom section, I get a triangle from the bottom, if I select the top, I get the entire rectangle.
The only difference is I had to select multiple profiles to do it. The overall shape is exactly the same, it really doesn't matter how you do it, either way is perfectly fine depending on your needs. I'm going to go ahead and hit Escape on the keyboard to get out of that, and double click on the sketch in the browser to edit it one more time. Let's go ahead and right click on that line and convert it back to Construction. We're going to zoom out just a little bit so we can talk a little bit more about other options we have. As I mentioned earlier, any sketch geometry you create can be converted to Construction or Centerline.
It doesn't always make sense that everything would be changed, but it's important to know that that's possible. So let's go ahead and right click and select Create Line and we'll just create a few lines here. Then we'll right click and select Circle, create a circle, and we'll right click and select Rectangle. We've created a few different pieces of geometry and you could go back and individually right click on every single line and convert it to Construction. Instead, we could also left click and drag a rectangle around all the geometry, right click, and select Construction to convert them all at once.
Now there's going to be times where you may create a large amount of Construction geometry. So the final option is to enable the format before you start creating geometry. Now I don't do this just because sometimes I forget that I have it on, and it ends up causing me more work just to undo it, but there are going to be cases where it might be very beneficial for you. So if you look at the Sketch tab, under the Format panel here on the far right, you have a couple of options. One is Construction, and one is Centerline.
If you check these, or toggle these on, any geometry you create from this point forward will be Construction geometry. If we create a couple of lines, if we create a circle, those are all going to come out as Construction geometry because we have the format set to be Construction. Now the only problem with this is, if I were to walk away maybe get a cup of coffee or something, maybe a colleague comes by and talks to me, I might forget that that's on, and if I start creating geometry, it's going to be in that format.
It's not a big deal, it's just one of those things that could catch you off guard, so I'm going to toggle that off, and with it toggled off if you create geometry, you're back to standard sketch geometry. This should help you understand how sketch geometry is created and where it might be beneficial for you during your design process.
- Reviewing interface changes
- Projecting and importing geometry
- Working with Autodesk AnyCAD
- Understanding part modeling
- Building parts with placed features
- Working with partial chamfers