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In this movie we're going to focus on circle and rectangles. Now, because this is the last movie in the sketching chapter, we're also going to bleed a little bit into part modeling as we create the geometry to sketch on. It's not important that you understand everything from a part modeling aspect, because we're going to cover that later, but I think you'll start to see how sketching and part modeling are connected as we move through this video. We're going to begin by extruding this base plate that we've been creating over the previous movies. We're going to right-click and from the Marking menu select Extrude.
We can then select the two profiles that we created and give them an overall Height of .125. We can hit Enter on the keyboard to accept that value and our initial base feature has been created. You can see it here in the browser as Extrusion1. Before we continue sketching we need one more item added to this part, and that's a fillet. We're going to fillet each corner. We're going to start by selecting this first corner and the Heads-Up Display will present a Fillet and Chamfer option. We're going to select Fillet, which is the rounded corner, and we're going to work our way around the parts, selecting each corner edge.
You can select through the part, so I can get to this vertical edge in the back simply by selecting through the part. And once I've selected all four corners, I'll hit the check box to accept those. We've now created our base feature that we're going to build from, and we can begin looking at circles and rectangles. But before we do that I'm going to switch back to the faceplate, which is the completed part so you can see where we're headed. In this case, you can see where the base plate is located here, we're going to go ahead and create circles for these bosses on each corner. We're going to create a circle for the boss in the center.
We're going to create the center hole, and we're going to create a rectangle that locates these holes around the main boss. We'll switch back to our part and continue along the way. We're now ready to being sketching circles. We're going to start with the boss in the center of the part. To do that, we're going to select the top face and from the Heads-Up Display select Create Sketch on the far right. A couple of things happened, we rotated so that we're looking normal to the view. We're straight down on the sketch. And you'll notice the yellow lines were projected from the edges of the part below.
We're going to leverage this projected geometry to create the center boss of our part, and the reason for that is this boss needs to be perfectly centered in the middle of the base plate. To do this, we're going to start by Creating a Line--which we learned about in a previous movie--and we're going to start our line at the center point that was projected from the part. You'll notice as we hover near the center point a green dot appears, which indicates a coincident constraint is going to be applied. We can then hover the end of the line near the center point on the opposite corner, left-click to lock that into place.
We can hit Escape on our keyboard to get out of the command, and you'll notice we now have a line that's locked to the center points and the dark purple color indicates that it's permanently constrained. The next thing I'm going to do, I'm going to select this line, and because we're using this simply as a construction piece of geometry, we're using it just to create a midpoint that we can lock to, select that line, right-click, and the Heads-Up Display has changed to indicate things I can do this line. I could turn it to a Centerline, I could Delete it, or I could convert it to a piece of Construction geometry. That's what I'm going to do.
And after doing so you'll notice the display changes a bit. It's now a dashed line, and what that indicates is that it is construction geometry, and it will be ignored when creating modeling features. All it's there for is so that we can center our circle or our boss on the midpoint of this line. From the Marking menu I'm going to select Circle. I can now hover near the midpoint of this line. Again, I get the green dot to lock the center point to the midpoint. I'm going to left-click to place and begin to drag my circle out. Now, you'll notice the Heads-Up Display for a Circle is showing a Diameter dimension.
In this case, I know we need a radius dimension. So before placing the circle, while I'm in the middle of the command, I can right-click, and I do have an option to change to Radius. If at any point you need to switch back, you can simply right-click while you're in the middle of the command and switch back to a Diameter, it's just a toggle back and forth. In this case, I'm going to go ahead and right-click one more time because I do want that Radius value, and I'm going to enter .413 as my value. I'm going to hit tab on my keyboard to accept that, and then I'm going to left-click to place the circle.
I've now completed the sketch, and I can right-click in the graphics window and select Finish Sketch from the Marking menu, or I can go to the toolbar and select Finish Sketch at the far right, both do the exact same thing, and it's a matter of preference. From the Marking menu I'm now ready to extrude the circle I just created. I can select that circle on the screen and enter a value of .315 for its Height, hitting Enter on the keyboard will accept that value, and the boss is created. Now, it's a little hard to see because of the coloring. I'm going to use my Visual Styles, which we turned on in the navigation tools video, and I'm going to turn on my Shaded with edges option.
This allows me to see the top of the boss a little more clearly and will help as we continue along sketching. The next thing we need to do is add the bosses around each corner. I'm going to sketch on the same face again. It rotates into a Normal view, but this time you'll notice something happened. If I orbit a little bit, you'll notice that this sketch actually runs through this part. Now we're ready to create our circle bosses in each corner. I'm going to use the Marking menu to access the Circle tool, and in this case I'm going to use the projected geometry to completely define these bosses.
I'm going to hover over the center points of the fillets to lock my center point of the circle to that, and I'm going to hover up near the edge of the part to get another coincident constraint. I'm going to left-click, and you'll notice the circle that's created is automatically purple. The center point is locked to the fillet and the outer edge is locked to the edge of the part. This completely defines the circle, and I don't have to add any dimensions. If the fillet underneath changes, the circles will also update. I'm going to work my way around and repeat that process for each of the corners, and we'll be ready to extrude our bosses.
With those completed, I can hit Escape on my keyboard to get out of the Circle command, and I can right-click and select Finish Sketch from the Marking menu. Now we're ready to extrude those bosses. I can right-click on the Marking menu and select Extrude. I can select each of those bosses that I just created, and I can give them an overall Height value of .16. Hitting Enter on the keyboard accepts that value and the bosses are created. Next, I'm going to create the center hole that goes through this boss. To do so, I'm going to start a new sketch by selecting that face and from the Heads-Up Display select Create Sketch again.
Now that we're in the sketch environment, the Marking menu has my Sketch Tools again, and I can select Circle. I'm going to lock it to the center of that part, and I'm going to give it an overall value of .5. I'm going to hit tab on my keyboard to lock that in. But you'll notice that it remembered the Radius that we used previously. While I'm in this command, before I place it, I can right-click and again select Diameter, and you'll notice it maintains the .5 that I entered, but changes it to a Diameter dimension. Left clicking places that, and I'm ready to finish the sketch.
With that circle created I can right-click and select Extrude from the Marking menu. I can select the circle that we created, and I'm going to select a Through All option for this extrusion. I'm going to select the check box in the Heads-Up Display to accept that, and we now have a hole that goes all the way through the part. The final element we're going to cover are the holes that surround the boss. Just to refresh, if I switch back to the base plate, you can see them surrounding the boss here and here, there is four total. We're going to switch back to our part, and we can being a new sketch on that face.
Now here we notice something happens that's a little different than we've seen before. While we get the projected edges, if I orbit a little bit, you'll see that this sketch actually cuts through the part a bit. In order to help with visibility while sketching, you have the ability to right-click in the graphics screen and select Slice Graphics. You can also hit F7 on your keyboard. What that does is temporarily slices the graphics away from the part so that you have better visibility of the sketch you're creating. Again, if I hit F7 on the keyboard, you'll notice it toggles back and forth.
It's a simple temporary visibility enhancement that allows you to see things that you're sketching on. Now, I'm going to rotate back to a Top view so we're looking normal at this view, and we can begin with our Rectangle command. Because we're in the sketch environment, we could bring up the Marking menu, but you'll notice that there is a Two Point Rectangle in our Marking menu. In this case, I don't want the rectangle that's defined by two corners. I'm going to go up to the Sketch tab, to the Draw panel, and find the Rectangle command. The Rectangle command has a split button, and if I select the dropdown option I have different types of rectangles that I can create.
In this case, I want a rectangle that's a Two Point, but one of those point is a center point, because of that I can select the center of this boss which was projected to our sketch. And as I start to drag you'll notice that my square or rectangle is locked into the center of that part. I'm going to use the Heads-Up Display to create dimensions on the fly. In this case, .716 is the Width of the rectangle. I'm going to hit tab on my keyboard to switch to the other dimension and enter .716 one more time.
I'm going to hit Enter on my keyboard to accept those values, and you'll notice the rectangle is created, it's locked to the center of the circle, and it's fully constrained, indicated by the purple geometry. I'm going to get out of my Rectangle command by hitting Escape on my keyboard, and I'm going to make one more change. Because this is construction geometry, I'm only creating this rectangle to locate the center of holes I'm going to create. I'm going to hold Shift down on my keyboard and select each of the outer edges of this rectangle, and with them selected right-click and change to Construction Geometry.
I'm going to hit Escape on my keyboard to make sure nothing is selected now, and I'm ready to finish this sketch. From the Marking menu I'm going to select Finish 2D Sketch, and I'm ready to create my holes now. From the Marking menu I can right-click and select Hole and in this dialog box you can see that I'm ready to select the center points. I can select the center point of these circles by clicking on the corners of the rectangle we just created, and I've now located each of those circles. In this case, the Diameter of the hole is .08, and I'm going to select the check mark to accept that value, and I've created my holes.
Now, because we're going to cover holes and other things around part modeling in future movies, we're going to stop here. At this point we've seen how to use circles and rectangles, and we've started to look at a little bit of part modeling as we prepare for that chapter.
- Navigating drawings with the View Cube and other navigation tools
- Sketching geometry
- Dimensioning parts
- Creating parameters
- Drawing circles, squares, and other shapes
- Creating extrusions
- Creating and managing constraints in assemblies
- Setting basic drawing dimensions