In the last lesson you learned that the first sketch of a part has a node on the origin, and you can use the node to permanently constrain the location of geometry. You also learned that there are two types of snaps, soft snaps and hard snaps. The green snap dot makes a hard snap that is permanent, and the yellow snap dot makes a soft snap that is unconstrained.
Now we’re going to look at some of the other methods of drawing geometry using soft and hard snaps as well as permanent constraints. Click the Line command. If you look in the status bar you can see that it says to select the start of the line, and it also says you can drag off the endpoint for tangent arc. We’ll talk about the tangent arc later in the course. For now I want you to select a point on the graphics area, and then select another point to draw a diagonal line.
If you move your pointer around on the graphics area you can see dotted lines that extend from existing geometry to the yellow snap dot. These locations are called inferred points, and they define soft snap locations. You can also move your pointer to show automatic constraints. This is the perpendicular constraint. If you select this point the new line will be perpendicularly constrained to the first line. You know that the line will be perpendicularly constrained to the first line because the first line has the perpendicular constraint symbol next to it. Move your pointer until you can see an inferred location and the perpendicular constraints, and then click your left mouse button. Now type the escape key to exit line mode.
The second line is constrained to the first line with the perpendicular constraint, but the end of the line was constrained with an inferred point. You can see how the line was constrained by dragging the node on the end of the line. The lines stay perpendicularly constrained, but the location of the node on the end of the line can change. So inferred points are soft snap constraints.
Now place your pointer over the line command in the ribbon. At the top left of the tool tip you can see the name of the command, and to the right of the name is the letter L in parentheses. This indicates that the letter L is a command alias for the Line command. Move your pointer into the graphics area, and then type the L key. Now that you’re in Line mode, select the end of the second line. The green snap dot is visible, so the lines will be permanently constrained together.
By default Automatic Constraints are not added between previously drawn geometry and new geometry. So you have to scrub the line you want to add a constraint to. All you really need to do is pass your pointer over the line. Now you can see that a perpendicular constraint will be added to the lines.
I prefer not having to scrub lines to add automatic constants, so let’s change a setting that will improve this workflow. Type the escape key to exit the line command, and then click the down arrow on the Constrain panel. Now select Constraint Inference Scope. The top option just adds automatic constraints within the current command. So we evoked the Line command and only the geometry created by that session of using the command will have automatic constraints. This can be helpful if you find that unwanted constraints are being added to your sketch geometry, but if you’re aware of how automatic constraints are added, you can prevent this problem yourself. It’s faster for most people to add automatic constraints to all the geometry on the sketch, so select this option. You can also select the geometry you want to apply automatic constraints to, but it’s just as fast to scrub the geometry. So this option is rarely used. With a little practice you’ll see that the All Geometry option is the best one to use, and we’ll use this setting throughout the rest of the course.
Click OK, and then type the L key to evoke the Line command. Now use the green snap dot to select the end of the line, and as you can see the perpendicular constraint will be added if I click my left mouse button. When you’re using automatic constraints you can control which line is used for the constraint. Here the perpendicular constraint will be added to the second line in the sketch. If you want to choose different base geometry you can scrub the geometry you want to use. For example, if I wanted the third line to be parallel to the first line I could scrub the first line with the pointer, and then draw the line. Notice that the parallel constraint is now on the first line, and the pointer has the parallel constraint next to it.
Another method of constraining geometry on a sketch is to use dimensions. If you place your pointer over the general dimension command you can see that typing the D key can evoke the command. Click the command, or type the D key, and then place your pointer over the circle. The diameter symbol is next to the pointer, which indicates that you’re creating a diametral dimension. Select the circle, and then select a point on the graphics area. When you do, a Dimension box appears. Enter .094 of an inch, and then click the green check, or type the enter key to enter the dimension.
The first dimension scales the geometry on the sketch, and to zoom into the circle, place your pointer over the circle and roll the wheel on your mouse backward. Whenever you create a sketch you need to be sure to fully constrain it, and the best way to tell if the sketch is fully constrained is to look in the status bar. As you can see 6 dimensions are needed to fully constrain the sketch.
Also notice that the color of the circle has changed to blue. This indicates that the circle is adequately constrained. You’ll learn the difference between adequately constrained geometry and fully constrained geometry later in the course. For now notice that the lines are black, which means they are not adequately constrained.
You saw earlier that you can delete geometry by selecting it and then typing the delete key. You can also drag a window around geometry to select it. When you drag the window to the left, the geometry inside the window and the geometry the window crosses over is selected. When you drag the window the right, only the geometry inside the window is selected. Use any method you prefer to highlight the lines, and then type the delete key to delete them.
Now if you look in the status bar the sketch is fully constrained. In the next lesson you’ll use this sketch to create a pin.