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Autodesk Inventor 2016 Training Lesson - The Heads-Up Display

Autodesk Developer Network

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Now you're going to learn about the Heads Up Display. Click the Line command. The Heads Up Display is the boxes shown just to the right of your pointer.

There are two modes for the display, and currently it's in Point Input mode, which means you need to select a point on the graphics area.

You can click you're left mouse button to select a point, but since I'm showing you how the heads up display works, we'll use it to select the first point of the line. Type the tab key, and the X coordinate highlights. Type zero, and to enter the Y coordinate type the tab key.

The yellow snap dot is locked on the Y axis, and the heads up display is waiting for input for the Y coordinate. Enter zero, and then type the enter key. Now the line starts on the origin and the heads up display is in dimension input mode.

In this mode you can enter a length and an angle. We're going to draw an equilateral triangle so enter 5 for the length. Type the tab key and then enter 60-degrees for the angle. Type the enter key, and the line has been drawn. Now enter 5 and type the tab key.

The heads up display uses relative polar coordinates instead of absolute coordinates so you need to be careful about using the command. We're drawing a line downward about like this and in absolute polar coordinates the angle would be minus 60 degrees, but the heads up display draws lines relative to the last line drawn. So the angle you see on your screen is the angle between the new line and the last line drawn.

I also want you to notice that when the first line was draw a construction line was drawn along the X axis. It's the dashed line. The first line was drawn relative to the construction line, so the angle between the construction line and the line is 60 degrees, which is defined by the dimension.

Now let's finish the second line. Enter 60-degrees in the cell, and then type the enter key. I'll talk about closed profiles later in the course, but for now I'll just say that you can click the end of the first line to create a closed profile. Another way to do it is to right click and select Close, and you can enter 5 inches and 60 degrees in the heads up display.

The close command works pretty well, but to assure that the end of the new line is constrained to the end of the first line, make sure the green snap dot is visible and then click the end of the line.

Now I'll show you how the heads up display can cause problems. Click the Fillet command. Set the radius to 1-inch, and then select the lines near the corners to create the fillets. Type the escape key, and now if you place your pointer on the X axis you can see that the last line was not trimmed to the fillet. That's because Inventor trimmed the construction line instead of the normal line. As a result, you won't be able to apply feature commands to the profile.

Let's finish the sketch and I'll show you what I'm talking about. Click the Finish Sketch command. As you can see the line extends beyond the closed profile.

Now click the Extrude command. Feature commands like the Extrude command need a closed profile. It can't have lines that extend beyond the profile and it has to be fully closed. So you can't select this profile to create the feature.

So let's fix it. Cancel the command and then double click Sketch-1 to edit it. Now trim the line using the Trim command. Click the command and then place your pointer over the end of the line. Click your left mouse button, and the line has been trimmed to the fillet.

Now finish the sketch, and then open the Extrude command. Now you can see how the Extrude command is supposed to work. Click OK, and the feature has been created.

Now click the Undo command until the first line is the only line on the sketch, and then set the view normal to the sketch using the Look At command. Click the command and then select the sketch.

The heads up display is just one way of drawing this line, and as you saw it creates a construction line which can cause trouble later on. Now that you know this you can use the heads up display, but be aware of this potential problem.

Throughout the course I'm going to manually draw lines and other sketch geometry so that you can see the details of the geometry and to assure that the geometry is constrained correctly. After you've mastered sketch geometry and sketch constraints you might want to try using the heads up display again. Just be sure to check the geometry to assure that it's constrained the way it's constrained in the course. Before you proceed to the next lesson, delete the lines. Click the line and then type the delete key.