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Autodesk Inventor 2016 Training Lesson - Sketches vs. Profiles

Autodesk Developer Network

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Earlier we brought up a very important question. What is the difference between a profile and a sketch? And in this lesson you’ll learn the difference. You’ll also learn how to use the Trim command. Start by opening a new standard part.

Before we talk about the differences between sketches and profiles I want to talk about the first sketch of a part. When we constructed the pin we created the sketch on the XY plane, and I mentioned that it saves time and speeds up your work if you always use the same plane to create your first sketch. Now we’re going to change an application option that will automatically create the sketch on the XY plane.

Click the Tools tab, and then open the Application Options. Now select the Part tab. No New Sketch is active by default, which means you have to select a plane to create the first sketch. We’re always going to create the first sketch on the XY plane, so select this option. Now click OK. The changes won’t take place until the next time you open a new file. So close this file, and then open a new standard part file. As you can see the part opens in the sketch environment, and the sketch is on the XY plane.

Now we’re ready to talk about the differences between sketches and profiles. Start by drawing 4 horizontal lines. The first line will snap to a horizontal position and you’ll see the horizontal constraint just below your pointer. Click to accept the position, and type the escape key to end Line mode. Now draw the second line. You can use the L key on your keyboard to evoke the command. The horizontal constraint will be added to the line, but if you want it to be parallel to the first line pass your pointer over the line. Now the lines will be parallel. As you saw earlier, Inventor is visually asking if you want to make the second line parallel to the first line. Click to accept the constraint and end position of the line. Type the escape key and then type the L key to start a new line and continue drawing lines until you have 4 horizontal lines.

Now draw 4 vertical lines. The first line is automatically constrained with the vertical constraint. While you draw the vertical lines, perpendicular and vertical constraints will be added.

Now we’re going to use the Trim command to trim all the lines except the rectangles in the corners. Use a mouse gesture to launch the Trim command, and then move your pointer over a line you want to trim. The section of line turns into a dashed line, which is the part that will be trimmed. Click your left mouse button, and continue trimming all the lines until you have 4 rectangles. When you’re finished, you should have 4 rectangles in the graphics area.

Now change the view to the isometric view. Finish the sketch, and then open the Extrude command. Now I can tell you about the difference between sketches and profiles. Profiles are used to create geometry. When you’re creating 3-dimensional geometry the profile has to be a closed loop. There are four closed loops in the sketch, but you can only call a closed loop a profile if it is used to create geometry.

The reason I’m making this distinction is to let you know that you can draw anything you want on a sketch like construction geometry and closed loops. Closed loops can be used to generate 3-dimensional geometry, and you don’t have to use all the closed loops on the sketch.

The Extrude command is active, but as you can see, none of the rectangles have been selected. That’s because Inventor gives you the option of selecting the profile or profiles you want to use. When this happens the Extrude command is automatically set to profile selection mode. So you have to select a profile. Click inside the upper left rectangle and the lower right, and then use the mouse gesture that applies the command. As expected, two rectangular solid bodies were created by the operation. Now edit the Extrusion. Right click Extrusion-1, and then select Edit Feature.

Once a feature has been created from a sketch profile, the profile selection mode does not automatically turn on. So you have to manually turn it on. To do this, click the Profile, button. Now select the upper right rectangle. Once you’ve done that, apply the operation.

The difference between sketches and profiles is sketches are used to draw and constrain profiles, and profiles are used to generate 3D geometry. The geometry on a sketch can consist of profiles and non-profile geometry like construction geometry.