Create a 2D sketch in Inventor

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All part models created in Autodesk Inventor start with sketches,

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which you create by drawing geometric elements, such as points, lines, shapes, and arcs.

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The sketch becomes the basis for sketched features,

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such as extrusions, revolutions, lofts, coils, or sweeps, which add volume to the sketched part.

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On the Home tab, open the Projects menu and click Settings.

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In the Projects dialog, click Browse, and then navigate to where you saved the project files for this tutorial.

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Select Steering Knuckle.ipj, and then click Open.

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In the Projects dialog, click Done.

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Then, in the Quick Access Toolbar, click New.

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This opens the Create New File dialog.

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Select Standard.ipt.

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This template lets you create a 2D or 3D object.

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Click Create.

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Once the template is applied, the graphics window opens.

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Now you can create a sketch.

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To do so, right-click in the modeling window.

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From the marking menu, select New Sketch.

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This opens the sketch environment, which includes sketching tools and commands,

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and the graphics window, where you work directly on your sketch.

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It also includes the browser, which shows a sketch icon as soon as you create a sketch.

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In the graphics window, set the X-Z plane as the sketch plane.

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Using the ViewCube, use the rotation arrow to rotate the view until the word Top is horizontally displayed.

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Right-click to open the marking menu again, and select Two Point Rectangle.

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In the graphics window, place the first point at the origin point to start the rectangle, and then move your cursor to the upper right.

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In the dynamic dimensioning boxes, enter 0.12 in for the horizontal value.

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Press TAB, enter 0.5 in for the vertical value, and then press ENTER to create the rectangle.

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Right-click, and from the marking menu, select OK to close the rectangle command.

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Open the marking menu again, and this time, click Create Line.

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Start the line by clicking the top right corner of the rectangle.

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Move your cursor down and to the right.

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In the dynamic dimension box, enter “ArmLength = .7 in” and press TAB.

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This creates a parameter named ArmLength that can be referenced in other dimensions.

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For the angular dimension, enter “ArmAngle = 180-52”.

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This calculates the value for the ArmAngle parameter as 128-degrees.

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Click to complete the line.

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Click on the endpoint of the previous line and drag to create an arc off to the lower left of the last point.

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Then, click the bottom right corner of the rectangle to add a final line segment.

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Right-click, and from the marking menu, select OK to close the line command.

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A critical aspect of sketching is making sure that your geometry is stable.

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Inventor automatically applies some constraints to sketch geometry as you work, and you can also add geometric constraints manually.

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Press and hold CTRL as you right-click the graphics window to open the constraint marking menu.

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Select Tangent.

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A Tangent constraint positions faces, planes, cylinders, spheres, cones, and ruled splines tangent to one another.

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Select the arc and line segment to add a tangent constraint, and then press ESC.

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Open the marking menu again and select General Dimension.

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Select the arc, and then click to place the dimension.

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In the dimension box, type 0.13 in.

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Press ENTER.

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You have now created a 2D sketch using rectangles, lines, and arcs.

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Right-click, and from the marking menu, select Finish 2D Sketch.