Create a 2D sheet metal sketch in Inventor

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In Inventor, a sheet metal part starts out as a flat piece of metal with a consistent thickness.

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In this tutorial, you set sheet metal defaults and create a 2D sketch for sheet metal design.

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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 Assembly, Cartridge Body.ipj, and then click Open.

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In the Projects dialog, click Done.

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Click New.

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In the Create New File dialog, expand the Templates folder and select Metric.

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Under Part—Create 2D and 3D objects, select the template Sheet Metal (mm).ipt.

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This template creates a 3D object fabricated from sheet materialmetal.

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Click Create.

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The Sheet Metal environment opens.

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First, configure the Sheet Metal Rule and any options or parameters for the active model state.

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From the ribbon, Sheet Metal tab, Setup panel, select Sheet Metal Defaults.

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The Sheet Metal Defaults dialog displays.

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Here, you can choose which sheet metal rule to apply, the material for the part, the unfold rule, and the thickness of the material.

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Edit the thickness of the sheet metal you will be working with.

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First, ensure that the Use Thickness from Rule option is deselected.

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Then, in the Thickness field, enter a value such as 1.17 mm.

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Expand the Material drop-down.

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Here, all materials in the active library display.

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If the desired material is in another library, you can browse to that library and select the material.

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If the necessary material library is not in the project file, it is recommended that you add it to the project, so it is readily accessible.

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For this example, from the list, choose Stainless Steel.

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Click OK.

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Now, use sketch commands to create a profile for a base face.

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From the ribbon, Sheet Metal tab, Sketch panel, select Start 2D Sketch.

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In the graphics window, pick the XY plane.

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Then, right-click to open the marking menu.

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Select the Create Line command.

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Start the line at the origin, and enter a length of 62.5 mm.

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Pick an endpoint for the line to the right of the origin, making the line horizontal.

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Continue the line straight upward, setting the length to 18.5 mm and clicking at a point perpendicular to the first line.

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Add another endpoint to the left of the last point, then add a point up, perpendicular to the last point.

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Moving to the left, add another point in line with the origin, and then a final point back at the origin.

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To ensure that the dimensions are precise, from the ribbon, Constrain panel, select Dimension.

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Then, in the graphics window, select the line representing the height.

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A dimension displays.

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Pick to place the dimension.

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An Edit Dimension field opens.

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Here, enter a value of 32.5 mm.

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Next, select the top line segment, place the dimension, and enter a value of 46.5 mm.

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To complete the profile outline, from the Sketch tab, Exit panel, click Finish.

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When working with sheet metal parts in Inventor, you can configure rules and begin a part using sketch commands.