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In this section, we create a work plane on a curved surface to provide a flat area for a 2D sketch. We use projected geometry to assist in accurately placing hole location geometry.
- Right-click the XY Plane in the Origin folder, and check the Visibility option to turn it on.
NoteAs you become a more advanced user, you might prefer to control globally the visibility of Work Geometry, Sketches, and more by using an Object Visibility filter in the View tab. If you switch the visibility off using these controls, right-click a work plane, other work feature, or sketch and note that the visibility is enabled but the feature is off. To enable it, switch the visibility to on in the Object Visibility area.
- Select Tangent to Surface and Parallel to Plane from the Plane drop-down menu. Select the edge of the XY Plane and the tangent face of the curved surface to create the work plane.
- Start a new sketch on the work plane.
- Start the Project Geometry command. Select the two edges of the mounting tab as shown in the following image to project them to the sketch plane. Repeat this process for the other tab before leaving the Project Geometry command.
- Start the Line command, and draw a line from the midpoint of one line to the midpoint of the other line. Repeat this process for other tab.
- Place a Point, Center Point at the midpoint of each line to locate the hole in the middle of the mounting tab. These points also allow the Hole command to detect them for hole placement.
- Finish the sketch.
- Start the Hole command. The Placement option defaults to From Sketch because Autodesk Inventor LT detects that an unconsumed sketch is present. Autodesk Inventor LT detects the hole centers and selects them for the hole location.
TipAutodesk Inventor LT
automatically selects hole locations from sketch points if no other unconsumed sketch exists.
- Select the Tapped Hole option. Set the Thread Type to ANSI Metric M Profile, the Size to 6, and the Designation to M6x1.
- Select To in the Termination option to terminate the tapped holes on the center holes.
- Select an inside face of one of the existing holes to satisfy the termination selection. Make sure the check box in the dialog box is selected as shown here, or the operation fails. Click the OK button to create the holes and exit the Hole command.
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