Autodesk Inventor - Basics Tutorial Exercise 1 Launch Inventor Professional 2015 1. Start a New part. Depending on how Inventor was installed, using this icon may get you an Inch or Metric file. To be sure, we ll use the New file button in screen: the top left corner of the Select a Standard (mm) ipt file and click Create 2. Start a new sketch and pick the XY plane 3. Click the 2 point Rectangle tool on the sketch toolbar. Click a point close to the origin, then move the cursor to create a rectangle that is approximately 75 x 50. You may have to zoom out, using the mouse s scroll wheel. Pressing the wheel allows you to pan the view. *You may notice that the zoom function is the reverse of AutoCad. To switch this so it is the same go to the top left corner big I button and go to options, then display tap, zoom behavior and click reverse direction box. 4. Click the General Dimension tool and select the top horizontal line, then click a pint above the line to place the dimension. Enter 75 in the Edit dimension dialogue box, and then click the check mark.
5. Click the vertical line and then click a point to the right to place the dimension. 6. Click the Finish sketch icon. The view will change to isometric, and the 3D Model tab will automatically be selected. 7. Click the Extrude tool. A dialogue box will appear and it will automatically choose your sketch to extrude. If there were multiple, you would choose. Enter 8 for the extrusion distance, then click the direction 2 button. (The arrow in the preview should point away from you) Click OK to create the extruded feature.
8. In the browser to the left of the model space, you should now see a feature that says Extrusion1. Click the + button and you will see that the sketch is now consumed by the extrusion. The sketch defines the extruded shape. Go back to the Sketch tab. 9. Click the Start 2D Sketch tool and select the front face of the extruded box. We can now draw on this face. 10. Click the Circle tool. Click a point in about the center of the face. Move the cursor to create a circle with a diameter of approximately 30. 11. Click General Dimension tool and select the circle. Place the dimension above and to the right of the circle, and enter a value of 35.
12. Using the General Dimension tool again, click the left vertical line, and then the center of the circle. Place the dimension above the part. In the dimension dialogue box, enter d0/2 and click the check mark. Doing this will lock the distance that the circle is away from the edge, exactly in the middle of the part. d0 refers to the very first dimension we gave, which was the length of the rectangle, and we are telling our new dimension to divide whatever that number is by 2. 13. Click the top horizontal line and the center of the circle and click a point to the right of the part to place the dimension. Enter d1/2 and click the check mark. This will center the circle along the rectangles height. (d1) 14. Click the Finish Sketch icon. 15. In the 3D Model tab, click Extrude tool. Click the inside of the circle to select it as the profile to extrude, and enter 22 for the extrusion distance. Click OK to create the feature. Make sure the extrusion is coming out of the first object. 16. Create a New Sketch on the front face of the extruded cylinder.
17. Click the Point tool. Move the cursor over the center of the circle. The cursor should snap to the center of the circle and click that point. This will create a coincident constraint for the hole you are about to create. 18. Finish Sketch 19. Select the Hole Feature icon in the 3D Model tab. Enter 25 for the hole diameter and select Through All from the termination list. Click OK to create the hole feature. 20. Create a Sketch on the front face of the rectangle box again. 21. Click the Point tool. Move the cursor over the edge of the circle. Don t click yet!! Move the cursor to the right to display a dashed line (object tracking), then click a point to create the first hole center. 22. Drag the cursor to the left, ensuring there is still a dashed line, and click a point to create the second hole center. 23. Create a Dimension for both holes so that they are 27.5 from the center.
24. Finish the sketch. 25. Select the Hole Feature icon. Enter 8.1 for the diameter and select Through All. Click OK. 26. Click the Fillet icon. Enter 10 for the radius and select all four corners of the base. Click OK to create the fillet feature. *Rotate the object if you need by turning the view cube or by holding shift and panning 27. Under the dropdown menu on the Fillet icon, select Chamfer. Choose the Distance and Angle option. Click the end of the cylinder and the inside edge. Enter 5 as the distance and 30 as the angle. Click OK to finish.
28. The model you have created is a parametric model. This means that all the dimensions are stored as parameters, and as they are changed, the model will update to accommodate these changes. Click on the Manage tab, and then the Parameters icon. A list of the parameters for this model appears: *notice how parameters d5 and d6 use the equation that you entered. If d0 changes, then so will d5* 29. Click on the parameter name d0, and change it to length. Note that his change also occurs in the equation for d5.
30. Change the equation for length (or d0) to 100. Click Done. Notice that the model automatically adjusts itself to the new length and that the circle is still centered. 31. These changes can also be made by adjusting the original sketches by finding them in the browser. 32. Lean back and marvel at the awesomeness of solid modelling!