1. Autodesk Inventor Design Exercise: CO2 CAR Developed by Tim Varner – Synergis Technologies

2. Step 1. – Launch Autodesk Inventor by double (L) clicking the Inventor Icon on the Windows desktop. Step 2. – Double (L) click on New then select Metric as the units of measure.
Step 2

3. Step 3. – Double (L) click on Standard (mm). ipt
Step 3. – Double (L) click on Standard (mm).ipt. This opens a new part file with the metric units of measure.
Step 3

4. The Inventor User Interface
Command Panel
Standard
toolbar
Lists the commands that
are currently available in
Sketch or Model mode
Graphics Window
Displays your model
Model Browser
Message Bars
Records a history of
the operations you
have performed
Prompts the user
for input
(similar to the Command
Line in AutoCAD)

5. The Inventor User Interface
Dialog Boxes open when
Information needs to be
Input by the user

6. More about the User Interface
Left clicking on a down arrow
next to a command will open
a pull-down menu with additional
options
Slider bar – used for
scrolling up and down
Fly out tabs show the user the
command before selection

7. Using the Mouse A click with the right (R) mouse button
invokes “pop-up”
menus
The left (L) mouse
button selects
commands and objects
The mouse wheel
Is used to
Zoom and Pan
The Escape key
ends commands

8. Step 4. - From the Sketch panel, select the Line command with a single (L) click. Draw the rough sketch shown. Don’t worry about exact dimensions but try to make the sketch proportional to the one shown below.
Step 4
Step 4

9. Step 5. – From the Sketch panel, select the General Dimension command with a single (L) click. Move the cursor over the bottom (horizontal) line of the sketch and select it with a single (L) click. The line will change color, indicating that it has been selected. Move the cursor below the line and locate the dimension with a single (L) click.
Step 5

10. Step 6 Single (L) click on the dimension Opens the Edit Dimension
Step 6. – A single (L) click on the dimension you just placed will open the Edit Dimension dialog box, as shown. Type in the number 295 and press Enter - or single (L) click on the green check mark in the dialog box. Your sketch will change size to equal the dimension you typed. This process is called “parametric sketching”.
Step 6
Single (L) click on the
dimension
Opens the
Edit Dimension
dialog box

11. Step 7. – Zoom out so you can see the entire sketch by rolling the wheel of the mouse forward. Using the General Dimension command, repeat Step 6 to add the other dimensions as shown. NOTE: to change a dimension after it has been entered, move the cursor so that the dimension to be changed is highlighted and double (L) click on it to open the Edit Dimension dialog box. Type in the new dimension and press Enter - or (L) click on the green check mark.
Step 7

12. Step 8. – Move the cursor to any point in the drawing window and (R) click to open the pop-up menu. (L) click on Done. (R) click again to open the pop-up menu shown below and select Isometric View with a single (L) click. NOTE: To Pan press down and hold the mouse wheel while moving the mouse. (R) click anywhere in the drawing window and (L) click on Done.
Step 8

13. Step 9. – (L) click on the Sketch panel then select the Features option to open the Features panel.

14. Step 10 Profile Join Distance (thickness) of extrusion
Step 10. – Select the Extrude command with a single (L) click. This will open the Extrude dialog box. Take a minute to familiarize yourself with the Extrude dialog box. The Profile to be extruded has already been selected (shaded a different color). The Join button is depressed indicating that we will be adding material, and the Distance is set to 10mm and is highlighted. Type in the number 41 - then toggle the direction of extrusion buttons (indicated by the yellow rectangles with arrows). Notice how the sketch changes. (L) click on the toggle button with the arrow pointing to 7 o’clock and (L) click on OK.
Profile
Join
Distance (thickness) of extrusion
Direction of extrusion toggle buttons
Step 10

15. Step 11 Rotate button Free Rotate target
We now have extruded our sketch to create the blank for our car body. We still need to put a hole in the end of the blank for the CO2 cartridge. We must first rotate our blank so that we are viewing the end where the hole will be placed. Step 11. – Single (L) click on the Rotate button in the standard toolbar and a “free rotate target” will appear on the screen. Move the cursor inside the target, depress and hold the left mouse button while moving the mouse. Notice how the view rotates. Next, move the cursor just outside the target; depress and hold the left mouse button while moving the mouse. Notice how the view rotates.
Step 11
Rotate button
Free Rotate
target

16. Step 12. – Practice with the Free Rotate command until you feel comfortable. Now move the cursor inside the Free Rotate target and single (R) click to open the dialog box shown below. Select the Common View [SPACE] option. NOTE that pressing the Space Bar on the keyboard will toggle between the Free Rotate target and the Common View box.
Step 12

17. Step 13. – When the Common View command is selected, the Free Rotate target disappears and the Common View box is displayed. The green arrows indicate the direction from which your model will be viewed. As you move the cursor over the green arrows with the mouse they change color. When the arrows are highlighted and selected with a single (L) click, the view changes according to the direction the selected arrow was pointing. Practice using the Common View rotation command until you feel comfortable with it.
Step 13
Common View box

18. Step 14. – Using Free Rotate, the Common View box, or a combination of both; rotate the model so you are looking directly into the large end (as shown). (R) click in the drawing area to open the dialog box shown below and select Done – OR – press the Escape key to end the command. The Common View box will disappear and we are ready to start a new sketch for the hole where the CO2 cartridge will be placed.
Step 14

19. Step 15. – Zoom in with the mouse wheel to enlarge the view
Step 15. – Zoom in with the mouse wheel to enlarge the view. (R) click in the drawing window to open the dialog box shown below and (L) click on New Sketch. You will notice that the cursor changes, and when you move the cursor over the model, the outline of the model highlights in red. With the cursor over the model, (L) click to open a new sketch. Notice also that a grid has appeared indicating the new sketch plane, and the Features panel on the left side of the screen has been replaced by the Sketch panel.
Step 15

20. Step 16 Construction lines (Design Alternative)
Step 16. – From the Sketch panel, select the Point, Hole Center command. Your cursor turns to a yellow dot, and as you move the dot along the outline of the sketch, it will turn green at the end points and mid-points of the lines. Once the mid-points have been found, construction lines will project from the yellow dot as you move close to the center of the rectangular shape of the sketch. When you have located the center of the sketch, (L) click to place a tic mark. DESIGN ALTERNATIVE – you can also locate the tic mark for the hole center by placing it anywhere on the sketch then using the General Dimension command to parametrically move it to the center of the rectangle.
Step 16
Construction
lines
(Design Alternative)

21. Step 17. – Use the Free Rotate command or Common View box to rotate the view of the sketch as below. (L) click on the Sketch panel and (L) click on Features.
Step 17
Rotate button

22. Step 18 change dimensions
Step 18. – From the Features panel (L) click on the Hole command to open the Hole dialog box. Change the depth of the hole by double (L) clicking on the number and typing in 51mm; then change the diameter to 19mm (as shown). To make the hole, (L) click on OK.
change dimensions
Step 18

23. Step 19. – You can see the hole has been placed in our model and we are now ready to make the wing. (R) click anywhere on the drawing window and select New Sketch. (L) click on the face where you just made the hole.
Step 19

24. Step 20. – Notice that when New Sketch was selected in the previous step, a grid was placed over the drawing window and the panel bar on the left of the screen switched from Features back to Sketch. Using the Common View box, rotate the view of your model so that it looks like the one below. Select the Two Point Rectangle command with a (L) click and draw the two rectangles as shown below.
Step 20
Rotate button

25. Step 21. – Using the General Dimension command, dimension the left rectangle as shown below.

26. Step 22 Instead of typing 18 in the Edit Dimension
Step 22. – We will now constrain (dimension) the right rectangle so that it is the same as the left. (L) click on the left vertical line of the right rectangle then (L) click on the right vertical line of the sketch. Drag the dimension above the rectangle and (L) click again to open the Edit Dimension dialog box. This time, instead of typing in the number 18 – move your curser over the 18 dimension we placed on the left rectangle and (L) click. In the Edit Dimension : d15 dialog box, the number changes to read “d14”. Press the Enter key or (L) click on the green check mark. (R) click and select Done in the pop-up menu to close the command.
Step 22
Instead of typing 18 in
the Edit Dimension
dialog box, move your
curser over this dimension
and (L) click.
This number changes and
now reads d14

27. Step 23 Change this dimension and the other will automatically
Step 23. –Your drawing will look like the one below. The dimensions on both of the horizontal lines read “18”. But, we did something else that is very important – we have linked the second dimension (d15) to the first (d14). What this means is that if we come back later and change dimension (d14) - the other dimension (d15) will automatically change to the new value as well. We do not have to change both dimensions individually, only one.
Step 23
Change this dimension
and the other will
automatically
change also

28. Step 24 Double (L) click on this dimension and change the number to 13
Step 24. – Try it for yourself and see. Double (L) click on the left “18” dimension to open the Edit Dimension dialog box. Notice that the header of the dialog box actually reads Edit Dimension : d14. This tells us that this was the 14th dimension that we placed on our drawing. Type the number 13 in the dialog box and (L) click on the green check mark. BOTH dimensions will be changed to “13” and the rectangles have both been resized. Change the dimensions back to 18 and we will finish constraining the right rectangle.
Step 24
Double (L) click on
this dimension and
change the number
to 13

29. Step 25. – On the Sketch panel, scroll the slider bar down until you see Perpendicular - (L) click on the down arrow next to the Perpendicular tab.
Step 25
Slider bar

30. Step 26 Select this line first Then this line
Step 26. – (L) click on the Colinear constraint and select the top horizontal line of the left rectangle, then the top horizontal line of the right rectangle. The second line will move to line up with the first line (they will be colinear). Repeat this step for the bottom horizontal lines of the rectangles.
Step 26
Select this line first
Then this line

31. Step 27. – Your sketch will now look like this
Step 27. – Your sketch will now look like this. Note that using the Colinear constraint links the lines together so that if one is moved, the other moves along with it. DESIGN NOTE: this ability to place constraints on geometry in Inventor sketches is a powerful feature of solids modeling that is not found in CAD; but some thought must be given as to how you place constraints on your sketches. For more information, refer to “Constraints” in the Inventor Help file. (R) click in the drawing window and (L) click on Done.

32. Step 28. – (L) click on the Rotate button in the main tool bar
Step 28. – (L) click on the Rotate button in the main tool bar. Use the Common View box to rotate the sketch to the view shown below. (L) click on the Sketch panel and (L) click on Features.
Rotate button
Step 28

33. Step 29. – (L) click on Extrude to open the Extrude dialog box
Step 29. – (L) click on Extrude to open the Extrude dialog box. Notice that the Profile button is depressed, move the cursor over the first rectangle in our sketch and (L) click. It will highlight in a different color when selected. Now, select the other rectangle. Be sure the Cut button is depressed by (L) clicking on it.
Profile
Cut
Step 29

34. Step 30 Down arrow All Direction of Cut arrow
Step 30. – Under the Extents panel, (L) click on the down arrow and select All with a (L) click. Finish the cut operation by (L) clicking on OK. Notice that a red arrow appeared on the sketch to indicate the direction of the cut.
Down arrow
All
Step 30
Direction of Cut arrow

35. This cut creates the basic wing shape.

36. Step 31. – Select the Rotate button in the main toolbar and, using the Common View box, rotate the model to the view shown below. (R) click in the drawing window and (L) click on Done. Move the cursor until the correct part of the model highlights (see below). (R) click and select New Sketch.
Step 31
Rotate

37. Step 32. – (L) click on the Line command and draw a line from point 1 to 2, and another line from point 3 to 4 (below). (L) click on the Sketch panel then (L) click on Features.
Step 32 1 3 2 4

38. Step 33 Extents - All Profile Direction Cut
Step 33. – (L) click on Extrude. Check to be sure the Profile button is depressed and select the highlighted portions of our sketch by (L) clicking on them. Next select the Cut button with a (L) click. Under Extents, set the distance to All. (L) click on the direction button with the arrow pointing to 1 o'clock. Finish the cut by (L) clicking on OK.
Extents - All
Profile
Direction
Cut
Step 33

39. Step 34. – Move the curser over the body of the car, (R) click to select the highlighted surface (below) and (L) click on New Sketch.
Step 34

40. Step 35. – Zoom out by turning the mouse wheel and pan the car to the top of the drawing window by pressing and holding the mouse wheel while moving the mouse. When your drawing window looks like the view below, (L) click on the Center Point Circle command in the Sketch panel.
Step 35

41. Step 36 Circle center point
Step 36. – Draw a large circle as shown below. Locate the center point first with a (L) click then move the mouse to drag out the circle. (L) click again to complete the circle. Note: the diameter of the circle should be about 1700mm.
Step 36
Circle center point

42. Step 37 Step 37 Tangent points Tangent constraint
Step 37. – Zoom back in to see if the circle gives a graceful curve to the body of the car. You can adjust the size and location of the circle by (L) clicking and holding down the (L) mouse button on the center point of the circle while dragging it to a new location. It may also help if you apply a Tangent constraint to the circle and the straight lines on the body of the car. (L) click on the down arrow next to the Perpendicular constraint in the Sketch panel, and (L) click on Tangent. (L) click on the circle, then (L) click on the line you want the circle tangent to.
Step 37
Step 37
Tangent points
Tangent constraint
Tangent constraint

43. Step 38. – In the Sketch panel, select the Trim command with a (L) click. Move the curser over the line to be trimmed (it will turn dashed when selected). Trim the line by (L) clicking on the dashed line.
Step 38

44. Step 39. – (L) click on the Sketch panel then (L) click on Features.

45. Step 40. – Rotate the model with the Common View box until it appears as below. (L) click on Extrude. Move the curser to highlight the profile in blue (below) and (L) click. (L) click on the Cut button. Select All in the Extents box. Notice that a red arrow appears indicating the direction of the cut. (L) click on OK.
All
Profile
Cut
Step 40

46. Step 41 + Sign Sketch 1 Edit Sketch
Step 41. – Next we want to make the holes for the axles, and the cut-outs for the wheels. Use the Common View box to rotate the model as shown below. We will now use the Model browser to select our original sketch. (L) click the + sign beside Extrusion 1 in the Model browser. (R) click on Sketch 1 then (L) click on Edit Sketch. This will allow us to go back and work on our original sketch without having to redraw it. Note that the original sketch, with dimensions, will highlight.
Step 41
+ Sign
Sketch 1
Edit Sketch

47. Step 42. – Use the Common View box to rotate the model to the view shown below. In the Sketch panel, (L) click on Center Point Circle and draw 2 small circles on the sketch as shown.
Step 42

48. Step 43. – Draw two more Center Point Circles as shown below.

49. Step 44. – Use the General Dimension command in the Sketch panel to dimension the circles as shown below.
Step 44

50. Step 45. – Zoom and Pan in on the rear wheel by scrolling the wheel on the mouse. Use the General Dimension command to place the dimensions (shown) that locate the center of the rear axel and wheel.
Step 45

51. Step Use the General Dimension command to place the dimensions (shown) to locate the front axel and wheel.
Step 46

52. Step 47. – (R) click in the drawing window and (L) click on Done
Step 47. – (R) click in the drawing window and (L) click on Done. (R) click on Sketch 1 in the Model browser and (L) click on Finish Sketch.
Step 47

53. Step Use the Common View box to rotate the model to the view shown below. (R) click on Sketch 1 in the Model browser then (L) click on Share Sketch. Notice in the Model browser, Sketch 1 will now have the hand symbol under it, indicating that it is shared; and the Sketch panel will change to the Features panel.
Step 48

54. Step 49 Step 49 Be careful to select ONLY the small holes
Step 49. – Zoom in slightly so your drawing area looks like it does below. (L) click on the Extrude command in the Features toolbar. For the Profile, move the curser carefully over the small hole for the front axle until just the hole is highlighted and select it by (L) clicking on it. Next, select the other small hole for the rear axle. Both of the small axle holes will now be highlighted indicating that they have been selected. In the Extrude dialog box, (L) click on the Cut button and set the Extents distance to All. Notice the red arrow indicating the direction of the cut. Finish the cut by (L) clicking on OK.
Be careful to select ONLY
the small holes
Axel holes
highlighted
Step 49
Direction of
Cut arrow
Step 49
Direction of Cut arrow

55. Step 50. – (L) click on the Extrude command again and carefully select the circle for the front wheel. It will highlight when selected. (L) click on the Cut button. Change the depth under Extents to 2 and (L) click on the direction button with the arrow pointing to 7 o’clock. (L) click on OK.
Step 50

56. Step 51. – Repeat the procedure in Step 50 but, this time, select the rear wheel and set the depth of cut to 7.5. (L) click on OK to complete the cut.
Step 51

57. Step 52. – Using the Free Rotate command or Common View box, rotate the model so it looks like the picture below. Move the curser over the side of the car and, when it highlights, (R) click to open the screen menu. (L) click on New Sketch.
Step 52

58. Step 53 Center points for circles
Step 53. – From the Sketch panel, (L) click on Center Point Circle and draw 2 circles using the center points of the front and rear axle holes as the center points for the circles. Don’t worry about the size of the circles you draw.
Step 53
Center points
for circles

59. Step 54 Dimension for front wheel Dimension for rear wheel
Step 54. – From the Sketch panel, (L) click on the General Dimension command and select the rear wheel circle. (L) click on the dimension again to open the Edit Dimension dialog box. Click on the 40 dimension (highlighted in red below). Click on the green check mark. Next dimension the front wheel circle the same way, (L) clicking on the dimension that reads This will make the dimensions of both rear wheels the same and both front wheels the same.
Step 54
Dimension for
front wheel
Dimension for
rear wheel

60. Step 55. – (R) click anywhere in the drawing window and (L) click on Done. After dimensioning the wheels, (R) click on Sketch 1 in the Model browser and uncheck the Visibility option. This will hide all of the dimensions that are on Sketch 1.
Step 55

61. Step 56. – (L) Click on the Sketch panel then (L) click on Features
Step 56. – (L) Click on the Sketch panel then (L) click on Features. (L) click on Extrude. For the Profile, (L) click on the rear wheel. (L) click on the Cut option. Under Extents, set the depth of cut to 7.5 and check the direction of cut so that you are cutting into the car body. (L) click on OK.
Step 56

62. Step 57. – In the Model browser, (L) click on the + sign next to Extrusion 8, (R) click on Sketch 6 to open the screen menu and (L) click on Share Sketch.
Step 57

63. Step 58. - (L) click on Extrude in the Features toolbar
Step (L) click on Extrude in the Features toolbar. For the Profile, select the front wheel circle with a (L) click. (L) click on the Cut button and under Extents, set the depth of cut to 2. Check to make sure the correct direction of cut button is depressed. (L) click on OK.
Step 58

64. Step 59. – In the Model browser, (R) click on Sketch 6 under Extrusion 7, and uncheck the Visibility option to hide the dimensions.
Step 59

65. Step 60. – We have now completed the basic shape of our car model and are ready to add some finishing touches with the Fillet command. In the Features panel, (L) click on Fillet. In the Fillet dialog box, set the Radius to 36 and press the Enter key. Move the cursor until the edge (see below) highlights and (L) click. Notice that when an edge has been selected, a preview of the filet will appear on the model. If the fillet radius looks too big, simply reenter a smaller number in the Fillet dialog box. When the fillet is the way you want it, (L) click on OK.
Step 60
Highlighted edge

66. Step 61. – On the screen shot below, notice that we have added more fillets to the wing using the Fillet command in the Features panel. You will have to use the Free Rotate command, and Zoom and Pan often while placing fillets in order to be able to see the corner where you want to place a fillet. Occasionally, you will try to add a fillet that has too large of a radius (blue highlighted corner below). When this happens, a dialog box opens to show you what went wrong and how to correct it. To resize a fillet (L) click on the Edit box to reenter the Fillet command, and type in a smaller size radius.
2mm was entered for this fillet radius. This was too large and had to be made smaller
Step 61
Problem warning
and solution

67. Step 62. – Continue using the Fillet command to round the corners
Step 62. – Continue using the Fillet command to round the corners. Experiment with different sizes of fillets until your model looks the way you want.
Step 62

68. Step 63. – Editing Features
Step 63. – Editing Features. If you don’t like the way a particular fillet (or other feature) looks, it can be easily changed. Move your curser up an down in the Model browser. Notice that as you move from one feature to another, the feature will highlight on your model. When you get to the fillet or feature you want to change, (R) click on it in the Model browser then (L) click on Edit Feature. In this example, the Fillet command dialog box will open, enter a different fillet radius and (L) click on OK.
Step 63
Features highlight as you move the curser from item to item in the Model browser. (R) click on the feature then (L) click on Edit Feature.
Fillet 11 feature
Is highlighted

69. Step 64. – Our model is now finished
Step 64. – Our model is now finished. Save your work by (L) clicking on File in the pull down menu bar at the top of the screen. (L) click on Save Copy As.
Step 64

70. Step 65. – In the Save In field, enter the drive or folder location where you want to save your model. Under File name, type in the name you want to save your file as. (L) click on Save.
Step 65

71. Step 66. – In order for our model to be exported to the Denford CNC Router or Mill, we also need to save a copy of our Inventor model as an STL file type (which stands for Stereo Lithography). The STL file format is commonly used by Computer Aided Manufacturing (CAM) software programs that run rapid prototyping machines and CNC machine tools. Saving your Inventor model in the STL format allows it to be exported directly into the Denford MiniCAM software. Enter the File name in the box. (L) click on the down arrow and (L) click on the STL file type. (L) click on Save.
Step 66
Down arrow