Creating general annotations

Any referenced datasets can be downloaded from "Module downloads" in the module overview.

Creating general annotations - Exercise

  1. Open the Gear_Housing_Annotate.ipt part file from your working folder. 
  2. Activate the Annotate tab from the Inventor ribbon. 
  3. Expand Extrusion 4 and right-click on Sketch1. Select Visibility from the drop-down menu.

  4. Click on the 11.300 dimension. Right-click and select Promote from the drop-down menu:

  5. Right-click on Sketch1 in the model browser and select Visibility to turn it off. 
  6. From the Annotate tab>General Annotations panel – select Dimension. 
  7. Select the two faces from the model as shown below:

  8. Hit the SPACEBAR on your keyboard to move the dimension to the same plane as the 11.300 dimension. 
  9. Left-click to confirm placement:

  10. Click on the Edit Dimension button.
  11. Activate the Precision and Tolerance tab. 
  12. Change the Primary Unit and Primary Tolerance values to 3.123.

  13. Click OK. 
  14. Click the Green Checkmark to confirm. 
  15. From the Annotate tab>General Annotations panel – select Hole/Thread Note. 
  16. Choose the bored hole shown below and left-click to confirm placement:

  17. Click the Edit Hole Note button.
  18. Click the Precision and Tolerance button.
  19. Change the Unit Precision for Primary diameter and depth to 3.123.  
  20. Under Tolerances, Check the box next to Upper. 
  21. Change the Method to Limits - Stacked. 
  22. Type 0.020 in the box for Upper. 
  23. Change the Precision value to 3.123 using the drop-down menu.

  24. Click OK. 
  25. Click the Green Checkmark to confirm. 
  26. From the Annotate tab>Notes panel – select Leader Text. 
  27. Click the edge of the housing as shown below. 
  28. Click in the graphics window to confirm leader plane placement. 
  29. Type BREAK ALL EDGES in the text box. 
  30. Click OK to confirm.



  31. From the Annotate tab>Notes panel – select General Note. 
  32. Click in the upper left quadrant when the screen turns blue. 
  33. Type UNLESS OTHERWISE SPECIFIED ALL DIMENSIONS BASIC in the text box. 
  34. Click OK to confirm.

  35. From the Annotate tab>Notes panel – select General Profile Note. 
  36. Click in the upper left quadrant when the screen turns blue. 
  37. Right-click on the <<$GENERAL_PROFILE_TOL>> text and select Edit Profile Tolerance.

  38. Change the Tolerance value to 0.020. 
  39. Click OK twice to confirm. 
  40. Save and Close the part file.