Monday, November 18, 2013

Creating hole on a curve surface (Autodesk Inventor 2013)

 

Creating hole on a curve surface

Serial No.148

Creating hole on a curve surface (Autodesk Inventor 2013)

Autodesk Inventor Tutorial with Caption and Audio narration

 

 

 download-Link

 

Click the following link to get the drawing sheet of the model: http://a360.co/13F1eQr

 

 Transcription of Video

Creating hole on a curve surface

In this Video we will show how to create holes on a Curved Surface using our Model ‘Strainer’.

  1. This is the model of ‘Strainer’ on which we want to create holes on it curved surface like this.
  2. First of all, we will enter in the part modelling environment by double clicking the Part1.
  3. We have already created Work Points on the curved surface of Strainer on the basis of a previously created sketch.
  4. These are all the Work Points, which you can see in the Browser Bar as well as in the design window.
  5. In the half section view, you can see it clearly that all the Work Points are landing on the curved face on the Strainer.
  6. This is the sketch on the basis of which all the Work Points were created earlier.
  7. A sketch of hole is required to create a hole on the Work Point.
  8. So first of all we will create a Work Plane on the Work Point that would be tangent to the curved surface of the Strainer.
  9. Take the project of Work Point and start the Circle Tool to create a circle of 0.03125 unit length.
  10. Finish the sketch.
  11. To create a hole on this sketch, we will use Extrude Command.
  12. Click Extrude from the Create Panel of 3D Model Tab.
  13. Click the circular profile.
  14. In the direction field, select ‘Symmetric’ option.
  15. Select ‘Cut’ option to remove the material from the curved surface of the Strainer and the hole is created.
  16. Turn off the visibility of the Work Plane.
  17. Now we will use the Circular Pattern Tool, that will replicate this extrude feature 80 times.
  18. First select the feature then the rotation axis.
  19. We will select the rotation axis as Y Axis from the Browser Bar.
  20. In the Placement field type 80.
  21. All the holes are now created.
  22. In the same way, we will create another hole on this Work Point.
  23. Same operations are being performed.
  24. This time we will activate the Extrude Command by just clicking the sketch, here you can see.
  25. The Extrude Command is visible there.
  26. In the second row, the circumference of the model has decreased, so we have to select less number of holes (i.e., 78 occurrences) in this Circular Pattern.
  27. In the same manner other holes can be created on the curved surface of the object easily, to get the desired result.
  28. Here is the finished Assembly of the Strainer you can see all the holes are here.