Mug-Plastic (SolidWorks 2014 Tutorial)

Serial No. 81

Mug-Plastic (SolidWorks 2014 Tutorial)

Click the following link to get the model file: -http://bit.ly/31KHYXb

Creating a Notch of Mug-Autodesk Inventor 2013 (with caption and audio narration)

Serial No. 201

Creating a Notch of Mug-Autodesk Inventor 2013 (with caption and audio narration)

In this exercise, we are using a partially constructed model of ‘Mug-Plastic’. We will take help of 2D&3D sketches, work planes, work points, 3D surfaces by using boundary patch tool and sculpt feature to complete the model.

 

Click the following link to get the model file: - http://bit.ly/2osv0P9

 

 

Transcription of Video

1. Open the file of ‘Mug-Plastic’.
2. At present a surface is visible in the design window which is created with the help of Revolve Tool.
3. Open the visibility of Sketch1 from the browser bar.
4. Create a new work plane on this point, perpendicular to Y Axis of the model.
5. Auto-Resize this work plane.
6. Create a sketch on the newly created Work Plane11.
7. Take the project of XY plane and top circular edge of the model with the help of Project Geometry Tool.
8. Convert all the projected edges into construction geometry.
9. Close the visibility of Sketch1 from the browser bar.
10. Now proceed ahead and draw a triangular shape geometry intact with the projected circular edge of the model.
11. The sketch is complete, so exit from the sketching environment.
12. Create a new work plane, parallel to Work Plane11 at an offset distance of 1.25 inches in downward direction.
13. Close the visibility of Work Plane11.
14. Create a new sketch on Work Plane12.
15. Take the project of the model by using Project Cut Edges tool.
16. And take the project of XY Plane with the help of Project Geometry tool.
17. Finish the 2D sketch.
18. Create a work point at the intersection of this line and circle.
19. In the same manner add three more work points at the vertices of the triangular shaped geometry.
20. Close the visibility of Work Plane12 and Sketch22.
21. Activate ‘New 3D Sketch’ command from the marking menu.
22. Create a 3D Line between Work Point5 and Work Point6.
23. Right click in the graphic window and finish the 3D sketch.
24. In the same way, create a 3D Line between Work Point5 and Work Point7 in a new 3D sketch.
25. At last connect the Work Point8 with the Work Point5 by following the same procedure.
26. Close the visibility of all Work Points.
27. Activate the ‘Boundary Patch’ tool from the Surface Panel of 3D Model Tab.
28. Boundary Patch dialogue is visible in the graphics window.
29. Select two 3D Lines and one edge of triangular shaped geometry for creating a new 3D surface.
30. Click Ok to create the Boundary Patch Feature.
31. Open the visibility of Sketch21 which is hidden under the Boundary Patch Feature.
32. Activate the Boundary Patch Tool once again.
33. This time select the edge of Boundary Patch4 and both visible lines to create another Boundary Feature.
34. Activate the ‘Extend Surface’ tool from the drop down list of Surface panel.
35. Extend Surface dialogue box is visible in the graphics window.
36. Edges selection is active by default.
37. Select this edge of Boundary Patch4 to extend the surface.
38. Leave the value of Extents distance as it is and click Ok to execute the command.
39. In the same manner Extend the other 3D surface created with the help of Boundary Patch5.
40. Close the visibility of Sketch21.
41. Open the visibility of Work Plane11.
42. Activate the ‘Sculpt’ tool from the Surface Panel of 3D Model Tab.
43. Sculpt tool dialogue box is visible in the graphics window.
44. Surfaces selection is active by default.
45. Right click in the graphics window and ‘Select All’ option from the context menu.
46. A preview of sculpt is visible in the graphic window.
47. Click OK to create the Sculpt feature.
48. Sculpt feature combined all the surfaces into a solid body.
49. Close the visibility of Work Plane11 and save the part file.
50. Create a new sketch on the top face of the model.
51. Convert the projected top edge of the model into construction geometry.
52. Duplicate this enclosed profile by using Offset tool.
53. And set the offset distance value 0.125 inch.
54. Exit from the sketching environment.
55. Activate the Extrude command from the marking menu.
56. Enclosed profile is automatically selected in the graphics window.
57. Drag the direction indicator in downward direction.
58. Set the distance value 0.0625 inch on the mini tool bar.
59. Select ‘Join’ operation.
60. Click the green check mark to execute the extrude command.
61. Rotate the model on the back side.
62. Create a new sketch on this face.
63. Duplicate the outer projected edge of the model by offset tool.
64. Enter the offset distance value 0.0625 inch.
65. Finish the 2D Sketch.
66. Extrude this profile 0.1875 inch.
67. Click Home View button over the View Cube.
68. Activate the Shell tool from the Modify panel of 3D Model tab.
69. Shell dialogue box is visible in the graphics window.
70. Remove Faces selection option is activated by default.
71. Select top face of the model to remove it.
72. The preview of shell is visible in the graphics window.
73. Set the Thickness value 0.0625 inch.
74. Click OK to execute the Shell feature.
75. Now the notch of Mug is complete.
76. Inspect the model with the help of ‘Cross Section Analysis’ tool.

Application of ‘Loft’ tool Ex.2--Autodesk Inventor 2013 (with caption and audio narration)

Serial No. 200

Application of ‘Loft’ tool Ex.2--Autodesk Inventor 2013 (with caption and audio narration)

In this exercise, we are using a partially constructed model of ‘Mug-Plastic’. We will create a Handle on the curve surface of the model, for this we will add some 2D sketches, work planes and Loft feature.

 

 

Click the following link to get the model file: - http://bit.ly/2nNFfgo

 

 

 Transcription of Video

1. Open ‘Mug-Plastic’ part file.
2. Create a new work plane 0.25 inch below from the top face of the model.
3. Create a new sketch for upper portion of handle on the newly created work plane.
4. Right click in the graphics window and select Slice Graphics command.
5. Take the project of the model by using Project Cut Edges tool.
6. And with the help of Project Geometry tool, take the project of XY Plane.
7. Select all the sketches in the design window and convert them into construction geometry.
8. Now proceed further and draw a sketch with the given dimensions.
9. Exit from the sketching environment.
10. Close the visibility of Work Plane8 from the Browser Bar.
11. Create another work plane named 9, 3 inch below from the top face of the model.
12. Create a new sketch for lower portion of handle on Work Plane9.
13. Close the visibility of work plane and activate the Slice Graphics command.
14. Draw the sketch with the given dimensions.
15. Now the sketch is complete.
16. Finish the sketch.
17. Activate the ‘Loft’ tool.
18. Select the upper and lower sketch profiles in the graphics window.
19. Preview of Loft is visible.
20. Click OK to execute the loft feature.
21. Open the visibility of Sketch17 from the Browser Bar.
22. Create a new sketch on Work Plane8.
23. Take the project of these two lines and arc.
24. Draw a centre point arc between point1 and point2 (indicated by blue colour).
25. Close the visibility of Sketch17 from the browser bar.
26. Revert these two construction lines into regular lines.
27. Exit from the sketching environment.
28. Create a new work plane named 10, 0.0625 inch below from the top face of the handle.
29. Auto-Resize the work plane.
30. Create a new sketch on work plane 10.
31. Activate the Slice Graphics command.
32. Close the visibility of Work Plane10.
33. Take the project of the model by using Project Cut Edges tool.
34. And with the help of Project Geometry tool, take the project of XY plane.
35. Convert all the sketches in the graphics window into the construction geometry.
36. Draw the sketches as displayed.
37. Finish the sketch.
38. Activate the Loft tool once again.
39. Select the upper and lower enclosed profiles, created over the handle.
40. And click OK to execute the loft feature.
41. Now most of the portion of the handle is complete.
42. Save the part file.