Application of 3D Sketch in Solid Edge ST9 (with caption and audio narration)

Serial No. 106

Application of 3D Sketch in Solid Edge ST9 (with caption and audio narration)

This partial design has been used in my model 'Bulb Shade (Solid Edge Tutorial)'. I tried to emphasize regarding the use of 3D Arc by 3 Points tool, simultaneously creating surface with the help of 'Bound' command.

 

 

Transcription of the Video

1. Create a new sketch on XY plane.
2. Draw the two circles coincident from the part origin.
3. Apply the desired dimension.
4. Apply the symmetric constraint on these two lines and give the angular dimension.
5. Create a 3 Point Arc, between the intersection point of line and circle.
6. Save the part file.
7. Create a point H₁ on the circle and which lie on the end point of the vertical line.
8. Create a new Plane 1/2 inch below from XY plane along Z axis.
9. Create a new sketch on Plane4.
10. Create a point on Plane4 which is the project of point H₁.
11. In Sketch panel, click on 3D Sketch tool.
12. In 3D Draw panel, click on 3D Arc by 3 Points tool.
13. Select two endpoints A & B are on the arc of outer circle, and lie on XY Plane. Next, select point H₂ which lies on Plane4 which is the project of point H₁. (A, B and H₁ are coplanar points and lies on XY Plane).
14. Exit from the 3D sketch environment.
15. Go to the Surfacing tab, in the Surfaces panel click on Bounded tool.
16. Select the 3D Arc and Edge Set of (Sketch1).
17. Click on finish button to create the surface.

Allen Screwdriver—Double Ended (Solid Edge ST9 Tutorial)

Serial No. 30

Allen Screwdriver—Double Ended (Solid Edge ST9 Tutorial)
In this Solid Edge Tutorial we will describe how to build the model ‘Allen Screwdriver (Double Ended)’. The edge of Allen screwdriver (Double Ended) has been constructed by different surface tools like Bound, Stitch, Extend etc. It is a Part and Assembly modelling tutorial. This assembly consist 3 part files (Handle, Circular Rod, Sleeve etc.).
It will cover the following topics.
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• Creating 2D Sketches on different Planes.
• Use some sketch constraints as Connect, Horizontal/Vertical, and Equal etc. that are applied on during sketch creation.
• Use solid and surface feature command such as Revolved Cut, Bounded, Stitched, Extrude, Cut, Circular Pattern, Subtract, Round etc.
• How to create a line by using ‘3D Line’ command in 3D Sketch environment.
• How to change the color of the model by using ‘Part Painter’ tool.
• How to insert component into the assembly using drag and drop from parts library by using ‘Insert Component’ command.
• How to resize (scale) the handle of screwdriver with the help of ‘Part Copy’ command. You use the Part Copy Parameters dialog box to specify which geometry you want to copy and whether you want to mirror, scale, or flatten the copied geometry.
• How to create a sleeve part in context of an assembly in the assembly environment with the help of ‘Create Part In-Place’ command.
• How to mate the parts by using ‘Flash Fit’ command in the assembly.
• How to flip the component by using ‘Flip Side’ option in ‘Flash Fit’ command in the assembly.
• How to lock the rotation of the component by using ‘Lock Rotation’ option in ‘Flash Fit’ command in the assembly.
• Use the ‘Subtract’ command (Boolean) to remove the tool body volume from selected target bodies in the assembly. You can select multiple target bodies and multiple tool bodies.

Click the following link to get the model file: - http://bit.ly/35gBCB8

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.