Motor Blower Assembly : Week 4 Challenge

Motor Blower Part design and Assembly.(Top Down Assembly method)

Part design and Assembly(Geometrical set=GS)

1. In Mechanical Design, open assembly work bench and name the product as motor blower.
2. In product work bench, under insert option select the new part body and name it as Lower Housing.
3. In the above new body, create a origin point at x=0,y=0& z=0.draw a profile using circle and centre rectangle command and remove all unwanted lines using quick trim option.
4. Extrude the above profile to 4mm on both side along y-axis.
5. In new GS,draw a closed semi circle with it centre coincident to the origin point and on xz plane. extrude the profile to 3.75mm on both side along y-axis in new body and then remove this body from the above body using remove command under boolen operation.
6. in new GS, select the top plane as sketch plane and draw 8 circle of dia 0.41mm at given location. then use pocket command and select the circles, to create circular pocket on the part body.
7. in new GS, draw a semi circle of R4.88mm on surface parallel to xz plane and 4mm from the origin and create a circular cut on body using pocket command and selecting the current profile.
8. In new GS, draw a close semi circle of R1.5mm on plane parallel to xz plane and at 4mm from the origin. create a pocket on the body by selecting the current profile.
9. Under the product, create a new part body and rename it as Upper Housing. make origin point at x=0,y=0& z=0.
10. In new GS, draw a rectangle of 7.25mm*5.25mm at a height of 4.75mm on a plane parallel to yz plane and at a dist of 11.97mm from the origin. draw another rectangle of 5.75mm*4.2mm at a height of 4.8mm on plane parallel to yz palne and at a dist of 6.22mm from the origin.
11. Draw two seperate sketch using line and arc command on xz plane.
12. Select the above two rectangle sketch and the line & arc under multi section solid command as section and guide to form a body.
13. In new GS, draw a profile using three point arc and line command on xz plane.
14. In new sketch, draw a rectangle of 5.75mm*4.2mm on plane parallel to yz plane at 6.22m from the origin.
15. Select the above two sketch under rib command as profile and guide curve to form a body. add this body to the above body using add command under boolen operation.
16. In new GS, draw profile using circle of R6mm and line and extrude it to 4mm on both side along y-axis in body. Add the current body with the above body using add command.
17. Use shell command on the body obtained from adding the above three bodies, with inner thickness of 0.25mm and select the faces to remove.
18. In new GS, draw 8 circles of 0.41mm dia at required location and use pocket command to create screw hole by selecting the current profile.
19. In new GS, draw close semi circle of dia 4.88mm on plane parallel to xz plane at a dist of 4mm from the origin and create a pocket on the body using pocket command and current profile.
20. In new GS, draw a close semi circle profile of R1.5mm on plane parallel to xz plane at a dist of -4mm from the origin along y-axis and create a pocket on body using current profile.
21. Under product , create new part body and name it as Blower. make a origin point at x=0,y=0 & z=0.
22. draw a profile using line command on yz plane and use shaft command on the current profile to create part.
23. in new GS, draw a blade like structure using circle and line command on top surface as a sketch plane and extrude it to 6.5m along z-axis in new body. select the current body and add it to part body using add command under boolen operation.
24. In new GS, draw two concentric circle of dia 10.85mm and dia 8mm on plane parallel to xy plane at a dist of 6.5mm from the origin. and extrude it to 0.25mm along z-axis on new body and add the current body with the above body using add command.
25. Under product, create a new part body and name it as Motor. make a origin point at x=0,y=0 & z=0 using reference element.
26. Draw a profile using circle of R3.5mm and line command on xz plane with centre of circle coincident with origin. extrude the profile to 6.5mm along y-axis.
27. In new GS, draw a circle coincident to circle on the above profile and extrude it to 2.75mm along y-axis in new body and add the current to the above body using add command.
28. In new GS, draw a circle of dia 10mm with three small circle at 4.25mm from the centre with angular spacing of 120 degree on the surface at 2.75 mm from the origin as sketch plane. extrude the current profile to 0.5mm towards the part in new body and the add it to the above body.
29. In new GS, draw a heat exchange fin structure with height of 6mm from the centre using profile command and give the required dimension on a plane parallel to xz plane at a dist of 2.25mm fromm the origin.
30. Extrude the above body to 8mm along y-axis in new body and add it to the main part body.
31. In new GS, draw a circle of dia 6mm on a plane parallel to xz plane at a dist 2.75mm from the origin. extrude the current profile to 8.75 mm into the part in new body and then remove the current body from the main part body to generate a cylindrical hole.
32. In new GS, draw a circle of dia 1.5mm on the surface of the part parallel to xz plane at 6.5mm from the origin as sketch plane and generate a hole using current profile through pocket command.
33. Under the product, add a new part and name it as Cover. make origin point at x=0,y=0 & z=0.
34. Draw a circle of dia 7mm and extrude it to 2.5mm along z-axis.
35. In new GS, draw three screw flange at circumfrence of above profile using two concentric of R0.75mm & D0.75mm and lines tangent to R0.75mm circle. extrude the current profile to 0.5mm along z-axis in new body.
36. Add the above body to the main part using add command under boolrn operation.
37. In new GS, draw 7 elongated hole of D0.35mm and instance spacing of 0.6mm along y-axis on top surface of part body or plane parallel to xy plane at 2.5mm from the origin as sketch plane.
38. Extrude the above profile to 0.5mm into the part in new body and the remove the current body from the main part body.
39. In new GS, draw a circle of R1.4mm on plane parallel to xy plane at adist of 2.25 mm from the origin. extrude the curren tprofile to 1mm along z-axis in new body and add it to the main part body.
40. In new GS, draw a circle of D1.5mm on top surface of the part as sketch plane at 3.5mm form the origin. extrude the current profile to 1mm into the part in new body, then remove it from the main part body using remove command under boolen operation.
41. Under product, add a new part body and name it as shaft. draw a shaft profile and use shaft command to make shaft. then double click on product to get back to assembly work bench.
42. Fix the Motor using fix command and then assembly the Motor & Cover using coincident and contact constraint.
43. Assembly the Upper and Lower housing using contact and coincident constraint.
44. Assembly the blower with Lower or Upper housing using coincident and offset constraint.
45. Move the housing assembly towards the motor using manipulation command wit recpect to the axis.
46. Assembly the shaft with housing assembly and motor assembly and update the constraint.
47. Double click on product, then go to enhaced scene option under scenes. select exploded view command and take motor as fix component. this process will create exploded view of the assembly.
48. Exit from the scenes, then double click on product to activate it. select the generate numbering command to create numdering for the assembly.

Drafting

1. In Mechanical design open drafting work bench with ISO standard and sheet size of A2.
2. Select isometric view in projection, then go to assembly work bench and click on any surface of assembly under isometric view. this process will generate a drawing of assembly in the sheet.
3. Select the isometric view, then go to product work bench and select View under application then click on any surface of the assembly. this will generate a drawing of exploded view of the assembly in the drawing sheet.
4. Select the exploded view drawing and then click on balloon generation to create numbering of the assembled part.
5. Select Bill of Material option under generation to create a BOM of the assembled part.