Stock Bracket Assembly : Week 4 Challenge

Part design and Assembly of Stock bracket

Part design and Assembly            (GS= geometrical set)

1. In Mechanical design open a new product work bench and name it as Stock bracket.
2. Under the product open a new part body and name it as Base. draw a profile on yz plane and use shaft command with respect to z-axis to create a body.
3. In new GS, draw three screw flange using circle of R0.74mm & line tangent to circle. extrude the current profile in new body along y-axis to 1.5mm and add the curren tbody to the above body using add command.
4. In new GS, draw a circle of D1.5mm on plane parallel to xz plane at dist of 4.28mm from the origin and extrude the profile to 1.62mm along y-axis in new body. add the current body with the main part body.
5. then draw a circle of D0.75mm on the above cylinder and pocket it to 1.62mm into the body.
6. Select the hole command on bottom surface at 1.5mm fromm the origin of the main part body and create a counter bore hole of spicified dimension and use pattern command to get the desired hole in specific location.
7. In new GS, draw a circle of D1.5mm at given location and extrude it to the surface of main part in new body. draw a circle of D1.75mm concentric to the above created cylinder and extruded it to 0.38mm in the same body.
8. Add the above body to the main part body using add command under boolen operation.
9. Under the product, open a new part body and name it as Stock support roller. draw a geometry using profile command with the required dimension and using shaft command with y-axis as axis of rotation to generate a roller body.
10. Under the product, create a new part body and name it as Adjusting screw nut. draw a cross section profile of the nut and use shaft command to make a part.
11. In new plane at 1.5mm away from the origin and parallel to the xz plane, create hole of D0.75mm and depth of 1.3mm into the body. use circular pattern command to create 3 more pocket with circular surface as a reference. 
12. Under the product, create a new part body and name it as Support roller bracket. draw a profile using arc and line command of required dimensions and extrude it to 2mm on both side along x-axis.
13. In new GS, draw a roller support profile using line , circle of R0.75mm and cornor option. and extrude it to 0.6mm into the part in new body. add the current body to the main part body using add command.
14. In new GS, draw profile on the yz plane and extrude it to 0.5mm on both side along x-axis in new body to create a support. add the current body to the main part body using add command.
15. In new GS, draw a circle of D2mm and extrude it to 2.48mm along z-axis in new body and remove it from the current  body to generate a vertical cylindrical hole in the part.
16. In new GS, draw a cirlce of D0.6mm on yz plane at 0.95mm from the origin with its center coincident with z-axis  and extrude it to 1mm on both side along x-axis in new body. remove the current body from the main part to create horizontal cylindrical hole across the body.
17. Under the product creat a new part body and name it as Adjusting screw guide. draaw a linear proflie of length 11mm and use shaft command to create screw guide.
18. in new GS, draw a profile using circle & line command. extrude it to 0.37mm into the part in new body, then remove the current form the part to make screw head.
19. In the product, create anew part body and name it as Adjusting nut handle. draw a handle profile and use shaft command to create a handle. use chamfer command on sharp edge of handle with dimension of 0.06mm*90degree.
20. In product, create a new part body and name it as Support adjusting screw. draw a profile of length 23mm using line command and create shaft using shaft command.
21. In product, create a new part body and name it as Thrust. Draw a bearing profile of appropriate dimension and use shaft command to create a bearing body.
22. In new GS, go to generative shape design and creat a point at x=- 2.135, y=0 & z=0. use the point to generate a sphere using sphere command. go back to part design work bench, select the close surface command to create a 3D sphere. then use pattern command to get desired number thrust bearing ball.
23. Add the bearing ball to the bearing part body using add command.
24. Double click on product to get back to the assembly work bench. fix the Base using fix command under constraint option.
25. Bring the Adjusting nut handle to the product work bench three times, as required number is 4 for the assembly.
26. Use coincident and offset command to assembly the Stock support roller and support roller bracket. update the process.
27. Assembly the Support roller bracket and support adjusting screw using coincident & contact constraint.
28. Assembly Adjusting screw guide and base using coincident & offset command. then update the process.
29. Assembly the Base and Thrust using coincident & contact constraint command.
30. Assembly Adjusting screw nut using coincident constraint to assembly it to base and use contact constraint to attach it with the thrust. update the process.
31. Assembly all four Adjusting nut handle to the Adjussting screw nut using coincident and contact constraint.
32. Select the product and then click on generate numbering command to create numbering.
33. Open enhanced scenes option and select the assembbled product. click on exploded view then fix the base to create a exploded view. exit the secene work bench.

Drafting

1. Open drafting work bench and select the ISO standard with A0 Sheet size.
2. Select the isometric view, then go to product work bench and click on any surface of the assembly in isometric view. this process will create a drawing of assembly in drafting sheet.
3. Select the isometric view, then go to assembly work bench and click on exploded view under application and after select view click on any surface of assembly to generate a drawing of exploded vieiw of the assembly in the drafting sheet.
4. Select bolloon option under generation to create a bolloon numdering of the assembly.
5. Select the Bill of Matterial option to create a BOM of the assembled parts.