Carb Intake Plate -- Autodesk Inventor 2018 Tutorial (with caption and audio narration)

Serial No. 291

Carb Intake Plate -- Autodesk Inventor 2018 Tutorial (with caption and audio narration)

Hello viewers in this tutorial we are going to create a model named ‘Carb Intake Plate’. This component is used in the assembly of ‘Carb’. ‘Carb’ is used as the subassembly in ‘Engine MKII’ model with 2 Clutch Shoes provided by the Autodesk Inventor software as the sample file.

Click the following link to get the model file: - http://bit.ly/2o4EQGy

 

Transcription of the Video

1. Create a New part file with Inch units.
2. Create the sketch over the XY Plane.
3. Create a center point rectangle, coincident with the sketch origin.
4. Apply 0.55 inches of dimension on its two sides.
5. Apply fillets of 0.083 inches on all the four corners of the rectangle.
6. Finish the sketch and activate the Extrude command, set the value of extrusion to 0.0625 inches next click OK.
7. Change the Lightning in the file, here we are importing a customized settings which we saved earlier.
8. Change the colour of the model as per your wish so that it looks good.
9. Save the file with the name Carb Intake Plate.
10. Now create a sketch on the front face of the model.
11. Take the project of this face of the model by using the Project Cut Edges command.
12. Convert projected edges into the construction geometry.
13. Select four center points of the arc and convert it to center point.
14. Activate the Hole command, you can see here all the four points will be selected automatically, that were converted into center point earlier.
15. Fill the diameter of holes 0.1 inches and through all in termination field.
16. Click Ok to create the hole.
17. Turnoff the shaded view.
18. Create a work plane, -0.15 inches away from this face of the model.
19. Draw a sketch on this plane.
20. Activate Slice Graphic command and take the project of intersecting edges of the model.
21. Convert all the projected edges into construction geometry except following one.
22. Draw a line 0.25 inch offset from this line next add two more lines to create an a closed profile.
23. Add another line and add a coincident constraint between the midpoint of this line and end point of this line.
24. Convert this line into construction geometry.
25. Apply the angular dimension of 45° between these lines.
26. And exit from the sketching mode.
27. Create another work plane similar to the last one on the opposite side.
28. Activate the Extrude command sketch will be selected automatically, in the Extents field select ‘To’ option and select this work Plane.
29. Click Ok to create extrude feature.
30. Close the visibility of open work planes.
31. Apply a fillet of 0.125 inches on these two corners of the model.
32. Turnoff the textures to see the model clearly.
33. Create a hole on following face of the model.
34. Fill 0.15 and 0.125 inches in linear offset distance after defining the reference edges.
35. Fill the diameter of the hole 0.1875 and 0.3 inches in depth field.
36. The file is complete so save it.