Saturday, December 2, 2017

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

Carb Intake Plate

Serial No. 291

Carb Intake Plate -- Autodesk Inventor 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.

download-Link

 

 

Click the following link to get the model file: - http://a360.co/1PtcVCR

 

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.

Engine Piston -- Autodesk Inventor Tutorial (with caption and audio narration)

Engine Piston_1

Serial No. 290

Engine Piston -- Autodesk Inventor Tutorial (with caption and audio narration)

The Design of ‘Engine Piston’ has been taken from Assembly file of 'Rear Exhaust-2 Shoe' of ‘Sample files’ of Autodesk Inventor, it is a fragment of ‘Engine MKII’ Assembly.
Rest components of the model ‘Engine MKII Assembly’ (consisting of several numbers) have also been designed. You may watch them by visiting on the following playlist:-
https://www.youtube.com/playlist?list=PLKWX3xUP3pPp1ndQrE1t73DCTp-W4ZWLd
________________________________________________________________
In this Inventor tutorial, we will create a Piston of an Engine. It is a part modelling tutorial that will cover following topics: ---
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• Creating 2D sketch profiles on different planes with the help of Circle tool, Rectangle tool, three-point Arc tool, Line tool etc.
• Each of the sketches will be fully constrained with proper dimensioning and sketch constraints or you can say by using Dimension tool.
• Adding 'Extrude' tool on the sketch to create the solid part and Extrude tool with 'Cut' option to remove the material from the solid body.
• Mirroring the feature about the centre plane of the model, adding fillets feature and changing the colour of the model the model.

download-Link

 

 

Click the following link to get the model file: - http://a360.co/1gBD5Y0

 

Transcription of the Video

  1. Create a new inch part file.
  2. Activate the Extrude command and create a new sketch over the XY plane.
  3. Create a circle of 0.551 inch diameter coincident from the origin.
  4. Finish the sketch, set the value 0.375 inch of extrusion and click OK.
  5. Fill the name of the file ‘Engine Piston’ and save it.
  6. Create a sketch on this face, take the project of the circle by using ‘Project Geometry’ command.
  7. Create a center point rectangle which is coincident with the center point of circle.
  8. Draw the two arcs and apply the dimensions.
  9. Add the equal and concentric constrain to get the sketch fully constrained.
  10. Activate the Extrude command, select the profile and choose ‘Cut’ option and set the depth value, click OK.
  11. Create a sketch on this face, take the project of part face by using ‘Project Geometry’ command.
  12. Choose slice graphics option, take the offset outside of the circle and set dimension value.
  13. Draw two lines between endpoint of tangent arc and line.
  14. Convert this circle into construction geometry and create another 3point arc to close the profile.
  15. Finish the sketch, select the profile and extrude it 0.0925inch, click OK.
  16. Now see, add another extruded feature has been created, which was made by the ‘Join’ operation earlier.
  17. Activate the ‘Mirror’ command select the extruded feature and choose mid plane, click OK.
  18. Activate the Fillet command, the fillet select mode type as feature select any one edge of the inside of part, it will be automatically selected all inside edges and apply it.
  19. Here three types of selection mode are available, any option can be selected as you need according to your design.
  20. Click Ok to create the fillet.
  21. The file is complete and save it.