Monday, November 18, 2013

Creating a component in an Assembly (Autodesk Inventor 2013)

 

Creating a component in an Assembly

 

Serial No. 147

Creating a component in an Assembly (Autodesk Inventor 2013)

Autodesk Inventor Tutorial with Caption and Audio narration

 

 

Transcription of Video

Creating a component in an Assembly

This video will display how to create a component in the context of an Assembly. Creating a component in this way has many benefits. We can Project faces and edges of the Assembly in the new component. The faces of other components can be copied and placed as surfaces and many more things can be done. So watch the video to understand.

  1. We have an Assembly named ‘Mesh (Front)’ consisting two components ‘Part1’ and ‘Part2’.
  2. Now we want to create a new component named ‘Part3’ in this Assembly like this.
  3. The Vertical distance between Part1 and Part2 is 1.625 inch.
  4. We will start our work with creating a new component in this Assembly.
  5. The degree of freedom command shows that the newly created Part3 is not fully constrained with the Assembly.
  6. So we will apply a Mate Constraint between the Part3 and Assembly’s Z Axis.
  7. Next a Mate Constraint will be applied between XZ Planes of Assembly and Part3.
  8. In the following steps, we will create a loft feature in this component with the help of two sketches and a centre line rail.
  9. By double clicking the Part3 we will enter in the Part Modelling Environment.
  10. First of all we will get the edges of previously created components with the use of ‘Project Geometry Tool.’
  11. These projected geometries are required only for reference. We are actually going to use these geometries in the developing the loft feature, that is why we will convert them in Construction Geometry.
  12. By applying Coincident Constraint we will properly position our geometry.
  13. Again unnecessary sketches will be converted into Construction Geometry.
  14. So we have created the required sketch now.
  15. Now we will create a New Work Plane parallel to YZ Plane of Part3 (7.625 inch away).
  16. Now we will create the remaining sketch on the XZ Plane of the Part3 that will be used for Centre line loft.
  17. From here we will change the colour of the Part to ‘Being Personal.’
  18. In the next following steps we will develop the second loft feature in this Part.
  19. At present we are copying the outer face of the Part2 with the ‘Copy Object’ Tool. This will place a new surface component in this part.
  20. Now we will project this sketch on the previously created surface component with the help of ‘Project to 3D Sketch’ Tool.
  21. At present this 3D sketch is intact. We cannot use its one edge as a rail in the loft feature. So we will create a new 3D sketch and project its one edge in it with the use of ‘Include Geometry’ Tool.
  22. Repeat the same process to create the second Rail.
  23. In this way, we found our two separate rails required for the loft.
  24. Now we will create two 3D sketch profiles required for the loft.
  25. So everything is set. Start the ‘Loft’ Tool.
  26. Model edges can also be used as rails.
  27. So in this way we created our second loft feature in the Part3.
  28. We will now replicate this (Part3) 8 times at an angle of 45 degree by using ‘Pattern Component’ Tool, available at Component Panel of Assembly Tab.
  29. If you want to watch the development of other components, used in the ‘Mesh of Table Fan’ Assembly, watch our previous video named ‘Mesh of Table Fan’ (Autodesk Inventor 2010).