Saturday, February 1, 2014

Double Sided Half V-Groove Weld Joint (Autodesk Inventor 2013)

Double Sided Half V-Groove Weld Joint

Serial No. 28

Double Sided Half V-Groove Weld Joint (Autodesk Inventor 2013)

Video Tutorial with Caption and Audio Narration

 

download-Link 

Click the following link to get the model file: -http://a360.co/12vcVMh

 

 

 

Transcription of Video

  1. Create a New Standard (in).ipt file.
  2. Draw a new sketch on XY Plane.
  3. Draw a Rectangle of sides 1 inch and 1/8 inch with the help of ‘Three point Centre Rectangle’ tool.
  4. The center point of the rectangle should lie on the auto projected part origin.
  5. Take the project of X Axis of part file by using Project Geometry tool.
  6. Select all the sketches in the graphics window and convert them into construction geometry.
  7. Add two more lines in the sketch and apply Symmetric constraint between them.
  8. And apply 45 degree dimension between these two lines.
  9. Close the profile by using line tool.
  10. Finish the 2D sketch.
  11. Select any one of the line of enclosed profile, a mini-toolbar will appear in the graphics window.
  12. Click the ‘Create Extrude’ icon.
  13. Extrude dialogue box is visible in the graphics window.
  14. In the Extents field, select ‘Symmetric’ option.
  15. Fill the value 2inch in the distance input box.
  16. Click OK to create the extrude feature.
  17. Change the model colour to 'Flaked Reflective - Beige'.
  18. Save the part file with its default name (Part1).
  19. Close the part file.
  20. Create a New Standard (in).iam file.
  21. Place two instances of ‘Part1’ in the assembly with the help of ‘Place Component’ tool.
  22. Save the Assembly with the name ‘Double Sided Half V-Groove Weld Joint’.
  23. Click the ‘Rotate’ icon on the Position panel of Assemble tab.
  24. Select Part1:2 in the design window and rotate the part as displayed.
  25. Right click in the graphics window and click OK to close the tool.
  26. Activate the Constraint command from the marking menu.
  27. Place Constraint dialogue box is visible in the graphics window.
  28. By default ‘Solution Type’ is set to Mate, change it to Flush.
  29. Select the top face of both parts to apply a flush mate.
  30. Apply a Flush mate once again but this time select front face of both parts.
  31. Apply a Mate constraint between side edges of both parts.
  32. Now our assembly is fully constrained.
  33. There is no degree of freedom.
  34. To apply a weld between these parts convert the assembly into weldment , click the ‘Convert to Weldment’ icon, located on the Convert panel of Assemble tab.
  35. Click Yes button, when prompted that you will not be able to revert this data to a basic assembly.
  36. Convert to Weldment dialogue box is visible in the graphics window.
  37. Leave the default settings click and OK to close the dialogue box.
  38. Double-click the ‘Welds’ group in the browser to activate the weldment tools.
  39. Activate the ‘Groove Weld’ tool, located on the Weld panel of Weld tab.
  40. Groove Weld dialogue box is visible in the graphics window.
  41. Select the Full Face Weld check box in the Face Set 1 and Face Set 2 under the Bead box field.
  42. Click the Face Set 1 button.
  43. Select this face of the Part.
  44. Click the Face Set 2 button.
  45. Select this face of adjacent part.
  46. Click OK to create a groove weld between the both parts.
  47. In the same manner apply another groove weld over the rear side of the model.
  48. Save the Assembly.