3 answers

• 
  Sudhir Gill about 1 year ago

  Here is the tutorial.

  1. Step 1

     Start SolidWorks.

     

  2. Step 2

     Top plane >> Sketch.

     

  3. Step 3

     Draw three equal construction line at 120º.

     

  4. Step 4

     Exit the sketch.

     

  5. Step 5

     Reference geometry >> Plane. Select the line and the end point. Click OK.

     

  6. Step 6

     Similarily create another plane for the line.

     

  7. Step 7

     Same step for third.

     

  8. Step 8

     Plane1 >> Sketch.

     

  9. Step 9

     Draw a circle of 50mm dia.

     

  10. Step 10

      Select Extruded surface under surface tab.

      

  11. Step 11

      Extrude it towards the Origin with a distance of 100mm.

      

  12. Step 12

      Plane2 >> Sketch.

      

  13. Step 13

      Draw circle of 50mm diameter.

      

  14. Step 14

      Extrude surface it with the same distance and towards the origin.

      

  15. Step 15

      Plane3 >> Sketch.

      

  16. Step 16

      Draw circle of 50mm diameter.

      

  17. Step 17

      Extrude surface it with the same distance and towards the origin.

      

  18. Step 18

      Top plane >> Sketch.

      

  19. Step 19

      Draw 3 lines collinear to each other and parallel to edge of pipe. These are 3 lines not one. This will create 3 edges.

      

  20. Step 20

      Exit the sketch and select trim surface under surfaces tab.

      

  21. Step 21

      Trim the surface using the line sketch as trimming tool.

      

  22. Step 22

      Similarily trim other two extrusions.

      

  23. Step 23

      Select lofted surface tool under surfaces tab.

      

  24. Step 24

      Select the edge of the pipe.

      

  25. Step 25

      And the corresponding edge of the other pipe.

      

  26. Step 26

      Under start/End constraints change them to Tangency to face. Click OK.

      

  27. Step 27

      Create the same feature for other two pipes.

      

  28. Step 28

      Same step for remaining two edges.

      

  29. Step 29

      Select Filled surface tool under surfaces tab.

      

  30. Step 30

      Select all upper the edges of the pipes.

      

  31. Step 31

      Change contact to tangent.

      

  32. Step 32

      Enable Apply to all edges. Click OK.

      

  33. Step 33

      Repeat the same step for lower side.

      

  34. Step 34

      Knit surface under surfaces tab.

      

  35. Step 35

      Select all surfaces and enable merge entities. Click OK.

      

  36. Step 36

      Now all surfaces are knitted into one.

      

  37. Step 37

      Select Thicken tool under surfaces tab.

      

  38. Step 38

      Select the surface knit and thickness be 2mm outside direction. Click OK.

      

  39. Step 39

      And the 3-pipe joint is created.

      

  1. 
     Branko Stokuca about 1 year ago

     Nice and elegant.

• 
  Chirag Aggarwal about 1 year ago

  very nice man!

  1. 
     Steve 12 months ago

     What do you mean by draw 3 collinear lines? Can you explain that a bit more please.

  2. 
     Sudhir Gill 12 months ago

     at step 19 there are three lines by 4 points... these are collinear and feels like one line.

  3. 
     nakama 2 months ago

     Hi Sudhir Gill, How did you select only a segment of the edge at Step 24 ??
     Thanks

• 
  Siboulotte 5 months ago

  Hy,
  Thanks for your help but how did you select only a part of the edge (Step24)
  Regards

  1. 
     nakama 2 months ago

     Me too same problem.....HOW to select only a segment ???

  2. 
     Sudhir Gill 2 months ago

     please check step 19 again. there are 3 lines not single line