Tutorial - Modeling 3 pipe joint in SolidWorks?

Here is the tutorial.
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Step 1:
Start SolidWorks.
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Step 2:
Top plane >> Sketch.
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Step 3:
Draw three equal construction line at 120º.
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Step 4:
Exit the sketch.
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Step 5:
Reference geometry >> Plane. Select the line and the end point. Click OK.
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Step 6:
Similarily create another plane for the line.
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Step 7:
Same step for third.
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Step 8:
Plane1 >> Sketch.
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Step 9:
Draw a circle of 50mm dia.
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Step 10:
Select Extruded surface under surface tab.
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Step 11:
Extrude it towards the Origin with a distance of 100mm.
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Step 12:
Plane2 >> Sketch.
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Step 13:
Draw circle of 50mm diameter.
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Step 14:
Extrude surface it with the same distance and towards the origin.
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Step 15:
Plane3 >> Sketch.
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Step 16:
Draw circle of 50mm diameter.
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Step 17:
Extrude surface it with the same distance and towards the origin.
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Step 18:
Top plane >> Sketch.
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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.
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Step 20:
Exit the sketch and select trim surface under surfaces tab.
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Step 21:
Trim the surface using the line sketch as trimming tool.
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Step 22:
Similarily trim other two extrusions.
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Step 23:
Select lofted surface tool under surfaces tab.
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Step 24:
Select the edge of the pipe.
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Step 25:
And the corresponding edge of the other pipe.
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Step 26:
Under start/End constraints change them to Tangency to face. Click OK.
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Step 27:
Create the same feature for other two pipes.
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Step 28:
Same step for remaining two edges.
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Step 29:
Select Filled surface tool under surfaces tab.
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Step 30:
Select all upper the edges of the pipes.
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Step 31:
Change contact to tangent.
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Step 32:
Enable Apply to all edges. Click OK.
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Step 33:
Repeat the same step for lower side.
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Step 34:
Knit surface under surfaces tab.
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Step 35:
Select all surfaces and enable merge entities. Click OK.
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Step 36:
Now all surfaces are knitted into one.
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Step 37:
Select Thicken tool under surfaces tab.
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Step 38:
Select the surface knit and thickness be 2mm outside direction. Click OK.
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Step 39:
And the 3-pipe joint is created.