Tutorial - Making a bolt in Solidworks?

Here is the Tutorial. The attached file is the final output.
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Step 1:
Start Solidworks.
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Step 2:
Right Plane>>Sketch.
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Step 3:
Make a polygon circumscribed with circle dia 18mm.
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Step 4:
Extrude it by 7mm.
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Step 5:
We have the extruded polygon.
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Step 6:
On the right plane of the polygon start a sketch. Normal View to sketch.
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Step 7:
Make a circle tangent to the sides of polygon.
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Step 8:
Under features tab select Extruded Cut.
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Step 9:
Change extrude depth to 7mm. The draft angle to 60degree and check the flip side to cut. Click OK.
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Step 10:
Now you can see the polgon has rounded edges.
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Step 11:
Repeat the same steps for the other face also.
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Step 12:
Click on the right side circular face of the polygon and select sketch.
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Step 13:
Make a concentric circle of dia 16.6mm.
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Step 14:
Extrude it by 0.60mm.
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Step 15:
Select the circular face of the extruded body in previous step and select sketch.
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Step 16:
Make a circle of 12mm dia concentric to previous one.
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Step 17:
Extrude it by 50mm.
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Step 18:
Now we have the basic body of the bolt.
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Step 19:
Under features>>fillet arrow>>Chamfer.
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Step 20:
Select the circular edge of the bolt.
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Step 21:
Change chamfer settings to 1mm distance and 45degree.
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Step 22:
Now we have the chamfered body.
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Step 23:
Select this face and sketch.
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Step 24:
Under Sketch Tab choose convert entities.
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Step 25:
Select this edge and then click OK.
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Step 26:
Again click OK to exit convert entities.
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Step 27:
Under Features tab>>Curves>>Helix and Spiral.
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Step 28:
Choose Defined by Height and Pitch. Change the Height Value to 46mm and pitch value to 1.75mm keep other settings default.
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Step 29:
Click OK and we can see that helix has been creted.
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Step 30:
Top Plane>>Sketch.
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Step 31:
Make a equilateral triangle of side 1.7mm with one point coincident to the edge of the bolt.
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Step 32:
Under Features tab choose Swept cut.
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Step 33:
Choose the triangle sketch as profile.
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Step 34:
Choose helix as the path of the swept cut. Click OK.
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Step 35:
Now we are done, we have the bolt created.