**Regular Polygon - Begin Sketching ** Start with creating a sketch in the x-y plane. Draw a circle with its center at the midpoint of one of the reference planes. | |

**Construction ** Using the **Construction** tool, toggle the circle to construction. | |

**Irregular Polygon ** Using the **Line** tool, create an irregular polygon. Draw the lines on the construction circle, so that the endpoints are **connected** to the circle. | |

**Avoid Relations ** Take care that new points are **not** horizontally or vertically aligned with existing points. See figure. | |

**Last Point ** Draw six lines to create a hexagon. Take care that the last point clicked is on the end-point of the first line and not on the circle. See figure. | |

**Make Regular ** Click the **Equal** geometric relationship tool. Make the first line equal to the second line in the irregular polygon. See figure. | |

**Make Regular - Carry On ** Similarly, make the second line equal to the third line. and so on... | |

**Make Regular – Finish ** Finally, all sides of the polygon are equal. This makes the polygon a regular one. | |

**Make Horizontal ** If the polygon looks a little tilted, make one of its sides horizontal. Click the **Horizontal/Vertical** geometric relationship tool. Select a line to make horizontal. | |

**Make Horizontal – Done ** Since all the lines are connected to the circle and fully constrained, the hexagon rotates. Your figure should now look as shown with a side at the top or with one vertex at the top. | |

**Hexagon Dimension ** Apply a Smart Dimension to the circle. This dimension will control the size of the hexagon. | |

**Hexagon Dimension - Test It ** Tweak the dimension value. The hexagon should : Update accordingly. All lines should remain inside the circle. The hexagon should not rotate. | |

**Make a Nut ** Start the Protrusion command and select the hexagon as shown in figure. | |

**Make a Nut – Finish ** Complete the Protrusion. | |

**Revolved Cut – Begin ** Click the **Revolved Cut** tool on the **Features** toolbar. Select one of the vertical planes. | |

**Revolved Cut - Plane Select ** Choose the plane such that two faces of the nut are visible in the sketcher. This is important. See figure. | |

**Revolved Cut - Plane Check ** If you picked a plane and three faces of the nut are seen in the sketcher then, Click **Finish** in the sketcher **immediately** and return to the model. Click the other vertical reference plane. | |

**Axis of Revolution ** Click the **Axis of Revolution** tool and select the vertical plane. See figure. | |

**Draw Line ** Click the **Line** tool and draw a line as shown in figure. The first endpoint of the line should be **connected** to the vertical reference plane. | |

**Angular Dimension ** The other endpoint of the line should be **connected** to the end of the nut as shown. Apply an angular dimension of 30 deg to the line as shown in figure. | |

**Exit Sketcher ** Click **Finish** on the ribbon bar. Indicate the direction as shown in figure. | |

**All Round Cut ** Click the **Revolve 360** option on the ribbon bar. You will get the chamfer as desired. The elegance of this approach is that the revolved cut always remains as desired without adjusting any dimension or relation. | |

**Finish ** The only dimension to change is the diameter of the construction circle and the whole nut updates. Do you know what cMayoCAD is …?
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