Tutorial AR: Hexagonal Nut

Source	Ming C. Leu, Wenjin Tao, Amir Ghazanfari and Krishna Kolan, NX 12 for Engineering Design (Missouri University of Science and Technology), section 4.7.2 (Hexagonal Nut).
You learn	Polygon, Sphere at a typed point with Intersect, Mirror Feature through a face of the body, Cylinder with Subtract, Chamfer
Sizes	the book’s, in inches, typed in millimetres. Hexagon side 0.28685, extruded 0.125. Sphere Ø0.57 at (0, 0, 0.125). Hole Ø0.25 × 1 at the origin. Chamfer 0.0436.

Step by step

1. The hexagon

Ctrl+N and save the part as Impeller_hexa-nut. Click Sketch, pick the XC-YC plane and press MB2. Press P for Polygon, type 6 sides, then type the centre (0, 0) and the corner: length 7.28599 mm (0.28685 in) at angle 0. Press MB2, then Ctrl+Q.

Click Extrude, click a side of the hexagon, and type 3.175 mm (0.125 in). Click OK.

2. Half a nut

Click Sphere, keep Center Point and Diameter, and type XC 0, YC 0, ZC 3.175 (0.125 in). Type Diameter 14.478 (0.57 in), choose Intersect, and click OK.

3. The other half

Select the Intersect in the Part Navigator and click Mirror Feature (Home › Pattern). Choose Transform body, so that the whole half is mirrored. In the plane list choose Select reference… and pick the half’s flat top face. FreeCAD shows the origin planes while you pick, and one of them is in front of the face: press and hold MB1 and choose the face in QuickPick. Press MB2. The mirrored half is united with the body, so the book’s Unite step has nothing left to do.

4. The hole and the chamfers

Click Cylinder, choose ZC, keep the point at (0, 0, 0), and type Diameter 6.35 and Height 25.4. Choose Subtract, and click OK.

Select the hole’s two circular edges, click Chamfer, type 1.10744 mm (0.0436 in) and press MB2.

The finished nut: rounded corners on both faces

Save the part.

The replay

#	In the book (NX)	In FreeCAD NX-Style	Result	Notes
AR1	Create a new file (Impeller_hexa-nut)	Ctrl+N, Model template	same	new document ['Unnamed2']
AR2	Units in the New dialog (the book picks inches)	metric part kept; book sizes typed in mm	differs	FreeCAD sets units in Preferences, not in the New dialog; NXStyle defaults to millimetres (document: Standard (mm, kg, s, °); 25.4 mm shows as 25.40 mm)
AR3	Save it as Impeller_hexa-nut	file name given once by script (the system file dialog is not driven); a change, then the Ctrl+S key	same	Impeller_hexa-nut.FCStd rewritten by Ctrl+S: the file holds the change and the part is unmodified afterwards (modified before the key: True); FreeCAD format, not .prt
AR4	Polygon: 6 sides, Side Length 0.28685, at the origin	ribbon 'Home › Direct Sketch > Sketch' on 'XY-plane (Base plane)', P key ('Create Regular Polygon' 6 sides, OK; tool True), centre typed, corner typed, MB2	differs	6 sides; corners at the book’s hexagon (side 7.28599 mm, a corner on XC): all six. NX 12’s Insert > Curve > Polygon is a curve outside sketches; NX-Style draws the polygon in a sketch (NX 2212: Sketch > Polygon), whose corner is typed as the circumradius, which a hexagon’s side length equals
AR5	Extrude the hexagon, End Distance 0.125	ribbon 'Home › Feature > Extrude', a side picked (click; Curve Rule Inferred Curves), dialog opened True; Boolean 'None', 'lengthEdit' = 3.175 mm; OK clicked	same	volume 437.9 mm^3, expected 437.9; 1 solid(s); the part’s first solid
AR6	Sphere: Center Point (0, 0, 0.125) in the Point Dialog, Diameter 0.57, Boolean Intersect, OK	ribbon 'Home › Feature', Type 'Center Point and Diameter', XC/YC/ZC 0/0/3.175 typed, Diameter 14.478 typed, Boolean 'Intersect', OK	same	volume 433.2 mm^3, expected 433.2; 1 solid(s); origin (0.0, 0.0, 3.175); one undo step ['Sphere']; with Body
AR7	Edit > Transform: the model, Mirror Through a Plane, its flat side, Copy	the Intersect selected + ribbon 'Home › Pattern > Mirror Feature', Transform body True, plane 'Select reference…' and the flat top face by QuickPick (['Body › Origin › XZ-plane', 'Body › Origin › YZ-plane', 'Face4 of Body › Intersect', 'Face2 of Body › Intersect']) (Face4), MB2 = OK	differs	plane shown 'Intersect:Face4'; 1 solid, 866.4 mm^3 (twice 433.2), z -0.000 to 6.350 mm. NX’s Transform copies the body unparametrised; Mirror Feature keeps the copy following the half
AR8	Combine > Unite: the two halves	nothing to do	differs	Mirror Feature with Transform body unites the copy with the body itself: the nut is one solid
AR9	Cylinder: ZC, at the origin, Diameter 0.25, Height 1, Subtract from the nut, OK	ribbon 'Home › Feature', Type 'Axis, Diameter, and Height', Specify Vector 'ZC', XC/YC/ZC 0/0/0 typed, Diameter 6.35 and Height 25.4 typed, Boolean 'Subtract', OK	same	volume 665.3 mm^3, expected 665.3; 1 solid(s); origin (0.0, 0.0, 0.0); one undo step ['Cylinder']; with Body
AR10	Chamfer: the two inner edges, Distance 0.0436, OK	['Edge14', 'Edge54'] selected + ribbon 'Home › Feature > Chamfer', 'chamferSize' = 1.10744 mm, MB2 = OK	same	volume 638.0 mm^3, expected 638.0; 1 solid(s)
AR11	The nut	compared with the book’s dimensions	same	same solid as the reference: 0 mm³ differ, box within 7.1e-15 mm, 25 faces (25 in the reference)
AR12	Save the model	file name given once by script (the system file dialog is not driven); a change, then the Ctrl+S key	same	Impeller_hexa-nut.FCStd rewritten by Ctrl+S: the file holds the change and the part is unmodified afterwards (modified before the key: True); FreeCAD format, not .prt

In the book (NX)

In FreeCAD NX-Style

Result

Notes

AR1

Create a new file (Impeller_hexa-nut)

Ctrl+N, Model template

same

new document ['Unnamed2']

AR2

Units in the New dialog (the book picks inches)

metric part kept; book sizes typed in mm

differs

FreeCAD sets units in Preferences, not in the New dialog; NXStyle defaults to millimetres (document: Standard (mm, kg, s, °); 25.4 mm shows as 25.40 mm)

AR3

Save it as Impeller_hexa-nut

file name given once by script (the system file dialog is not driven); a change, then the Ctrl+S key

same

Impeller_hexa-nut.FCStd rewritten by Ctrl+S: the file holds the change and the part is unmodified afterwards (modified before the key: True); FreeCAD format, not .prt

AR4

Polygon: 6 sides, Side Length 0.28685, at the origin

ribbon 'Home › Direct Sketch > Sketch' on 'XY-plane (Base plane)', P key ('Create Regular Polygon' 6 sides, OK; tool True), centre typed, corner typed, MB2

differs

6 sides; corners at the book’s hexagon (side 7.28599 mm, a corner on XC): all six. NX 12’s Insert > Curve > Polygon is a curve outside sketches; NX-Style draws the polygon in a sketch (NX 2212: Sketch > Polygon), whose corner is typed as the circumradius, which a hexagon’s side length equals

AR5

Extrude the hexagon, End Distance 0.125

ribbon 'Home › Feature > Extrude', a side picked (click; Curve Rule Inferred Curves), dialog opened True; Boolean 'None', 'lengthEdit' = 3.175 mm; OK clicked

same

volume 437.9 mm^3, expected 437.9; 1 solid(s); the part’s first solid

AR6

Sphere: Center Point (0, 0, 0.125) in the Point Dialog, Diameter 0.57, Boolean Intersect, OK

ribbon 'Home › Feature', Type 'Center Point and Diameter', XC/YC/ZC 0/0/3.175 typed, Diameter 14.478 typed, Boolean 'Intersect', OK

same

volume 433.2 mm^3, expected 433.2; 1 solid(s); origin (0.0, 0.0, 3.175); one undo step ['Sphere']; with Body

AR7

Edit > Transform: the model, Mirror Through a Plane, its flat side, Copy

the Intersect selected + ribbon 'Home › Pattern > Mirror Feature', Transform body True, plane 'Select reference…' and the flat top face by QuickPick (['Body › Origin › XZ-plane', 'Body › Origin › YZ-plane', 'Face4 of Body › Intersect', 'Face2 of Body › Intersect']) (Face4), MB2 = OK

differs

plane shown 'Intersect:Face4'; 1 solid, 866.4 mm^3 (twice 433.2), z -0.000 to 6.350 mm. NX’s Transform copies the body unparametrised; Mirror Feature keeps the copy following the half

AR8

Combine > Unite: the two halves

nothing to do

differs

Mirror Feature with Transform body unites the copy with the body itself: the nut is one solid

AR9

Cylinder: ZC, at the origin, Diameter 0.25, Height 1, Subtract from the nut, OK

ribbon 'Home › Feature', Type 'Axis, Diameter, and Height', Specify Vector 'ZC', XC/YC/ZC 0/0/0 typed, Diameter 6.35 and Height 25.4 typed, Boolean 'Subtract', OK

same

volume 665.3 mm^3, expected 665.3; 1 solid(s); origin (0.0, 0.0, 0.0); one undo step ['Cylinder']; with Body

AR10

Chamfer: the two inner edges, Distance 0.0436, OK

['Edge14', 'Edge54'] selected + ribbon 'Home › Feature > Chamfer', 'chamferSize' = 1.10744 mm, MB2 = OK

same

volume 638.0 mm^3, expected 638.0; 1 solid(s)

AR11

The nut

compared with the book’s dimensions

same

same solid as the reference: 0 mm³ differ, box within 7.1e-15 mm, 25 faces (25 in the reference)

AR12

Save the model

file name given once by script (the system file dialog is not driven); a change, then the Ctrl+S key

same

Impeller_hexa-nut.FCStd rewritten by Ctrl+S: the file holds the change and the part is unmodified afterwards (modified before the key: True); FreeCAD format, not .prt

Result	Means
same	The book’s NX steps work as written.
differs	It works, but the FreeCAD way is different; the notes say how.
limit	The book’s way fails in FreeCAD itself; a workaround follows in the next steps.
missing	FreeCAD has no such function; a stand-in follows.
skipped	Not replayed; the notes give the reason.
FAILED	Did not work.

Result

Means

same

The book’s NX steps work as written.

differs

It works, but the FreeCAD way is different; the notes say how.

limit

The book’s way fails in FreeCAD itself; a workaround follows in the next steps.

missing

FreeCAD has no such function; a stand-in follows.

skipped

Not replayed; the notes give the reason.

FAILED

Did not work.

The finished nut is compared with the book’s dimensions built by FreeCAD’s Part API.

What differs from NX

NX 12 draws the hexagon with Insert > Curve > Polygon. Here, as in NX 2212, it is drawn in a sketch.
The book mirrors the half with Edit > Transform > Mirror Through a Plane, Copy, then unites the two bodies. NX-Style’s Mirror Feature in Transform body mode does both, and the copy keeps following the half.