Tutorial AP: Impeller Shaft

Source	Ming C. Leu, Wenjin Tao, Amir Ghazanfari and Krishna Kolan, NX 12 for Engineering Design (Missouri University of Science and Technology), section 4.2.2 (Model a Shaft).
You learn	Cylinder (Axis, Diameter, and Height), Cone (Diameters and Height), Specify Vector, the Point Dialog’s Arc/Ellipse/Sphere Center, Boolean Unite, Orient View > Isometric
Sizes	the book’s, in inches, typed in millimetres. A cylinder Ø4 × 18 on ZC from the origin. A cone from Ø4 to Ø6, 10 high, on the cylinder’s top. A cylinder Ø6 × 20 on the cone’s top.

Step by step

1. The first cylinder

Ctrl+N and save the part as Impeller_shaft. Click Cylinder (Home › Feature). Keep the type Axis, Diameter, and Height and choose ZC as the vector. In Specify Point leave XC, YC and ZC at 0, then type Diameter 4 and Height 18. Click OK.

Ctrl+F fits the cylinder in the window and End turns the view to Isometric (NX: MB3 > Orient View > Isometric).

2. The cone

Click Cone. Keep Diameters and Height and the ZC vector. In Specify Point choose Arc/Ellipse/Sphere Center and click the cylinder’s top edge: XC, YC and ZC become (0, 0, 18). Type Base Diameter 4, Top Diameter 6 and Height 10, choose Boolean Unite and click OK. The cylinder is the part’s only body, so the dialog selects it for the Unite by itself.

The cone united with the top of the cylinder

3. The second cylinder

Click Cylinder again, keep ZC, and with Arc/Ellipse/Sphere Center click the cone’s top edge: (0, 0, 28). Type Diameter 6 and Height 20, choose Unite and click OK.

Save the part.

The replay

#	In the book (NX)	In FreeCAD NX-Style	Result	Notes
AP1	Create a new file (Impeller_shaft)	Ctrl+N, Model template	same	new document ['Unnamed']
AP2	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)
AP3	Save it as Impeller_shaft	file name given once by script (the system file dialog is not driven); a change, then the Ctrl+S key	same	Impeller_shaft.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
AP4	Cylinder: Axis, Diameter, and Height; ZC Axis; Point Dialog (0, 0, 0); Diameter 4, Height 18; OK	ribbon 'Home › Feature', Type 'Axis, Diameter, and Height', Specify Vector 'ZC', XC/YC/ZC 0 typed, Diameter 101.6 and Height 457.2 typed, Boolean 'None', OK	same	volume 3706666.6 mm^3, expected 3706666.6; 1 solid(s); origin (0.0, 0.0, 0.0); one undo step ['Cylinder']
AP5	MB3 > Orient View > Isometric	Ctrl+F (Fit, to see the cylinder whole), End (NX’s Isometric key)	same	view direction (-0.5774, 0.5774, -0.5774) (isometric 1.000000)
AP6	Cone: Diameters and Height; ZC Axis; Point Constructor, Arc/Ellipse/Sphere Center on the cylinder’s top edge; Base Diameter 4, Top Diameter 6, Height 10; Unite with the cylinder; OK	ribbon 'Home › Feature', Type 'Diameters and Height', Specify Vector 'ZC', 'Arc/Ellipse/Sphere Center', MB1 on the edge at pixel (557, 98): Select Object (1) Arc/Ellipse/Sphere Center: 0, 0, 457.2, Base 101.6, Top 152.4, Height 254 typed, Boolean 'Unite', OK	same	volume 6967160.3 mm^3, expected 6967160.3; 1 solid(s); origin (0.0, 0.0, 457.2); one undo step ['Cone']; united with Body
AP7	Cylinder: ZC Axis; Arc/Ellipse/Sphere Center on the cone’s top edge; Diameter 6, Height 20; Unite; OK	ribbon 'Home › Feature', Type 'Axis, Diameter, and Height', Specify Vector 'ZC', 'Arc/Ellipse/Sphere Center', MB1 on the edge at pixel (557, 96): Select Object (1) Arc/Ellipse/Sphere Center: 0, 0, 711.2, Diameter 152.4 and Height 508 typed, Boolean 'Unite', OK	same	volume 16233826.7 mm^3, expected 16233826.7; 1 solid(s); origin (0.0, 0.0, 711.2); one undo step ['Cylinder']; united with Body
AP8	The shaft: cylinder, cone and cylinder in one solid	compared with the book’s dimensions	same	same solid as the reference: 0 mm³ differ, box within 1.4e-14 mm, 5 faces (5 in the reference)
AP9	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_shaft.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

AP1

Create a new file (Impeller_shaft)

Ctrl+N, Model template

same

new document ['Unnamed']

AP2

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)

AP3

Save it as Impeller_shaft

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

same

Impeller_shaft.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

AP4

Cylinder: Axis, Diameter, and Height; ZC Axis; Point Dialog (0, 0, 0); Diameter 4, Height 18; OK

ribbon 'Home › Feature', Type 'Axis, Diameter, and Height', Specify Vector 'ZC', XC/YC/ZC 0 typed, Diameter 101.6 and Height 457.2 typed, Boolean 'None', OK

same

volume 3706666.6 mm^3, expected 3706666.6; 1 solid(s); origin (0.0, 0.0, 0.0); one undo step ['Cylinder']

AP5

MB3 > Orient View > Isometric

Ctrl+F (Fit, to see the cylinder whole), End (NX’s Isometric key)

same

view direction (-0.5774, 0.5774, -0.5774) (isometric 1.000000)

AP6

Cone: Diameters and Height; ZC Axis; Point Constructor, Arc/Ellipse/Sphere Center on the cylinder’s top edge; Base Diameter 4, Top Diameter 6, Height 10; Unite with the cylinder; OK

ribbon 'Home › Feature', Type 'Diameters and Height', Specify Vector 'ZC', 'Arc/Ellipse/Sphere Center', MB1 on the edge at pixel (557, 98): Select Object (1) Arc/Ellipse/Sphere Center: 0, 0, 457.2, Base 101.6, Top 152.4, Height 254 typed, Boolean 'Unite', OK

same

volume 6967160.3 mm^3, expected 6967160.3; 1 solid(s); origin (0.0, 0.0, 457.2); one undo step ['Cone']; united with Body

AP7

Cylinder: ZC Axis; Arc/Ellipse/Sphere Center on the cone’s top edge; Diameter 6, Height 20; Unite; OK

ribbon 'Home › Feature', Type 'Axis, Diameter, and Height', Specify Vector 'ZC', 'Arc/Ellipse/Sphere Center', MB1 on the edge at pixel (557, 96): Select Object (1) Arc/Ellipse/Sphere Center: 0, 0, 711.2, Diameter 152.4 and Height 508 typed, Boolean 'Unite', OK

same

volume 16233826.7 mm^3, expected 16233826.7; 1 solid(s); origin (0.0, 0.0, 711.2); one undo step ['Cylinder']; united with Body

AP8

The shaft: cylinder, cone and cylinder in one solid

compared with the book’s dimensions

same

same solid as the reference: 0 mm³ differ, box within 1.4e-14 mm, 5 faces (5 in the reference)

AP9

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_shaft.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 shaft is compared with the book’s, built from its dimensions: two cylinders and a frustum on one axis.

What differs from NX

NX’s Point Dialog opens as its own window. In NX-Style’s Cylinder and Cone dialogs its type and its XC, YC and ZC are fields of the dialog itself.
NX lists Cylinder and Cone under More in the Feature group; NX-Style shows them in the group.
The Cylinder’s Arc and Height type and the Cone’s other four types are not offered yet; the list’s tooltip names them.