Tutorial B: First part, cylinder and cone

Source	A first-part exercise put together from the NX textbooks (NotebookLM credited a university course but cited Shih and Tickoo)
You learn	Circle, Extrude, Revolve about a sketch axis
Sizes	Hollow cylinder Ø50/Ø30 × 50 mm; cone R25 × 50 mm

In short

Ctrl+N, X, XY_Plane, MB2.
O twice for the two circles, D for Ø50 and Ø30, Ctrl+Q, 50 mm, MB2.
A new part; Revolve with nothing selected; a triangle of R25 × 50 mm with Z; Ctrl+Q; revolve about the sketch’s vertical axis, MB2.

Step by step

#	In the book (NX)	In FreeCAD NX-Style	Result	Notes
B1	File > New (Ctrl+N), Model template, mm	Ctrl+N	same	new document ['Unnamed']
B2	Extrude (X), pick the XC-YC plane	X key, plane row + MB2	same	picked XY-plane (Base plane)
B3	Circle (O): two circles at the origin, MB2	O key + MB1 clicks + MB2	same	tool True; 2 circles; ended True
B4	Rapid Dimension: diameters 50 and 30	values applied	differs	same tool; values typed in FreeCAD’s dimension field
B5	Finish Sketch, Extrude 0 to 50 mm, OK	Ctrl+Q, 'lengthEdit' = 50, MB2 = OK	same	volume 62831.9 mm^3, expected 62831.9
B6	Revolve (ribbon)	ribbon 'Home › Feature > Revolve'	same	nothing selected: sketch first, as with Extrude
B7	Pick the YC-ZC plane	plane row + MB2	same	picked YZ-plane (Base plane)
B8	Line (L): right triangle on the axis, MB2	L key + MB1 clicks + MB2	same	tool True; 3 lines
B9	Rapid Dimension: height 50, radius 25	values applied	differs	same tool
B10	Finish Sketch returns to Revolve; axis = Z, 0..360 deg	Ctrl+Q	same	dialog open True; default axis ['V_Axis'] (sketch V axis = Z)
B11	Boolean Unite, OK	MB2 = OK	same	volume 95556.8 mm^3, expected 95556.8; features in one Body unite automatically
B12	Hold MB2 and drag to rotate	MB2 drag	same
B13	F8 snaps to the nearest standard view	F8 key	same	view Vector (0.0, 1.0, 0.0)
B14	The finished part is shown in the graphics window	render of the graphics window	same	11.3% of the view shows the part (an occupancy check: something is drawn; the shape itself is checked by its geometry)
B15	Save (Ctrl+S)	file name given once by script (the system file dialog is not driven); a change, then the Ctrl+S key	same	FirstPart.FCStd rewritten by Ctrl+S (1.1 s later), part unmodified afterwards (modified before the key: True); FreeCAD format, not .prt

In the book (NX)

In FreeCAD NX-Style

Result

Notes

File > New (Ctrl+N), Model template, mm

Ctrl+N

same

new document ['Unnamed']

Extrude (X), pick the XC-YC plane

X key, plane row + MB2

same

picked XY-plane (Base plane)

Circle (O): two circles at the origin, MB2

O key + MB1 clicks + MB2

same

tool True; 2 circles; ended True

Rapid Dimension: diameters 50 and 30

values applied

differs

same tool; values typed in FreeCAD’s dimension field

Finish Sketch, Extrude 0 to 50 mm, OK

Ctrl+Q, 'lengthEdit' = 50, MB2 = OK

same

volume 62831.9 mm^3, expected 62831.9

Revolve (ribbon)

ribbon 'Home › Feature > Revolve'

same

nothing selected: sketch first, as with Extrude

Pick the YC-ZC plane

plane row + MB2

same

picked YZ-plane (Base plane)

Line (L): right triangle on the axis, MB2

L key + MB1 clicks + MB2

same

tool True; 3 lines

Rapid Dimension: height 50, radius 25

values applied

differs

same tool

B10

Finish Sketch returns to Revolve; axis = Z, 0..360 deg

Ctrl+Q

same

dialog open True; default axis ['V_Axis'] (sketch V axis = Z)

B11

Boolean Unite, OK

MB2 = OK

same

volume 95556.8 mm^3, expected 95556.8; features in one Body unite automatically

B12

Hold MB2 and drag to rotate

MB2 drag

same

B13

F8 snaps to the nearest standard view

F8 key

same

view Vector (0.0, 1.0, 0.0)

B14

The finished part is shown in the graphics window

render of the graphics window

same

11.3% of the view shows the part (an occupancy check: something is drawn; the shape itself is checked by its geometry)

B15

Save (Ctrl+S)

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

same

FirstPart.FCStd rewritten by Ctrl+S (1.1 s later), part 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.