Tutorial D: Pulley with drawing

Book	Shih, Parametric Modeling with Siemens NX, ch. 11
You learn	Revolve, Mirror Feature, a pattern leader hole, Circular Pattern, Base View, Section View
Sizes	Ø101.6 × 25.4 mm, hub Ø38.1, bore Ø19.05, web 6.35, five Ø12.7 holes on a Ø63.5 pitch circle (the book’s Ø4.00 × 1.00 in and so on); NotebookLM’s reading of the figures

In short

Revolve with nothing selected: sketch the half section, Ctrl+Q, revolve.
Select the feature, then Mirror Feature.
One hole as the pattern leader, then Circular Pattern with 5 occurrences.
Ctrl+Shift+D: New Sheet, Base View (right view), Section View through the centre.

The pulley drawing: right view and section A-A

Step by step

#	In the book (NX)	In FreeCAD NX-Style	Result	Notes
D1	File > New (Ctrl+N), Model template	Ctrl+N	same
D2	Revolve, nothing selected	ribbon 'Home › Feature > Revolve'	same
D3	Pick the XY plane of the datum CSYS	plane row + MB2	same	XY-plane (Base plane)
D4	Profile (Z): closed half cross-section, MB2	Z key + 9 MB1 clicks + MB2	same	tool True; 8 curves; ended True
D5	Rapid Dimension: profile sizes	values applied	differs	same tool; no dynamic dimensions
D6	Specify Vector = X axis through the origin, 0..360°, OK	axis 'Base X-axis', MB2 = OK	same	volume 51079.3 mm^3, expected 51079.3; 1 solid(s); NX picks the axis in the graphics window, FreeCAD lists it in the dialog
D7	Mirror Feature: select the revolved feature, MB2 to proceed	feature selected + ribbon 'Home › Pattern > Mirror Feature'	differs	selecting first and then starting Mirror Feature replaces NX’s 'select, then MB2'
D8	Plane = the back face (on the YZ plane), OK; Unite	plane 'Base YZ-plane', MB2 = OK	same	volume 102158.6 mm^3, expected 102158.6; 1 solid(s); inside a Body the mirror unites by itself, so NX’s separate Unite step is not needed
D9	Pattern leader: Extrude on the front face of the web, Subtract	select face + ribbon 'Home › Feature > Extrude (Subtract)'	differs	subtracting extrude is its own button in FreeCAD
D10	Circle Ø0.50 on the 2.50 pitch circle	O key + MB1 clicks + MB2; values applied	same	tool True; 1 curves
D11	Reverse Direction, End = Through All, OK	'Through all', MB2 = OK	same	volume 101354.2 mm^3, expected 101354.2; 1 solid(s); no Reverse needed in FreeCAD
D12	Pattern Feature, Layout = Circular	leader selected + ribbon 'Home › Pattern > Circular Pattern'	differs	NX has one Pattern Feature with a Layout list; FreeCAD has separate linear and circular buttons
D13	Axis X, Count and Span: 5 over 360°, OK	axis 'Base X-axis', 'spinOccurrences' = 5, MB2 = OK	same	volume 98136.6 mm^3, expected 98136.6; 1 solid(s)
D14	The finished part is shown in the graphics window	render of the graphics window	same	12.6% of the view shows the part
D15	File > Drafting (Ctrl+Shift+D)	Ctrl+Shift+D	same	TechDrawWorkbench
D16	New sheet, A-size, 1:1	ribbon 'Home › Drawing > New Sheet'	differs	FreeCAD’s default template Default_Template_A4_Landscape.svg; an ANSI A sheet is one template choice away (Sheet from Template)
D17	Base View: Right view of the pulley	body selected + ribbon 'Home › View > Base View'; dialog closed with MB2	same	1 view(s) on the sheet; direction set to Right (+X)
D18	Add a projected view, select it, Delete key	Base View again + Delete key	differs	views 2 → 1. NX drags projected views off the base view; FreeCAD’s Projected View is a projection group, so a second Base View stood in for it
D19	Section View through the centre of the base view	base view selected + ribbon 'Home › View > Section View', direction 'pbLeft', MB2 = OK	same	1 section view(s), 42 visible edges
D20	Drag the section to the right of the base view, MB1 to place	X/Y of the section set	differs	FreeCAD places the section on top of the base view; it is moved afterwards (placed at x = 224.7 mm, base at 148.5 mm)

In the book (NX)

In FreeCAD NX-Style

Result

Notes

File > New (Ctrl+N), Model template

Ctrl+N

same

Revolve, nothing selected

ribbon 'Home › Feature > Revolve'

same

Pick the XY plane of the datum CSYS

plane row + MB2

same

XY-plane (Base plane)

Profile (Z): closed half cross-section, MB2

Z key + 9 MB1 clicks + MB2

same

tool True; 8 curves; ended True

Rapid Dimension: profile sizes

values applied

differs

same tool; no dynamic dimensions

Specify Vector = X axis through the origin, 0..360°, OK

axis 'Base X-axis', MB2 = OK

same

volume 51079.3 mm^3, expected 51079.3; 1 solid(s); NX picks the axis in the graphics window, FreeCAD lists it in the dialog

Mirror Feature: select the revolved feature, MB2 to proceed

feature selected + ribbon 'Home › Pattern > Mirror Feature'

differs

selecting first and then starting Mirror Feature replaces NX’s 'select, then MB2'

Plane = the back face (on the YZ plane), OK; Unite

plane 'Base YZ-plane', MB2 = OK

same

volume 102158.6 mm^3, expected 102158.6; 1 solid(s); inside a Body the mirror unites by itself, so NX’s separate Unite step is not needed

Pattern leader: Extrude on the front face of the web, Subtract

select face + ribbon 'Home › Feature > Extrude (Subtract)'

differs

subtracting extrude is its own button in FreeCAD

D10

Circle Ø0.50 on the 2.50 pitch circle

O key + MB1 clicks + MB2; values applied

same

tool True; 1 curves

D11

Reverse Direction, End = Through All, OK

'Through all', MB2 = OK

same

volume 101354.2 mm^3, expected 101354.2; 1 solid(s); no Reverse needed in FreeCAD

D12

Pattern Feature, Layout = Circular

leader selected + ribbon 'Home › Pattern > Circular Pattern'

differs

NX has one Pattern Feature with a Layout list; FreeCAD has separate linear and circular buttons

D13

Axis X, Count and Span: 5 over 360°, OK

axis 'Base X-axis', 'spinOccurrences' = 5, MB2 = OK

same

volume 98136.6 mm^3, expected 98136.6; 1 solid(s)

D14

The finished part is shown in the graphics window

render of the graphics window

same

12.6% of the view shows the part

D15

File > Drafting (Ctrl+Shift+D)

Ctrl+Shift+D

same

TechDrawWorkbench

D16

New sheet, A-size, 1:1

ribbon 'Home › Drawing > New Sheet'

differs

FreeCAD’s default template Default_Template_A4_Landscape.svg; an ANSI A sheet is one template choice away (Sheet from Template)

D17

Base View: Right view of the pulley

body selected + ribbon 'Home › View > Base View'; dialog closed with MB2

same

1 view(s) on the sheet; direction set to Right (+X)

D18

Add a projected view, select it, Delete key

Base View again + Delete key

differs

views 2 → 1. NX drags projected views off the base view; FreeCAD’s Projected View is a projection group, so a second Base View stood in for it

D19

Section View through the centre of the base view

base view selected + ribbon 'Home › View > Section View', direction 'pbLeft', MB2 = OK

same

1 section view(s), 42 visible edges

D20

Drag the section to the right of the base view, MB1 to place

X/Y of the section set

differs

FreeCAD places the section on top of the base view; it is moved afterwards (placed at x = 224.7 mm, base at 148.5 mm)

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.

What differs from NX

Mirror Feature: select the feature first, then start the command.
NX’s one Pattern Feature with a Layout list is two buttons here; the axis is chosen in the dialog.
Projected View is a projection group: a second Base View stands in for a view dragged off the base view.
A new section view lands on its base view and is moved afterwards.