Tutorial A: The Adjuster

Book	Shih, Parametric Modeling with Siemens NX, ch. 2
You learn	New part, Extrude from a sketch, Profile, Rapid Dimension, Extrude (Subtract)
Sizes	A 63.5 × 63.5 mm L outline with 19.05 mm legs, extruded 63.5 mm; a 25.4 mm wide, 19.05 mm deep slot (the book’s 2.5, 0.75 and 1.00 in)

In short

Ctrl+N, then X with nothing selected; pick XY_Plane, MB2.
Z (Profile): six MB1 clicks for the L, MB2 to end it.
D: the widths, heights and leg thicknesses.
Ctrl+Q: the Extrude dialog opens; 63.5 mm, MB2.
Select the top face, Home › Feature › Extrude (Subtract); R, two clicks, MB2; dimension the slot; Ctrl+Q; 19.05 mm, MB2.

The step list came from the book’s chapter by way of NotebookLM; its slot placement was ambiguous, so the slot is cut into the top of the vertical leg and the part stays one solid.

Step by step

#	In the book (NX)	In FreeCAD NX-Style	Result	Notes
A1	File > New (Ctrl+N), Model template	Ctrl+N	same	new document ['Unnamed'] with a Body; its datum planes appear when a plane is picked (kept hidden otherwise: FreeCAD 1.1.4 hides the part when they stay on)
A2	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)
A3	Extrude (X) with nothing selected	X key	same	FreeCAD asks for the sketch plane in the Dialog panel; NX asks in the graphics window
A4	Pick the XY plane, accept with MB2	plane row in the Dialog panel + MB2 click	same	picked XY-plane (Base plane); sketch in edit: Sketch
A5	Profile (Z), six MB1 clicks for the L outline	Z key + MB1 clicks in the graphics window	same	tool active True; 6 curves drawn
A6	MB2 ends Profile	MB2 click	same	tool ended = True
A7	Rapid Dimension (D): 2.5 width, 2.5 height, 0.75 legs	D key, values applied	differs	D starts FreeCAD’s Dimension tool. FreeCAD does not show NX’s dynamic dimensions on click, and there is no 'scale the whole sketch to the first dimension?' prompt
A8	Finish Sketch (Ctrl+Q) returns to the Extrude dialog	Ctrl+Q	same	Extrude dialog open = True; modals []
A9	Extrude: End = Value 2.5, Boolean None, OK	typed into 'lengthEdit', MB2 = OK	same	volume 130584.4 mm^3, expected 130584.4; same solid as the reference: 0 mm³ differ, box within 0 mm, 8 faces (8 in the reference)
A10	Extrude, pick the top face as sketch plane, Boolean Subtract	select face + ribbon 'Home › Feature > Extrude (Subtract)'	differs	the Extrude dialog’s Boolean list has Subtract (tutorial AE uses it); this replay uses the Extrude (Subtract) button, which starts the same command with Subtract chosen
A11	Rectangle ®, two MB1 clicks, MB2	R key + MB1 clicks + MB2	same	tool active True; 4 curves
A12	Rapid Dimension: 0.50 from edge, 1.00 wide, 0.75 deep	values applied	differs	as in step 6: same tool, no NX dynamic dimensions
A13	Finish Sketch returns to the (subtract) Extrude dialog	Ctrl+Q	same	dialog open = True
A14	Reverse Direction into the solid	-	differs	not needed: FreeCAD’s subtracting extrude cuts into the solid by default
A15	Slot depth 0.75, OK	'lengthEdit' = 19.05 mm, MB2 = OK	same	volume 121366.7 mm^3, expected 121366.7; 1 solid(s); same solid as the reference: 0 mm³ differ, box within 0 mm, 12 faces (12 in the reference)
A16	The finished part is shown in the graphics window	render of the graphics window	same	26.7% of the view shows the part (an occupancy check: something is drawn; the shape itself is checked by its geometry)
A17	Save (Ctrl+S)	file name given once by script (the system file dialog is not driven); a change, then the Ctrl+S key	same	Adjuster.FCStd rewritten by Ctrl+S (1.1 s later), part unmodified afterwards (modified before the key: True); FreeCAD format, not .prt
A18	Reopened part is shown	render of the graphics window	same	26.7% of the view shows the part (an occupancy check: something is drawn; the shape itself is checked by its geometry)

In the book (NX)

In FreeCAD NX-Style

Result

Notes

File > New (Ctrl+N), Model template

Ctrl+N

same

new document ['Unnamed'] with a Body; its datum planes appear when a plane is picked (kept hidden otherwise: FreeCAD 1.1.4 hides the part when they stay on)

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)

Extrude (X) with nothing selected

X key

same

FreeCAD asks for the sketch plane in the Dialog panel; NX asks in the graphics window

Pick the XY plane, accept with MB2

plane row in the Dialog panel + MB2 click

same

picked XY-plane (Base plane); sketch in edit: Sketch

Profile (Z), six MB1 clicks for the L outline

Z key + MB1 clicks in the graphics window

same

tool active True; 6 curves drawn

MB2 ends Profile

MB2 click

same

tool ended = True

Rapid Dimension (D): 2.5 width, 2.5 height, 0.75 legs

D key, values applied

differs

D starts FreeCAD’s Dimension tool. FreeCAD does not show NX’s dynamic dimensions on click, and there is no 'scale the whole sketch to the first dimension?' prompt

Finish Sketch (Ctrl+Q) returns to the Extrude dialog

Ctrl+Q

same

Extrude dialog open = True; modals []

Extrude: End = Value 2.5, Boolean None, OK

typed into 'lengthEdit', MB2 = OK

same

volume 130584.4 mm^3, expected 130584.4; same solid as the reference: 0 mm³ differ, box within 0 mm, 8 faces (8 in the reference)

A10

Extrude, pick the top face as sketch plane, Boolean Subtract

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

differs

the Extrude dialog’s Boolean list has Subtract (tutorial AE uses it); this replay uses the Extrude (Subtract) button, which starts the same command with Subtract chosen

A11

Rectangle ®, two MB1 clicks, MB2

R key + MB1 clicks + MB2

same

tool active True; 4 curves

A12

Rapid Dimension: 0.50 from edge, 1.00 wide, 0.75 deep

values applied

differs

as in step 6: same tool, no NX dynamic dimensions

A13

Finish Sketch returns to the (subtract) Extrude dialog

Ctrl+Q

same

dialog open = True

A14

Reverse Direction into the solid

differs

not needed: FreeCAD’s subtracting extrude cuts into the solid by default

A15

Slot depth 0.75, OK

'lengthEdit' = 19.05 mm, MB2 = OK

same

volume 121366.7 mm^3, expected 121366.7; 1 solid(s); same solid as the reference: 0 mm³ differ, box within 0 mm, 12 faces (12 in the reference)

A16

The finished part is shown in the graphics window

render of the graphics window

same

26.7% of the view shows the part (an occupancy check: something is drawn; the shape itself is checked by its geometry)

A17

Save (Ctrl+S)

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

same

Adjuster.FCStd rewritten by Ctrl+S (1.1 s later), part unmodified afterwards (modified before the key: True); FreeCAD format, not .prt

A18

Reopened part is shown

render of the graphics window

same

26.7% of the view shows the part (an occupancy check: something is drawn; the shape itself is checked by its geometry)

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

Units are a preference, not a choice in the New dialog; NX-Style parts are in millimetres.
No dynamic dimensions while you draw and no "scale the whole sketch?" prompt.
Subtracting is its own button, Extrude (Subtract); Extrude has no Boolean option.