Tutorial M: The U-Bracket, parent/child relations

Book	Shih, Parametric Modeling with Siemens NX, ch. 7
You learn	Parent/child relations, renaming, Suppress and Unsuppress, sketching on the datum plane to drop a dependency
Sizes	A plate with two Ø19.05 holes, a half-round body across it (−31.75 to 31.75 mm), a 50.8 × 25.4 mm cut under it and a Ø6.35 drill (the book’s 0.75, 1.25, 2.0 × 1.0 and 0.25 in). The plate’s end radius (R25.4) and the body’s radius (R44.45) are NotebookLM’s reading of the figures.

The U-Bracket with the round opening; the rectangular cut is kept

In short

The plate with its holes; the half-round body, extruded Two sided.
The rectangular cut (Rect-Cut) under it, and the drill sketched on the cut’s face.
F2: name the features.
Select Rect-Cut, Home › Edit Feature › Suppress: the drill’s sketch loses its face.
Unsuppress; delete the drill and sketch it again on the datum XY plane: it no longer depends on the cut.
Suppress the rectangular cut and make an R31.75 round opening instead.

Step by step

#	In the book (NX)	In FreeCAD NX-Style	Result	Notes
M1	File > New, Model template, name U-Bracket	Ctrl+N	same	named at the first save
M2	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)
M3	Extrude, the XY plane of the WCS	X key, plane row + MB2	same	picked XY-plane (Base plane)
M4	Profile: two horizontal lines and two tangent arcs, MB2 twice	Z key + MB1 clicks + MB2; the arcs and sizes applied	differs	4 curves clicked; NX switches Profile to an arc by dragging MB1, FreeCAD’s polyline by pressing M while drawing
M5	Two circles on the arcs' centres; dimensions (Equal Radius if needed)	O key + 2 MB1 clicks + MB2, twice; centres, Equal and the sizes applied	same	solver 'Fully constrained' (0 DoF); R1.00 ends 5.00 apart, Ø0.75 holes, centred on the origin
M6	Extrude 0.5 in, OK	Ctrl+Q, 'lengthEdit' = 12.7 mm, MB2 = OK	same	volume 100436.5 mm^3, expected 100436.5; 1 solid(s)
M7	Extrude, the XZ plane of the datum coordinate system	X key, plane row + MB2	same	picked XZ-plane (Base plane)
M8	Arc: centre on the sketch origin, end points on the edge; Line closing it; one radius dimension: fully constrained	A key + 3 MB1 clicks + MB2, L key + 2 clicks + MB2; R1.75	same	solver 'Fully constrained' (0 DoF); the book asks why one dimension is enough: the centre and the end points sit on the datum axes
M9	Limits: Start -1.25, End 1.25, Boolean Unite, OK	'Two sided', 'lengthEdit' = 'lengthEdit2' = 31.75 mm, MB2 = OK	same	volume 240949.5 mm^3, expected 240949.5; 1 solid(s); across -31.75 .. 31.75 mm. NX’s two limits are FreeCAD’s 'Two sided' (a length each way); features in a Body unite by themselves
M10	Extrude, the front vertical face	select Face7 + ribbon 'Home › Feature > Extrude (Subtract)'	differs
M11	Rectangle, dimensions 2.0 x 1.0	R key + 2 MB1 clicks + MB2; sizes applied	same	centred on the body, on the base plane
M12	Subtract, Through All both ways, OK	'Through all', MB2 = OK	same	volume 159014.2 mm^3, expected 159014.2; 1 solid(s); from the front face one way is all of it
M13	Extrude, the underside face of the cut	select Face15 + ribbon 'Home › Feature > Extrude (Subtract)'	differs
M14	More > Project Curve: the datum origin; Circle Ø0.25 on it	the origin point projected (API: it is hidden in the view); O key + 2 clicks + MB2; Ø applied	differs	origin projected: True; NX picks the datum origin in the graphics window, FreeCAD’s origin point is hidden unless the Body’s origin is shown
M15	Subtract, Through All, OK	'Through all', MB2 = OK	same	volume 158411.0 mm^3, expected 158411.8; 1 solid(s)
M16	Rename the features: Base, Main-Body, Rect-Cut, CenterDrill	select + F2, type, Enter (4 times)	differs	NX: click the name twice; FreeCAD: F2
M17	Part Navigator > Dependencies: the parents of CenterDrill	the feature’s links (sketch attachment, base feature)	differs	sketched on ['Rect-Cut'], cut from Rect-Cut: Rect-Cut is its parent, as in the book. FreeCAD shows these in the feature’s properties (Attachment, Base Feature) rather than a Dependencies panel
M18	Suppress Rect-Cut: NX warns that CenterDrill cannot be placed	Rect-Cut selected + ribbon 'Home › Edit Feature > Suppress'	differs	Rect-Cut suppressed True; FreeCAD cannot place the child either: its sketch says 'AttachEngine3D: subshape not found Pocket.Face15'. No message box: the error marks the sketch in the Part Navigator, and the part keeps its last shape (volume 158411.0 mm^3). NXStyle’s Suppress is new: FreeCAD 1.1 has the property but no command (its Freeze is different)
M19	Suppress CenterDrill as well: the part shows the plate and the body only	CenterDrill selected + ribbon 'Home › Edit Feature > Suppress'	limit	volume 158411.0 mm^3 (the plate and the body: 240949.5). FreeCAD 1.1.4 still recomputes the suppressed drill’s sketch, which cannot find its face, and stops there: Body, Sketch003, CenterDrill stay out of date. NX leaves a suppressed child alone. Unsuppressing the parent (the book’s next steps) brings the model back
M20	Unsuppress CenterDrill: NX brings its parent Rect-Cut back too	CenterDrill selected + ribbon 'Home › Edit Feature > Suppress' (a toggle)	differs	Rect-Cut back by itself: False. FreeCAD unsuppresses only the selected feature
M21	Unsuppress Rect-Cut too: both back	Rect-Cut selected + ribbon 'Suppress'	same	volume 158411.0 mm^3, expected 158411.8; 1 solid(s)
M22	Delete CenterDrill (MB3 > Delete)	CenterDrill selected + Delete key; its sketch deleted too	same	volume 159014.2 mm^3, expected 159014.2; 1 solid(s); feature gone True; FreeCAD keeps the feature’s sketch (True), NX removes it
M23	A different approach (BORN): Extrude on the datum XY plane	XY plane selected + ribbon 'Home › Feature > Extrude (Subtract)'	differs
M24	Circle Ø0.25 on the datum origin	O key + 2 MB1 clicks + MB2; on the origin, Ø applied	same	DoF 0
M25	Subtract, Through All, OK	'Through all', 'checkBoxReversed' on (up from the plane), MB2 = OK	same	volume 158411.0 mm^3, expected 158411.8; 1 solid(s); FreeCAD cuts away from the plane’s normal by default, so it is reversed to go up
M26	Dependencies: the new drill’s parents are the XY plane and the base; Suppress Rect-Cut: the drill stays	Rect-Cut selected + ribbon 'Home › Edit Feature > Suppress'	same	sketched on ['Origin']; drill valid True; volume 239541.9 mm^3 (expected 239542.7). In FreeCAD each feature is cut from the one before (Rect-Cut); a suppressed feature passes its input on, so that link does not break
M27	Extrude, the front vertical face (circular cut)	select Face8 + ribbon 'Home › Feature > Extrude (Subtract)'	differs
M28	Circle R1.25 centred on the datum origin	O key + 2 MB1 clicks + MB2; R applied	same	the book’s text says 'rectangle', its figure and the design change a circle of radius 1.25
M29	Subtract, Through All, OK: the bracket with a round opening	'Through all', MB2 = OK	same	volume 139996.8 mm^3, expected 139997.2; 1 solid(s); two design options now live in one model (Rect-Cut suppressed)
M30	The U-Bracket is shown in the graphics window	render of the graphics window	same	13.1% of the view shows the part

In the book (NX)

In FreeCAD NX-Style

Result

Notes

File > New, Model template, name U-Bracket

Ctrl+N

same

named at the first save

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, the XY plane of the WCS

X key, plane row + MB2

same

picked XY-plane (Base plane)

Profile: two horizontal lines and two tangent arcs, MB2 twice

Z key + MB1 clicks + MB2; the arcs and sizes applied

differs

4 curves clicked; NX switches Profile to an arc by dragging MB1, FreeCAD’s polyline by pressing M while drawing

Two circles on the arcs' centres; dimensions (Equal Radius if needed)

O key + 2 MB1 clicks + MB2, twice; centres, Equal and the sizes applied

same

solver 'Fully constrained' (0 DoF); R1.00 ends 5.00 apart, Ø0.75 holes, centred on the origin

Extrude 0.5 in, OK

Ctrl+Q, 'lengthEdit' = 12.7 mm, MB2 = OK

same

volume 100436.5 mm^3, expected 100436.5; 1 solid(s)

Extrude, the XZ plane of the datum coordinate system

X key, plane row + MB2

same

picked XZ-plane (Base plane)

Arc: centre on the sketch origin, end points on the edge; Line closing it; one radius dimension: fully constrained

A key + 3 MB1 clicks + MB2, L key + 2 clicks + MB2; R1.75

same

solver 'Fully constrained' (0 DoF); the book asks why one dimension is enough: the centre and the end points sit on the datum axes

Limits: Start -1.25, End 1.25, Boolean Unite, OK

'Two sided', 'lengthEdit' = 'lengthEdit2' = 31.75 mm, MB2 = OK

same

volume 240949.5 mm^3, expected 240949.5; 1 solid(s); across -31.75 .. 31.75 mm. NX’s two limits are FreeCAD’s 'Two sided' (a length each way); features in a Body unite by themselves

M10

Extrude, the front vertical face

select Face7 + ribbon 'Home › Feature > Extrude (Subtract)'

differs

M11

Rectangle, dimensions 2.0 x 1.0

R key + 2 MB1 clicks + MB2; sizes applied

same

centred on the body, on the base plane

M12

Subtract, Through All both ways, OK

'Through all', MB2 = OK

same

volume 159014.2 mm^3, expected 159014.2; 1 solid(s); from the front face one way is all of it

M13

Extrude, the underside face of the cut

select Face15 + ribbon 'Home › Feature > Extrude (Subtract)'

differs

M14

More > Project Curve: the datum origin; Circle Ø0.25 on it

the origin point projected (API: it is hidden in the view); O key + 2 clicks + MB2; Ø applied

differs

origin projected: True; NX picks the datum origin in the graphics window, FreeCAD’s origin point is hidden unless the Body’s origin is shown

M15

Subtract, Through All, OK

'Through all', MB2 = OK

same

volume 158411.0 mm^3, expected 158411.8; 1 solid(s)

M16

Rename the features: Base, Main-Body, Rect-Cut, CenterDrill

select + F2, type, Enter (4 times)

differs

NX: click the name twice; FreeCAD: F2

M17

Part Navigator > Dependencies: the parents of CenterDrill

the feature’s links (sketch attachment, base feature)

differs

sketched on ['Rect-Cut'], cut from Rect-Cut: Rect-Cut is its parent, as in the book. FreeCAD shows these in the feature’s properties (Attachment, Base Feature) rather than a Dependencies panel

M18

Suppress Rect-Cut: NX warns that CenterDrill cannot be placed

Rect-Cut selected + ribbon 'Home › Edit Feature > Suppress'

differs

Rect-Cut suppressed True; FreeCAD cannot place the child either: its sketch says 'AttachEngine3D: subshape not found Pocket.Face15'. No message box: the error marks the sketch in the Part Navigator, and the part keeps its last shape (volume 158411.0 mm^3). NXStyle’s Suppress is new: FreeCAD 1.1 has the property but no command (its Freeze is different)

M19

Suppress CenterDrill as well: the part shows the plate and the body only

CenterDrill selected + ribbon 'Home › Edit Feature > Suppress'

limit

volume 158411.0 mm^3 (the plate and the body: 240949.5). FreeCAD 1.1.4 still recomputes the suppressed drill’s sketch, which cannot find its face, and stops there: Body, Sketch003, CenterDrill stay out of date. NX leaves a suppressed child alone. Unsuppressing the parent (the book’s next steps) brings the model back

M20

Unsuppress CenterDrill: NX brings its parent Rect-Cut back too

CenterDrill selected + ribbon 'Home › Edit Feature > Suppress' (a toggle)

differs

Rect-Cut back by itself: False. FreeCAD unsuppresses only the selected feature

M21

Unsuppress Rect-Cut too: both back

Rect-Cut selected + ribbon 'Suppress'

same

volume 158411.0 mm^3, expected 158411.8; 1 solid(s)

M22

Delete CenterDrill (MB3 > Delete)

CenterDrill selected + Delete key; its sketch deleted too

same

volume 159014.2 mm^3, expected 159014.2; 1 solid(s); feature gone True; FreeCAD keeps the feature’s sketch (True), NX removes it

M23

A different approach (BORN): Extrude on the datum XY plane

XY plane selected + ribbon 'Home › Feature > Extrude (Subtract)'

differs

M24

Circle Ø0.25 on the datum origin

O key + 2 MB1 clicks + MB2; on the origin, Ø applied

same

DoF 0

M25

Subtract, Through All, OK

'Through all', 'checkBoxReversed' on (up from the plane), MB2 = OK

same

volume 158411.0 mm^3, expected 158411.8; 1 solid(s); FreeCAD cuts away from the plane’s normal by default, so it is reversed to go up

M26

Dependencies: the new drill’s parents are the XY plane and the base; Suppress Rect-Cut: the drill stays

Rect-Cut selected + ribbon 'Home › Edit Feature > Suppress'

same

sketched on ['Origin']; drill valid True; volume 239541.9 mm^3 (expected 239542.7). In FreeCAD each feature is cut from the one before (Rect-Cut); a suppressed feature passes its input on, so that link does not break

M27

Extrude, the front vertical face (circular cut)

select Face8 + ribbon 'Home › Feature > Extrude (Subtract)'

differs

M28

Circle R1.25 centred on the datum origin

O key + 2 MB1 clicks + MB2; R applied

same

the book’s text says 'rectangle', its figure and the design change a circle of radius 1.25

M29

Subtract, Through All, OK: the bracket with a round opening

'Through all', MB2 = OK

same

volume 139996.8 mm^3, expected 139997.2; 1 solid(s); two design options now live in one model (Rect-Cut suppressed)

M30

The U-Bracket is shown in the graphics window

render of the graphics window

same

13.1% of the view shows the part

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

FreeCAD keeps a feature’s links in its properties (Attachment, Base Feature) rather than a Dependencies panel.
A suppressed feature passes its input on; a sketch attached to its face loses that face.
Suppressing the child as well still leaves the part out of date in FreeCAD 1.1.4 (M19); unsuppressing the parent brings it back.
Unsuppressing a child does not bring its parent back (NX does). Deleting a feature keeps its sketch.