Tutorial E: Saddle Bracket

Book	Shih, Parametric Modeling with Siemens NX, ch. 4
You learn	Datum CSYS first (BORN), Symmetric extrude, Project Curve, renaming in the Part Navigator, Edit Parameters, Assign Material, Measure Bodies
Sizes	The text gives 63.5, 12.7, 50.8, Ø19.05 and R6.35 mm (2.5, 0.5, 2.0, Ø0.75 and R0.25 in). The L profile is in figures only, so it is this project’s own: 76.2 mm long, a 12.7 mm base, a 19.05 × 50.8 mm upright, a 25.4 × 19.05 mm notch.

The Saddle Bracket after the design changes

In short

Datum CSYS first; FreeCAD asks whether to continue without an attachment; a Body has its own origin anyway.
The L profile, extruded Symmetric 63.5 mm (the value is the total width, as in NX since NX 1926).
A circular end tied to a projected edge.
F2 in the Part Navigator to name the features.
Three design changes: the width 63.5 → 50.8 mm, Until Next → Through All, and a fillet added to the first sketch.
Render › Material › Assign Material: steel. Analysis › Measure › Measure Bodies: 86,504.5 mm³, 7900 kg/m³, 0.6834 kg.

Step by step

#	In the book (NX)	In FreeCAD NX-Style	Result	Notes
E1	File > New	Ctrl+N	same
E2	BORN: Datum CSYS at the WCS, OK	ribbon 'Home > Datum > Datum CSYS', MB2 = OK, Yes to FreeCAD’s question	differs	a FreeCAD Body already starts with its own origin (the BORN idea built in). With nothing selected FreeCAD asks 'no attachment mode fits the references, continue?'; NX places the CSYS at the WCS without asking
E3	Extrude (X), XZ plane, OK	X key, plane row + MB2	same	picked XZ-plane (Base plane)
E4	Profile (Z): the L-shaped outline, MB2	Z key + 7 MB1 clicks + MB2; sizes applied	same	tool True; 6 curves; ended True
E5	Start = Symmetric Value, distance 2.5, OK	'Symmetric', 'lengthEdit' = 63.5 mm, MB2 = OK	same	volume 107540.1 mm^3, expected 107540.1; 1 solid(s); width -31.75 .. 31.75 mm (NX 1926+ and FreeCAD both treat the symmetric distance as the total)
E6	Extrude, bottom face as the sketch plane	select face + ribbon 'Home › Feature > Extrude'	same	Face1
E7	Project Curve: the bottom right edge, OK	ribbon 'Project Curve' + MB1 on the edge + MB2	same	picked Edge2 in the graphics window
E8	Circle: centre at the edge midpoint, through the top corner	O key + 2 MB1 clicks + MB2; midpoint and corner as constraints	same	solver result 0 (0 = solved); NX snaps to the midpoint and corner while drawing, FreeCAD records them as constraints
E9	Finish the section: circle and projected edge	select the projected line + ribbon 'Convert To/From Reference'	differs	FreeCAD 1.1 projects a picked edge as defining geometry, so the profile had 2 curves and Extrude would report 'Wire is not closed'. NX builds regions from the circle and its diameter; in FreeCAD the projected line has to become construction geometry first
E10	Reverse Direction, distance 0.5, Boolean Unite, OK	'checkBoxReversed' on, 'lengthEdit' = 12.7 mm, MB2 = OK	same	volume 127650.1 mm^3, expected 127650.1; 1 solid(s); lowest point z = -0.00 mm
E11	Rename in the Part Navigator: Base, Circular_End	select + F2, type, Enter	differs	NX: click the name twice or MB3 > Rename; FreeCAD: F2 or MB3 > Rename
E12	Design change: Base distance 2.5 → 2.0, OK, F5	Base selected + ribbon 'Home › Edit Feature > Edit Parameters' (dialog True), 'lengthEdit' = 50.8 mm, MB2 = OK, F5	same	volume 98902.5 mm^3, expected 98902.5; 1 solid(s); NX edits the value from MB3 > Show Dimensions, FreeCAD reopens the Extrude dialog. Circular_End follows the narrower base (its circle is tied to the projected edge)
E13	Hole: Simple, Normal to Face, on the top face	select face + ribbon 'Home › Feature > Hole'	differs	FreeCAD’s Hole drills at circle centres in a sketch on the face
E14	Point: the centre of the top arc	O key + MB1 clicks + MB2; centre tied to the arc	differs	NX picks the arc centre directly; FreeCAD sketches a circle on it (Edge19 projected)
E15	Diameter 0.75, Depth Limit = Through Body, OK	'Diameter' = 19.05 mm, 'Through all', MB2 = OK	same	volume 95282.7 mm^3, expected 95282.7; 1 solid(s)
E16	Extrude on the right vertical face of the upright	select face + ribbon 'Home › Feature > Extrude (Subtract)'	differs	Face5; the button starts Extrude with Boolean Subtract chosen
E17	Rectangle at the upper edge, MB2; three dimensions	R key + 2 MB1 clicks + MB2; sizes applied	same	tool True; 4 curves; ended True
E18	Boolean Subtract, End = Until Next, OK	'To first', MB2 = OK	same	volume 86064.9 mm^3, expected 86064.9; 1 solid(s); FreeCAD calls Until Next 'To first'
E19	Rename the cut Rect_Cut	select + F2, type, Enter	differs
E20	Edit with Rollback: End = Through All, OK	Rect_Cut selected + ribbon 'Home › Edit Feature > Edit Parameters', 'Through all', MB2 = OK	same	volume 86064.9 mm^3, expected 86064.9; 1 solid(s); FreeCAD’s edit shows the model before the feature, like NX’s rollback
E21	Edit the Base sketch: Fillet (F) R0.25 on the inside corner, MB2	sketch selected + ribbon 'Edit Parameters', F key; corner filleted at 0.25	differs	NX: Edit with Rollback > Sketch Section; FreeCAD opens the sketch directly. The radius is typed after picking the corner
E22	Finish Sketch, OK: the whole part updates	Ctrl+Q	same	volume 86504.5 mm^3, expected 86504.5; 1 solid(s); later features (Circular_End, hole, Rect_Cut) follow the edited sketch
E23	Tools > Assign Materials: Steel, select the body, OK	body selected + ribbon 'View › Visualization > Assign Material', 'Steel-Generic', Close	differs	material Steel-Generic, density 7900.0 kg/m^3; the panel applies the choice at once and has Close instead of OK
E24	Analysis > Measure, Solid Body, physical properties in the Information window	body selected + ribbon 'Analysis › Measure > Measure Bodies'	differs	mass 0.6834 kg from 7900 kg/m^3; FreeCAD’s own Measure has no mass, so NXStyle adds Measure Bodies
E25	The finished part is shown in the graphics window	render of the graphics window	same	21.7% 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

same

BORN: Datum CSYS at the WCS, OK

ribbon 'Home > Datum > Datum CSYS', MB2 = OK, Yes to FreeCAD’s question

differs

a FreeCAD Body already starts with its own origin (the BORN idea built in). With nothing selected FreeCAD asks 'no attachment mode fits the references, continue?'; NX places the CSYS at the WCS without asking

Extrude (X), XZ plane, OK

X key, plane row + MB2

same

picked XZ-plane (Base plane)

Profile (Z): the L-shaped outline, MB2

Z key + 7 MB1 clicks + MB2; sizes applied

same

tool True; 6 curves; ended True

Start = Symmetric Value, distance 2.5, OK

'Symmetric', 'lengthEdit' = 63.5 mm, MB2 = OK

same

volume 107540.1 mm^3, expected 107540.1; 1 solid(s); width -31.75 .. 31.75 mm (NX 1926+ and FreeCAD both treat the symmetric distance as the total)

Extrude, bottom face as the sketch plane

select face + ribbon 'Home › Feature > Extrude'

same

Face1

Project Curve: the bottom right edge, OK

ribbon 'Project Curve' + MB1 on the edge + MB2

same

picked Edge2 in the graphics window

Circle: centre at the edge midpoint, through the top corner

O key + 2 MB1 clicks + MB2; midpoint and corner as constraints

same

solver result 0 (0 = solved); NX snaps to the midpoint and corner while drawing, FreeCAD records them as constraints

Finish the section: circle and projected edge

select the projected line + ribbon 'Convert To/From Reference'

differs

FreeCAD 1.1 projects a picked edge as defining geometry, so the profile had 2 curves and Extrude would report 'Wire is not closed'. NX builds regions from the circle and its diameter; in FreeCAD the projected line has to become construction geometry first

E10

Reverse Direction, distance 0.5, Boolean Unite, OK

'checkBoxReversed' on, 'lengthEdit' = 12.7 mm, MB2 = OK

same

volume 127650.1 mm^3, expected 127650.1; 1 solid(s); lowest point z = -0.00 mm

E11

Rename in the Part Navigator: Base, Circular_End

select + F2, type, Enter

differs

NX: click the name twice or MB3 > Rename; FreeCAD: F2 or MB3 > Rename

E12

Design change: Base distance 2.5 → 2.0, OK, F5

Base selected + ribbon 'Home › Edit Feature > Edit Parameters' (dialog True), 'lengthEdit' = 50.8 mm, MB2 = OK, F5

same

volume 98902.5 mm^3, expected 98902.5; 1 solid(s); NX edits the value from MB3 > Show Dimensions, FreeCAD reopens the Extrude dialog. Circular_End follows the narrower base (its circle is tied to the projected edge)

E13

Hole: Simple, Normal to Face, on the top face

select face + ribbon 'Home › Feature > Hole'

differs

FreeCAD’s Hole drills at circle centres in a sketch on the face

E14

Point: the centre of the top arc

O key + MB1 clicks + MB2; centre tied to the arc

differs

NX picks the arc centre directly; FreeCAD sketches a circle on it (Edge19 projected)

E15

Diameter 0.75, Depth Limit = Through Body, OK

'Diameter' = 19.05 mm, 'Through all', MB2 = OK

same

volume 95282.7 mm^3, expected 95282.7; 1 solid(s)

E16

Extrude on the right vertical face of the upright

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

differs

Face5; the button starts Extrude with Boolean Subtract chosen

E17

Rectangle at the upper edge, MB2; three dimensions

R key + 2 MB1 clicks + MB2; sizes applied

same

tool True; 4 curves; ended True

E18

Boolean Subtract, End = Until Next, OK

'To first', MB2 = OK

same

volume 86064.9 mm^3, expected 86064.9; 1 solid(s); FreeCAD calls Until Next 'To first'

E19

Rename the cut Rect_Cut

select + F2, type, Enter

differs

E20

Edit with Rollback: End = Through All, OK

Rect_Cut selected + ribbon 'Home › Edit Feature > Edit Parameters', 'Through all', MB2 = OK

same

volume 86064.9 mm^3, expected 86064.9; 1 solid(s); FreeCAD’s edit shows the model before the feature, like NX’s rollback

E21

Edit the Base sketch: Fillet (F) R0.25 on the inside corner, MB2

sketch selected + ribbon 'Edit Parameters', F key; corner filleted at 0.25

differs

NX: Edit with Rollback > Sketch Section; FreeCAD opens the sketch directly. The radius is typed after picking the corner

E22

Finish Sketch, OK: the whole part updates

Ctrl+Q

same

volume 86504.5 mm^3, expected 86504.5; 1 solid(s); later features (Circular_End, hole, Rect_Cut) follow the edited sketch

E23

Tools > Assign Materials: Steel, select the body, OK

body selected + ribbon 'View › Visualization > Assign Material', 'Steel-Generic', Close

differs

material Steel-Generic, density 7900.0 kg/m^3; the panel applies the choice at once and has Close instead of OK

E24

Analysis > Measure, Solid Body, physical properties in the Information window

body selected + ribbon 'Analysis › Measure > Measure Bodies'

differs

mass 0.6834 kg from 7900 kg/m^3; FreeCAD’s own Measure has no mass, so NXStyle adds Measure Bodies

E25

The finished part is shown in the graphics window

render of the graphics window

same

21.7% 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

Design changes reopen the feature’s dialog (Edit Parameters) instead of editing a dimension shown in the graphics window.
Assign Material applies at once and closes with Close; FreeCAD 1.1 also gives the body the material’s colour.
FreeCAD’s own Measure has no mass; Measure Bodies is NX-Style’s.