Tutorial N: The U-Bracket drawing

Book	Shih, Parametric Modeling with Siemens NX, ch. 8 (after Tutorial M)
You learn	Sheet size and projection, view styles, smooth edges, dimension settings, Hide and Show, center marks, associativity
Sizes	Tutorial M’s bracket; the hole changes from Ø19.05 to Ø15.875 mm (the book’s Ø0.750 → Ø0.625 in).

The U-Bracket drawing on a B sheet: front

In short

Ctrl+Shift+D, New Sheet: template ANSI A, Third angle; later swapped for ANSI B.
Base View front, with hidden lines; a second Base View from the top, lined up above it; an isometric one.
Reference dimensions on the top view; Smooth Visible off on the isometric view; FlipArrowheads on the diameter.
Ctrl+B hides two dimensions; select them in the Part Navigator and Ctrl+Shift+K shows them.
Center Mark on the arcs; a Radial dimension; two decimals with Format Spec %.2f.
Ctrl+M: the hole to Ø15.875; Ctrl+Shift+D: the drawing has followed.

Step by step

#	In the book (NX)	In FreeCAD NX-Style	Result	Notes
N1	File > Drafting	Ctrl+Shift+D	same	TechDrawWorkbench
N2	Sheet: Inches, Third Angle, A-8.5X11, scale 1:1, OK	ribbon 'Home › Drawing > New Sheet'; the sheet’s template, projection and scale	differs	template ANSIA_Landscape.svg, projection Third angle. NX asks in one Sheet dialog; FreeCAD’s New Sheet uses the default template, and size, projection and scale are the sheet’s properties. Units follow the preferences (mm here)
N3	Base View: Front; View Style: hidden lines dashed 0.35, visible lines 0.70; place it low on the sheet	body selected + ribbon 'Home › View > Base View', MB2; the view’s style properties	differs	16 visible, 34 hidden edges. NX sets the style in the view’s Settings dialog; TechDraw has Hard Hidden and the line widths in the view’s properties
N4	Projected Top view above the Front view	a second Base View, direction Top, aligned above	differs	as in tutorials D and H: NX drags projected views off the base view; FreeCAD’s Projected View is a projection group, so a Base View looking down stands in, lined up with the front view
N5	MB3 > Edit Sheet: B-11X17	the sheet’s template set to ANSI B	differs	template ANSIB_Landscape.svg; the views keep their places. NX changes the size in Edit Sheet; FreeCAD swaps the template
N6	Base View: Isometric, to the right	body selected + ribbon 'Home › View > Base View', isometric direction	same
N7	Hide the Datum Coordinate System and the view’s cross hair	-	same	nothing to hide: TechDraw draws only the solid, and NXStyle keeps the Body’s origin hidden (origin shown: False)
N8	Drafting Preferences: dimension text Horizontal (ANSI)	Preferences > TechDraw > Dimensions > Standard and Style = ASME Inlined	differs	was ASME Inlined
N9	Command Finder > Feature Parameters: the model’s dimensions on the views	-	missing	TechDraw has no command that brings a feature’s sketch dimensions onto a view; its dimensions are reference dimensions measured from the view (next steps). NX’s feature dimensions also drive the model from the drawing
N10	Instead: reference dimensions on the top view (5.000, 2.500, Ø0.750 in)	cosmetic vertices on the hole centres; ribbon 'Horizontal' (twice) and 'Diameter'	differs	measured (mm): {'centres': 127.0, 'to the middle': 63.5, 'hole': 19.05}, the book’s 127.00, 63.50 and Ø19.05. TechDraw dimensions need vertices at arc centres (as in tutorial H)
N11	Isometric view: Settings > Smooth Edges off	the view’s Smooth Visible property	same	smooth (tangent) edges were shown, as in NX, and are now off
N12	Edit the diameter dimension: Arrow Out	the dimension’s 'FlipArrowheads' property	differs	arrow properties: ['ArrowStyle', 'Arrowsize', 'FlipArrowheads']
N13	Immediate Hide: the two dimensions in the top view	both selected + Ctrl+B (Hide)	same	hidden [True, True]
N14	Show (Ctrl+Shift+K): the two dimensions back	selected in the Part Navigator + Ctrl+Shift+K	same	shown [True, True]; NX picks hidden objects in a list, here they are picked in the Part Navigator
N15	Center Mark: the two outer arcs and the drill in the top view	3 arcs selected + ribbon 'Home › Centerline and Hatch > Center Mark'	same	center lines 0 → 0, cosmetic edges 0 → 6; the book deletes NX’s automatic centre lines first: TechDraw adds none by itself
N16	Radial dimension on the bottom arc of the front view	arc selected + ribbon 'Home › Dimension > Radial'	same	R31.75 mm (the book’s R1.250 in)
N17	Edit Settings: the 5 and 2.5 dimensions with 2 decimals and trailing zeros	the dimensions' Format Spec = %.2f	differs	NX: Edit Settings > Text > decimals; TechDraw: the format spec (shown in the preferences units)
N18	Modeling: Base feature > Sketch Section, the diameter 0.750 → 0.625, Finish Sketch, OK	Ctrl+M; the base sketch’s diameter typed (0.625 in = 15.875 mm)	same	volume 142208.8 mm^3 (expected 142209.3)
N19	Drafting: MB3 on the drawing > Update; the diameter shows 0.625 in	Ctrl+Shift+D; the sheet updates by itself	same	diameter dimension now Ø15.875 mm; TechDraw keeps the sheet up to date (the page’s Keep Updated), NX marks it out of date and asks for Update

In the book (NX)

In FreeCAD NX-Style

Result

Notes

File > Drafting

Ctrl+Shift+D

same

TechDrawWorkbench

Sheet: Inches, Third Angle, A-8.5X11, scale 1:1, OK

ribbon 'Home › Drawing > New Sheet'; the sheet’s template, projection and scale

differs

template ANSIA_Landscape.svg, projection Third angle. NX asks in one Sheet dialog; FreeCAD’s New Sheet uses the default template, and size, projection and scale are the sheet’s properties. Units follow the preferences (mm here)

Base View: Front; View Style: hidden lines dashed 0.35, visible lines 0.70; place it low on the sheet

body selected + ribbon 'Home › View > Base View', MB2; the view’s style properties

differs

16 visible, 34 hidden edges. NX sets the style in the view’s Settings dialog; TechDraw has Hard Hidden and the line widths in the view’s properties

Projected Top view above the Front view

a second Base View, direction Top, aligned above

differs

as in tutorials D and H: NX drags projected views off the base view; FreeCAD’s Projected View is a projection group, so a Base View looking down stands in, lined up with the front view

MB3 > Edit Sheet: B-11X17

the sheet’s template set to ANSI B

differs

template ANSIB_Landscape.svg; the views keep their places. NX changes the size in Edit Sheet; FreeCAD swaps the template

Base View: Isometric, to the right

body selected + ribbon 'Home › View > Base View', isometric direction

same

Hide the Datum Coordinate System and the view’s cross hair

same

nothing to hide: TechDraw draws only the solid, and NXStyle keeps the Body’s origin hidden (origin shown: False)

Drafting Preferences: dimension text Horizontal (ANSI)

Preferences > TechDraw > Dimensions > Standard and Style = ASME Inlined

differs

was ASME Inlined

Command Finder > Feature Parameters: the model’s dimensions on the views

missing

TechDraw has no command that brings a feature’s sketch dimensions onto a view; its dimensions are reference dimensions measured from the view (next steps). NX’s feature dimensions also drive the model from the drawing

N10

Instead: reference dimensions on the top view (5.000, 2.500, Ø0.750 in)

cosmetic vertices on the hole centres; ribbon 'Horizontal' (twice) and 'Diameter'

differs

measured (mm): {'centres': 127.0, 'to the middle': 63.5, 'hole': 19.05}, the book’s 127.00, 63.50 and Ø19.05. TechDraw dimensions need vertices at arc centres (as in tutorial H)

N11

Isometric view: Settings > Smooth Edges off

the view’s Smooth Visible property

same

smooth (tangent) edges were shown, as in NX, and are now off

N12

Edit the diameter dimension: Arrow Out

the dimension’s 'FlipArrowheads' property

differs

arrow properties: ['ArrowStyle', 'Arrowsize', 'FlipArrowheads']

N13

Immediate Hide: the two dimensions in the top view

both selected + Ctrl+B (Hide)

same

hidden [True, True]

N14

Show (Ctrl+Shift+K): the two dimensions back

selected in the Part Navigator + Ctrl+Shift+K

same

shown [True, True]; NX picks hidden objects in a list, here they are picked in the Part Navigator

N15

Center Mark: the two outer arcs and the drill in the top view

3 arcs selected + ribbon 'Home › Centerline and Hatch > Center Mark'

same

center lines 0 → 0, cosmetic edges 0 → 6; the book deletes NX’s automatic centre lines first: TechDraw adds none by itself

N16

Radial dimension on the bottom arc of the front view

arc selected + ribbon 'Home › Dimension > Radial'

same

R31.75 mm (the book’s R1.250 in)

N17

Edit Settings: the 5 and 2.5 dimensions with 2 decimals and trailing zeros

the dimensions' Format Spec = %.2f

differs

NX: Edit Settings > Text > decimals; TechDraw: the format spec (shown in the preferences units)

N18

Modeling: Base feature > Sketch Section, the diameter 0.750 → 0.625, Finish Sketch, OK

Ctrl+M; the base sketch’s diameter typed (0.625 in = 15.875 mm)

same

volume 142208.8 mm^3 (expected 142209.3)

N19

Drafting: MB3 on the drawing > Update; the diameter shows 0.625 in

Ctrl+Shift+D; the sheet updates by itself

same

diameter dimension now Ø15.875 mm; TechDraw keeps the sheet up to date (the page’s Keep Updated), NX marks it out of date and asks for Update

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

Size, projection and scale are the sheet’s template and properties, not a Sheet dialog.
TechDraw has no Feature Parameters: reference dimensions measured from the view stand in; they follow the model but do not drive it.
The sheet updates by itself; NX marks it out of date and asks for Update.