Tutorial L: The Locator

Book	Shih, Parametric Modeling with Siemens NX, ch. 3 (a millimetre part)
You learn	Unite and subtract with Extrude, Project Curve, Hole, Until Next
Sizes	A 75 × 50 × 15 mm block; an R25 boss 40 mm high; a Ø30 bore; a Ø20 hole; a 20 mm slot. The text gives every size; the hole’s and the slot’s positions are in figures: the hole 25 mm from the right edge on the slot’s centre line, the slot 15 mm from the front edge.

In short

Ctrl+N, X, XY_Plane; R, 75 × 50, Ctrl+Q, 15 mm.
The bottom face, Extrude; Project Curve on an edge; a circle through its midpoint and corner; the projected edge to reference; 40 mm.
The cylinder’s top face, Extrude (Subtract): Ø30 through all.
Hole: Ø20 through all.
The right face, Extrude (Subtract): the 20 mm slot, To first (Until Next).

Step by step

#	In the book (NX)	In FreeCAD NX-Style	Result	Notes
L1	File > New, Millimeters, Blank template, name Locator	Ctrl+N	differs	NXStyle’s New is NX’s Model template (a part with a Body to sketch on); there is no Blank template, so the part is in Modeling already; the name is given at the first save
L2	File > Applications > Modeling	ribbon 'Application › Design > Modeling'	same	application modeling; the new part stays the active one: True (Unnamed1 : 1[*])
L3	Extrude, Sketch Section, the default XY plane, OK	X key, plane row + MB2	same	picked XY-plane (Base plane)
L4	Rectangle ®: two corners, MB2	R key + 2 MB1 clicks + MB2	same	tool True; 4 curves; ended True
L5	Dimensions 75 and 50 ('scale the sketch?': Yes)	values applied	differs	DoF 0; FreeCAD has no prompt to scale the whole sketch to the first dimension; the corner is put on the origin here (the book leaves the rectangle where it was drawn)
L6	Finish Sketch, distance 15, OK	Ctrl+Q, 'lengthEdit' = 15 mm, MB2 = OK	same	volume 56250.0 mm^3, expected 56250.0; 1 solid(s)
L7	Extrude, the bottom face as the sketch plane	select Face5 + ribbon 'Home › Feature > Extrude'	same
L8	More > Project Curve: the bottom left edge, OK	ribbon 'Project Curve' + MB1 on each edge + MB2	same	1 of 1 edges picked in the graphics window
L9	Circle: centre on the edge’s midpoint, through the left corner, MB2	O key + 2 MB1 clicks + MB2; midpoint and corner as constraints	same	DoF 0; the book: no dimension needed, the circle is defined by the midpoint and the corner. NX snaps while drawing, FreeCAD records the same as constraints
L10	(FreeCAD) the projected edge to reference	ribbon 'Convert To/From Reference'	differs	profile edges 2 → 1. FreeCAD 1.1 projects a picked edge as defining geometry, which would leave an open wire; NX makes regions
L11	End 40, Boolean Unite, Flip (upward), OK	'lengthEdit' = 40 mm, 'checkBoxReversed' on, MB2 = OK	same	volume 120063.6 mm^3, expected 120063.6; 1 solid(s); height 0.0 .. 40.0 mm. Features in a Body unite by themselves (no Boolean option)
L12	Extrude, the top face of the cylinder	select Face6 + ribbon 'Home › Feature > Extrude (Subtract)'	differs	the subtracting extrude is its own button
L13	Circle on the sketch origin, MB2; diameter 30	O key + 2 MB1 clicks + MB2; diameter applied	differs	centre tied to the cylinder’s edge (Edge10): the sketch origin is not at the centre; DoF 0
L14	Boolean Subtract, Through All, Flip (downward), OK	'Through all', MB2 = OK	same	volume 91789.3 mm^3, expected 91789.3; 1 solid(s); FreeCAD’s subtracting extrude goes into the part without a flip
L15	Hole (a placed feature): Simple, a point on the base’s top face	select Face5 + ribbon 'Home › Feature > Hole'	differs	FreeCAD’s Hole drills at circle centres in a sketch on the face: not placed without a sketch
L16	Location dimensions 25 and 30	O key + 2 MB1 clicks + MB2; centre placed by values	differs	centre at (50, 25): 25 from the right edge, on the slot’s centre line. NX adds the two location dimensions by itself
L17	Diameter 20, Depth Limit = Through Body, OK	'Diameter' = 20 mm, 'Through all', MB2 = OK	same	volume 87076.9 mm^3, expected 87076.9; 1 solid(s)
L18	Extrude, the right vertical face of the base	select Face3 + ribbon 'Home › Feature > Extrude (Subtract)'	differs
L19	More > Project Curve: the top and bottom edges, OK	ribbon 'Project Curve' + MB1 on each edge + MB2	same	2 of 2 edges picked in the graphics window
L20	Rectangle aligned to the top and bottom edges; dimensions 15 and 20	R key + 2 MB1 clicks + MB2; on the projected edges; values applied	same	15 from the front edge, 20 wide, full height; DoF 12
L21	(FreeCAD) the projected edges to reference	ribbon 'Convert To/From Reference'	differs	profile edges 6 → 4
L22	Subtract, End = Until Next (into the hole), OK	'To first' (FreeCAD’s Until Next), MB2 = OK	limit	removed 300.0 mm^3 of the 5143.8 the slot holds: FreeCAD 1.1.4’s 'To first' stops 1 mm into the part instead of at the hole’s wall (measured headless too, the same with 'Up to face' on the hole’s face); NX stops at the next face. Workaround next
L23	Workaround: the slot’s depth = 25 (to the hole’s axis)	slot selected + ribbon 'Home › Edit Feature > Edit Parameters', 'Dimension', 'lengthEdit' = 25 mm, MB2 = OK	same	volume 81933.1 mm^3, expected 81933.1; 1 solid(s); the same part as NX’s Until Next here, because the slot is as wide as the hole and on its centre line
L24	The finished Locator is shown in the graphics window	render of the graphics window	same	22.5% of the view shows the part

In the book (NX)

In FreeCAD NX-Style

Result

Notes

File > New, Millimeters, Blank template, name Locator

Ctrl+N

differs

NXStyle’s New is NX’s Model template (a part with a Body to sketch on); there is no Blank template, so the part is in Modeling already; the name is given at the first save

File > Applications > Modeling

ribbon 'Application › Design > Modeling'

same

application modeling; the new part stays the active one: True (Unnamed1 : 1[*])

Extrude, Sketch Section, the default XY plane, OK

X key, plane row + MB2

same

picked XY-plane (Base plane)

Rectangle ®: two corners, MB2

R key + 2 MB1 clicks + MB2

same

tool True; 4 curves; ended True

Dimensions 75 and 50 ('scale the sketch?': Yes)

values applied

differs

DoF 0; FreeCAD has no prompt to scale the whole sketch to the first dimension; the corner is put on the origin here (the book leaves the rectangle where it was drawn)

Finish Sketch, distance 15, OK

Ctrl+Q, 'lengthEdit' = 15 mm, MB2 = OK

same

volume 56250.0 mm^3, expected 56250.0; 1 solid(s)

Extrude, the bottom face as the sketch plane

select Face5 + ribbon 'Home › Feature > Extrude'

same

More > Project Curve: the bottom left edge, OK

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

same

1 of 1 edges picked in the graphics window

Circle: centre on the edge’s midpoint, through the left corner, MB2

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

same

DoF 0; the book: no dimension needed, the circle is defined by the midpoint and the corner. NX snaps while drawing, FreeCAD records the same as constraints

L10

(FreeCAD) the projected edge to reference

ribbon 'Convert To/From Reference'

differs

profile edges 2 → 1. FreeCAD 1.1 projects a picked edge as defining geometry, which would leave an open wire; NX makes regions

L11

End 40, Boolean Unite, Flip (upward), OK

'lengthEdit' = 40 mm, 'checkBoxReversed' on, MB2 = OK

same

volume 120063.6 mm^3, expected 120063.6; 1 solid(s); height 0.0 .. 40.0 mm. Features in a Body unite by themselves (no Boolean option)

L12

Extrude, the top face of the cylinder

select Face6 + ribbon 'Home › Feature > Extrude (Subtract)'

differs

the subtracting extrude is its own button

L13

Circle on the sketch origin, MB2; diameter 30

O key + 2 MB1 clicks + MB2; diameter applied

differs

centre tied to the cylinder’s edge (Edge10): the sketch origin is not at the centre; DoF 0

L14

Boolean Subtract, Through All, Flip (downward), OK

'Through all', MB2 = OK

same

volume 91789.3 mm^3, expected 91789.3; 1 solid(s); FreeCAD’s subtracting extrude goes into the part without a flip

L15

Hole (a placed feature): Simple, a point on the base’s top face

select Face5 + ribbon 'Home › Feature > Hole'

differs

FreeCAD’s Hole drills at circle centres in a sketch on the face: not placed without a sketch

L16

Location dimensions 25 and 30

O key + 2 MB1 clicks + MB2; centre placed by values

differs

centre at (50, 25): 25 from the right edge, on the slot’s centre line. NX adds the two location dimensions by itself

L17

Diameter 20, Depth Limit = Through Body, OK

'Diameter' = 20 mm, 'Through all', MB2 = OK

same

volume 87076.9 mm^3, expected 87076.9; 1 solid(s)

L18

Extrude, the right vertical face of the base

select Face3 + ribbon 'Home › Feature > Extrude (Subtract)'

differs

L19

More > Project Curve: the top and bottom edges, OK

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

same

2 of 2 edges picked in the graphics window

L20

Rectangle aligned to the top and bottom edges; dimensions 15 and 20

R key + 2 MB1 clicks + MB2; on the projected edges; values applied

same

15 from the front edge, 20 wide, full height; DoF 12

L21

(FreeCAD) the projected edges to reference

ribbon 'Convert To/From Reference'

differs

profile edges 6 → 4

L22

Subtract, End = Until Next (into the hole), OK

'To first' (FreeCAD’s Until Next), MB2 = OK

limit

removed 300.0 mm^3 of the 5143.8 the slot holds: FreeCAD 1.1.4’s 'To first' stops 1 mm into the part instead of at the hole’s wall (measured headless too, the same with 'Up to face' on the hole’s face); NX stops at the next face. Workaround next

L23

Workaround: the slot’s depth = 25 (to the hole’s axis)

slot selected + ribbon 'Home › Edit Feature > Edit Parameters', 'Dimension', 'lengthEdit' = 25 mm, MB2 = OK

same

volume 81933.1 mm^3, expected 81933.1; 1 solid(s); the same part as NX’s Until Next here, because the slot is as wide as the hole and on its centre line

L24

The finished Locator is shown in the graphics window

render of the graphics window

same

22.5% 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

NX-Style’s New is already the Model template; there is no Blank template to switch from.
A projected edge is defining geometry: turn it into reference geometry before extruding.
Hole drills at circle centres in a sketch; NX adds the location dimensions itself.
To first into the hole stops 1 mm into the part in FreeCAD 1.1.4 (L22); the workaround is a 25 mm depth, to the hole’s axis (L23).