Tutorial I: The Gasket

Book	Shih, Parametric Modeling with Siemens NX, ch. 6 (a millimetre part)
You learn	Quick Extend, Quick Trim, sketch Fillet, fully defining a sketch, Project Curve, Offset Curve, a design change the offset follows
Sizes	R20 fillets, a 5 mm plate, a 15 mm offset, the height changed to 150 mm. The outline’s sizes are in figures only: an 80 mm left side and an R30 boss here.

In short

An outline, a circle and a line tangent to it; E (Extend) and T (Quick Trim).
The book’s dimensions until the solver says Fully constrained.
F (Fillet) R20; add the R20 dimensions.
Extrude 5 mm.
On the front face: Project Curve, Offset Curve 15 mm inwards, Extrude (Subtract) through all with only the inner loop.
The design change: the overall height to 150 mm; the offset follows.

Step by step

#	In the book (NX)	In FreeCAD NX-Style	Result	Notes
I1	File > New, Model template, millimetres	Ctrl+N	same
I2	Extrude (X), YZ plane	X key, plane row + MB2	same	picked YZ-plane (Base plane)
I3	Profile (outline), Circle, Line ending on the bottom line, tangent to the circle	Z key + 4 MB1 clicks, O key + 2 clicks, L key + 2 clicks, MB2 after each	same	geometry ['GeomCircle', 'GeomLineSegment', 'GeomLineSegment', 'GeomLineSegment', 'GeomLineSegment']; tangent picked up while drawing True
I4	Extend: the top line up to the circle, MB2	E key, MB1 near the line’s end, MB1 on the circle, MB2	same	line now ends at x = 94.949 (meets the circle at 94.953)
I5	Quick Trim: the bottom line past the slanted line, the lower part of the circle, MB2	T key, MB1 on each part to remove, MB2	same	bottom line now ends at x = 88.798 (slanted line at 88.798); 1 arc, 0 full circle; outline closed True; geometry 5 → 5
I6	The book’s dimensions: centre in line with the top line (0.0), its horizontal location, the radius, the corner on the origin; horizontal/vertical constraints confirmed; fully defined	constraints: centre on the top line, radius, horizontal location of the centre, height of the centre, angle of the slanted line; H/V: Vertical 1 implied, Horizontal 2	same	centre -1.287 → -0.000 mm from the top line; outline closed True; solver: 'Fully constrained' (0 DoF). NX sets a 0.0 location dimension; FreeCAD has a point-on-object constraint for it; implied already: left edge on the origin, bottom edge on the origin
I7	Fillet R20 at the corners	F key; radius 20 at each corner where two curves meet at an angle	differs	4 fillets of 4 corners 95, 78), (0, 78), (0, 0), (89, 0; outline closed True; constraints re-confirmed after the fillets: Vertical 1, left edge on the origin, bottom edge on the origin; 4 R20 dimensions added (FreeCAD’s sketch fillet constrains tangency, not the radius); solver 'Fully constrained' (0 DoF). The book makes five, the arc-to-slanted-line join being tangent here leaves four; the radius is typed after picking in FreeCAD
I8	Finish Sketch, End 5 mm, OK	Ctrl+Q, 'lengthEdit' = 5 mm, MB2 = OK	same	volume 56106.6 mm^3, expected 56106.6; 1 solid(s); outline area 11221.3 mm^2
I9	Extrude, Sketch Section on the front face	select Face11 + ribbon 'Home › Feature > Extrude (Subtract)'	differs	subtracting extrude is its own button
I10	Project Curve (the whole face), Offset 15 mm, Reverse Direction to the inside, OK	9 edges projected; ribbon 'Sketch › Edit Curve > Offset Curve', 'Add offset constraint', MB1 15 mm inside; Select Redundant Constraints + Delete; offset dimension typed 15	differs	9 projected curves, 9 offset curves; the click gave 14.802 mm. FreeCAD’s own offset constraints left the sketch unsolvable (solver: 'Redundant constraints:'; selected ['Constraint17']); after deleting it the sketch solves (True). NX types the distance and flips the side with Reverse Direction; FreeCAD takes the side and distance from the click, the exact value from its offset dimension
I11	Offset loop: 15 mm inside the outline; only the inside loop is the section	measured in the sketch; profile edges 9, offset curves 9: the projected outline is reference geometry, as the book selects only the inside loop	same	closed True; nearest distance to the projected outline 15.0 mm
I12	Boolean Subtract, Reverse Direction, Through All, inner loop only, OK	'Through all', MB2 = OK	same	volume 29310.1 mm^3, expected 29310.1; 1 solid(s); the projected outline is reference geometry here, so only the inner loop cuts
I13	Change the overall height to 150 mm: the offset follows	the centre’s height dimension: 78.39 → 119.99 (+ R30.01 = 150)	same	overall height 108.398 → 150.0000 mm; inner loop 15.0 mm inside the outline
I14	The part is shown in the graphics window	render of the graphics window	same	5.2% of the view shows the part

In the book (NX)

In FreeCAD NX-Style

Result

Notes

File > New, Model template, millimetres

Ctrl+N

same

Extrude (X), YZ plane

X key, plane row + MB2

same

picked YZ-plane (Base plane)

Profile (outline), Circle, Line ending on the bottom line, tangent to the circle

Z key + 4 MB1 clicks, O key + 2 clicks, L key + 2 clicks, MB2 after each

same

geometry ['GeomCircle', 'GeomLineSegment', 'GeomLineSegment', 'GeomLineSegment', 'GeomLineSegment']; tangent picked up while drawing True

Extend: the top line up to the circle, MB2

E key, MB1 near the line’s end, MB1 on the circle, MB2

same

line now ends at x = 94.949 (meets the circle at 94.953)

Quick Trim: the bottom line past the slanted line, the lower part of the circle, MB2

T key, MB1 on each part to remove, MB2

same

bottom line now ends at x = 88.798 (slanted line at 88.798); 1 arc, 0 full circle; outline closed True; geometry 5 → 5

The book’s dimensions: centre in line with the top line (0.0), its horizontal location, the radius, the corner on the origin; horizontal/vertical constraints confirmed; fully defined

constraints: centre on the top line, radius, horizontal location of the centre, height of the centre, angle of the slanted line; H/V: Vertical 1 implied, Horizontal 2

same

centre -1.287 → -0.000 mm from the top line; outline closed True; solver: 'Fully constrained' (0 DoF). NX sets a 0.0 location dimension; FreeCAD has a point-on-object constraint for it; implied already: left edge on the origin, bottom edge on the origin

Fillet R20 at the corners

F key; radius 20 at each corner where two curves meet at an angle

differs

4 fillets of 4 corners 95, 78), (0, 78), (0, 0), (89, 0; outline closed True; constraints re-confirmed after the fillets: Vertical 1, left edge on the origin, bottom edge on the origin; 4 R20 dimensions added (FreeCAD’s sketch fillet constrains tangency, not the radius); solver 'Fully constrained' (0 DoF). The book makes five, the arc-to-slanted-line join being tangent here leaves four; the radius is typed after picking in FreeCAD

Finish Sketch, End 5 mm, OK

Ctrl+Q, 'lengthEdit' = 5 mm, MB2 = OK

same

volume 56106.6 mm^3, expected 56106.6; 1 solid(s); outline area 11221.3 mm^2

Extrude, Sketch Section on the front face

select Face11 + ribbon 'Home › Feature > Extrude (Subtract)'

differs

subtracting extrude is its own button

I10

Project Curve (the whole face), Offset 15 mm, Reverse Direction to the inside, OK

9 edges projected; ribbon 'Sketch › Edit Curve > Offset Curve', 'Add offset constraint', MB1 15 mm inside; Select Redundant Constraints + Delete; offset dimension typed 15

differs

9 projected curves, 9 offset curves; the click gave 14.802 mm. FreeCAD’s own offset constraints left the sketch unsolvable (solver: 'Redundant constraints:'; selected ['Constraint17']); after deleting it the sketch solves (True). NX types the distance and flips the side with Reverse Direction; FreeCAD takes the side and distance from the click, the exact value from its offset dimension

I11

Offset loop: 15 mm inside the outline; only the inside loop is the section

measured in the sketch; profile edges 9, offset curves 9: the projected outline is reference geometry, as the book selects only the inside loop

same

closed True; nearest distance to the projected outline 15.0 mm

I12

Boolean Subtract, Reverse Direction, Through All, inner loop only, OK

'Through all', MB2 = OK

same

volume 29310.1 mm^3, expected 29310.1; 1 solid(s); the projected outline is reference geometry here, so only the inner loop cuts

I13

Change the overall height to 150 mm: the offset follows

the centre’s height dimension: 78.39 → 119.99 (+ R30.01 = 150)

same

overall height 108.398 → 150.0000 mm; inner loop 15.0 mm inside the outline

I14

The part is shown in the graphics window

render of the graphics window

same

5.2% 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

A sketch fillet does not dimension its radius and removes the constraints that held its corner; put them back.
Offset Curve takes the side and the distance from an MB1 click; type the exact distance into its dimension afterwards.
With Add offset constraint on, FreeCAD 1.1.4 gives the closed loop one redundant constraint. Sketch › Select Redundant Constraints, then Delete (I10).