Tutorial J: Parametric constraints and relations

Book	Shih, Parametric Modeling with Siemens NX, ch. 5
You learn	Geometric constraints, degrees of freedom, Fix and Relax, dimension names and formulas
Sizes	An 88.9 mm (3.5 in) plate. The triangle’s own sizes are in figures only.

The triangle plate after the 25 × 20 size change; the hole follows its formulas

In short

A triangle; Perpendicular, a length and an angle; Fully Fixed; undo and Coincident instead; location dimensions; Relax Constraint on Perpendicular; Vertical; a tangent circle.
At every step, FreeCAD’s Under-constrained: N Degrees of Freedom or Fully constrained is compared with NX’s status line. It matches the book’s state each time.
Extrude the plate.
Name the dimensions and drive them with the book’s formulas after =, for example =Constraints.width / 5 * 1.6; the hole is a third of the height.
Two size changes, 25 × 15 and 25 × 20; the hole follows.

Step by step

#	In the book (NX)	In FreeCAD NX-Style	Result	Notes
J1	File > New, Model template	Ctrl+N	same
J2	Extrude (X), YZ plane of the datum CSYS	X key, plane row + MB2	same	picked YZ-plane (Base plane)
J3	Profile: a triangle with a horizontal base	Z key + 4 MB1 clicks + MB2	same	3 lines; implicit constraints ['Coincident', 'Horizontal']; DoF 5; FreeCAD says 'Under-constrained: / 5 Degrees of Freedom'
J4	Perpendicular: the two inclined lines, OK	both lines selected + ribbon 'Sketch › Constraints > Perpendicular'	same	angle between them 90.000° (90 wanted); DoF 4; 'Under-constrained: / 4 Degrees of Freedom'
J5	Dimensions: base length, angle to the right line; the triangle still moves	line + ribbon 'Sketch › Constraints > Distance' = 120 mm, two lines + 'Angle' = 60° (typed in FreeCAD’s dimension dialog)	same	base 120.000 mm; DoF 2 (size fixed, position free, as in the book); 'Under-constrained: / 2 Degrees of Freedom'
J6	Fix Curve on one line: fully defined	line + ribbon 'Sketch › Constraints > Fully Fixed'	same	DoF 0, fully constrained True; NX turns the sketch black and says it is fully defined, FreeCAD says 'Fully constrained'
J7	Undo, then Coincident: the left corner on the sketch origin	Ctrl+Z (DoF back to 2); Vertex1 + origin + ribbon 'Sketch › Constraints > Coincident'	same	corner at (0.000, -0.000); DoF 0; 'Fully constrained'
J8	Undo, then location dimensions from the Y axis and the X axis	Ctrl+Z (DoF 2); corner + Y axis, corner + X axis, ribbon 'Sketch › Constraints > Distance', 25.4 each	same	corner at (25.400, 25.400); DoF 0; 'Fully constrained'
J9	Delete the angle, relax Perpendicular, Vertical on the right line	angle + Delete; Perpendicular + ribbon 'Sketch › Constraints > Relax Constraint'; line + 'Sketch › Constraints > Vertical'	same	DoF after each: 1, 2, 1 (the book: one more constraint needed); 'Under-constrained: / 1 Degrees of Freedom'
J10	Vertical dimension: fully constrained	right line + ribbon 'Sketch › Constraints > Distance' = 72 mm	same	DoF 0; 'Fully constrained'
J11	Circle inside, Tangent to the left inclined line	O key + 2 MB1 clicks + MB2; circle + line + ribbon 'Sketch › Constraints > Tangent'	same	DoF 2 (centre still slides along the line); 'Under-constrained: / 2 Degrees of Freedom'
J12	Match the figure: circle located from the right side and the base, a diameter	values applied	differs	DoF 0; 'Fully constrained'; the figure’s values are not in the text
J13	Extrude, plate thickness 3.5 in	Ctrl+Q, 'lengthEdit' = 88.9 mm, MB2 = OK	same	thickness 88.900 mm; sketch Sketch
J14	Show the dimension names; enter p8/51.6 and p10/41.2; hole = 1/3 of the height	constraints renamed (width, height, hx, vy, dia) and given formulas	differs	FreeCAD names a dimension in its properties (NX: p0, p1 … automatically) and takes a formula after '=' in the dimension dialog: {'hx': 'Constraints.width / 5 * 1.6', 'vy': 'Constraints.height / 4 * 1.2', 'dia': 'Constraints.height / 3'}
J15	Change the triangle to 25 x 15 in: the hole follows	width = 635 mm, height = 381 mm	same	circle from the right side, from the base, diameter: 203.200, 114.300, 127.000 mm (formulas: 203.200, 114.300, 127.000)
J16	Change it to 25 x 20 in: location and size follow	width = 635 mm, height = 508 mm	same	circle from the right side, from the base, diameter: 203.200, 152.400, 169.333 mm (formulas: 203.200, 152.400, 169.333)
J17	The part is shown in the graphics window	render of the graphics window	same	6.4% 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, Model template

Ctrl+N

same

Extrude (X), YZ plane of the datum CSYS

X key, plane row + MB2

same

picked YZ-plane (Base plane)

Profile: a triangle with a horizontal base

Z key + 4 MB1 clicks + MB2

same

3 lines; implicit constraints ['Coincident', 'Horizontal']; DoF 5; FreeCAD says 'Under-constrained: / 5 Degrees of Freedom'

Perpendicular: the two inclined lines, OK

both lines selected + ribbon 'Sketch › Constraints > Perpendicular'

same

angle between them 90.000° (90 wanted); DoF 4; 'Under-constrained: / 4 Degrees of Freedom'

Dimensions: base length, angle to the right line; the triangle still moves

line + ribbon 'Sketch › Constraints > Distance' = 120 mm, two lines + 'Angle' = 60° (typed in FreeCAD’s dimension dialog)

same

base 120.000 mm; DoF 2 (size fixed, position free, as in the book); 'Under-constrained: / 2 Degrees of Freedom'

Fix Curve on one line: fully defined

line + ribbon 'Sketch › Constraints > Fully Fixed'

same

DoF 0, fully constrained True; NX turns the sketch black and says it is fully defined, FreeCAD says 'Fully constrained'

Undo, then Coincident: the left corner on the sketch origin

Ctrl+Z (DoF back to 2); Vertex1 + origin + ribbon 'Sketch › Constraints > Coincident'

same

corner at (0.000, -0.000); DoF 0; 'Fully constrained'

Undo, then location dimensions from the Y axis and the X axis

Ctrl+Z (DoF 2); corner + Y axis, corner + X axis, ribbon 'Sketch › Constraints > Distance', 25.4 each

same

corner at (25.400, 25.400); DoF 0; 'Fully constrained'

Delete the angle, relax Perpendicular, Vertical on the right line

angle + Delete; Perpendicular + ribbon 'Sketch › Constraints > Relax Constraint'; line + 'Sketch › Constraints > Vertical'

same

DoF after each: 1, 2, 1 (the book: one more constraint needed); 'Under-constrained: / 1 Degrees of Freedom'

J10

Vertical dimension: fully constrained

right line + ribbon 'Sketch › Constraints > Distance' = 72 mm

same

DoF 0; 'Fully constrained'

J11

Circle inside, Tangent to the left inclined line

O key + 2 MB1 clicks + MB2; circle + line + ribbon 'Sketch › Constraints > Tangent'

same

DoF 2 (centre still slides along the line); 'Under-constrained: / 2 Degrees of Freedom'

J12

Match the figure: circle located from the right side and the base, a diameter

values applied

differs

DoF 0; 'Fully constrained'; the figure’s values are not in the text

J13

Extrude, plate thickness 3.5 in

Ctrl+Q, 'lengthEdit' = 88.9 mm, MB2 = OK

same

thickness 88.900 mm; sketch Sketch

J14

Show the dimension names; enter p8/5*1.6 and p10/4*1.2; hole = 1/3 of the height

constraints renamed (width, height, hx, vy, dia) and given formulas

differs

FreeCAD names a dimension in its properties (NX: p0, p1 … automatically) and takes a formula after '=' in the dimension dialog: {'hx': 'Constraints.width / 5 * 1.6', 'vy': 'Constraints.height / 4 * 1.2', 'dia': 'Constraints.height / 3'}

J15

Change the triangle to 25 x 15 in: the hole follows

width = 635 mm, height = 381 mm

same

circle from the right side, from the base, diameter: 203.200, 114.300, 127.000 mm (formulas: 203.200, 114.300, 127.000)

J16

Change it to 25 x 20 in: location and size follow

width = 635 mm, height = 508 mm

same

circle from the right side, from the base, diameter: 203.200, 152.400, 169.333 mm (formulas: 203.200, 152.400, 169.333)

J17

The part is shown in the graphics window

render of the graphics window

same

6.4% 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

NX numbers dimensions by itself (p0, p1 …); FreeCAD names a dimension in its properties.
FreeCAD’s panel says the constraint state where NX’s status line does.