Tutorial AK: Holder

Source	Ming C. Leu, Wenjin Tao, Amir Ghazanfari and Krishna Kolan, NX 12 for Engineering Design (Missouri University of Science and Technology), exercise 3.6.2. The book gives only the dimensioned figure; the steps here are ours. Chapter 4 models the holder in 3D from this sketch: tutorial AW.
You learn	circles and their diameters, a reference curve, Quick Trim, a cross and lugs drawn once and copied with Rotate Curve (NX: Pattern Curve, circular), tangent arcs in Profile
Sizes	the book’s, in inches, typed in millimetres. Circles Ø0.75, Ø2.00 and Ø2.76 about the origin. The outline is a Ø3.50 circle and a 5.50 × 3.50 rectangle to its right, opened by a 0.50 slot along the X axis. A cross 0.25 wide runs from the Ø0.75 circle to the Ø2.76 circle. Three lugs sit on a Ø4.50 bolt circle, 120° apart. Each lug is a Ø0.38 hole in an R0.38 end, and its sides are tangent to the end and 1.00 apart where they meet the Ø3.50 circle.

The figure does not say where the sides of the lugs at 60° and 300° end. Here they end on the Ø3.50 circle, as at 180°, so all three lugs are the same.

Step by step

1. A new part and a sketch

Ctrl+N, then Sketch on the XC-YC plane and MB2.

2. The circles

Press O for Circle. Click the origin, then a point on the rim; do this four times, for Ø0.75, Ø2.00, Ø2.76 and Ø3.50, and press MB2. Give the diameters, biggest first: pick each circle and choose Radius / Diameter drop-down > Constrain diameter.

Draw the Ø4.50 bolt circle the same way. Select it and click Convert To/From Reference: it becomes a reference curve, drawn dashed.

3. The outline and the slot

Press Z for Profile. Click the top of the Ø3.50 circle, then go round the rectangle: right 5.50, down 3.50, back left to the bottom of the circle, and press MB2. The ends snap to the circle, tangent to it. Give the length: pick the top right corner and the Y axis, then Distance 5.50.

Press L for Line and draw the slot’s two sides, from the Ø3.50 circle to the right side. Dimension them: Distance 0.50 between them, and 0.25 from the X axis for the upper one.

Press T for Quick Trim, click the circle between the slot’s sides and press MB2. The sides stay tangent to what is left of the circle.

4. The cross

Draw one arm with Line: two lines from the Ø0.75 circle to the Ø2.76 circle, 0.25 apart, the upper one 0.125 above the X axis. Select the two lines and click Rotate Curve. In the Dialog panel set Copies to 3. Click the origin as the centre, then type 0° and 270° in the fields beside the pointer.

5. The lugs

Draw the lug at 180° with Profile:

start on the Ø3.50 circle, 0.5 below the X axis, and go out to the end;
press M three times for a tangent arc and go round the end;
go back to the circle, which FreeCAD draws as a tangent line.

Then fix it:

the arc’s centre on the bolt circle and on the X axis (Point on Curve);
the radius 0.38 (Radius / Diameter drop-down > Constrain radius);
Distance 1.00 between the two sides' ends on the circle, and the two sides Equal.

Draw the Ø0.38 hole: O, click the arc’s centre and the rim, then give its diameter. Select the lug’s three curves and the hole, click Rotate Curve, set Copies to 2, click the origin and type 0° and 240°.

Ctrl+Q, and save with Ctrl+S.

The replay

#	In the book (NX)	In FreeCAD NX-Style	Result	Notes
AK1	A new part in inches (Holder)	Ctrl+N, Model template	same	new document ['Unnamed1']
AK2	Units in the New dialog (the book picks inches)	metric part kept; book sizes typed in mm	differs	FreeCAD sets units in Preferences, not in the New dialog; NXStyle defaults to millimetres (document: Standard (mm, kg, s, °); 25.4 mm shows as 25.40 mm)
AK3	Sketch on the XC-YC plane, OK	ribbon 'Home › Direct Sketch > Sketch', plane row + MB2	same	picked XY-plane (Base plane)
AK4	Circles Ø0.75, Ø2.00, Ø2.76 and Ø3.50 about the origin	O key, MB1 at the origin and on the rim, 4 times, MB2; each circle + 'Radius / Diameter' drop-down > 'Constrain diameter', biggest first	same	Ø3.50, Ø2.76, Ø2.00, Ø0.75; largest error 1.4e-14 mm (centres on the origin, diameters); DoF 0
AK5	The Ø4.50 bolt circle, a reference curve	O key, MB1 at the origin and on the rim, MB2; circle + ribbon 'Sketch › Edit Curve > Convert To/From Reference'; Diameter 4.50	same	reference True; diameter 4.5000 in; DoF 0
AK6	Profile: the rectangle’s three sides from the top of the Ø3.50 circle to its bottom, 5.50 long	Z key, 4 MB1 clicks, MB2; the ends + circle or Y axis + 'Point on Curve'; corner + Y axis + 'Sketch › Constraints > Distance' 5.50	same	Horizontal/Vertical/Horizontal [True, True, True]; 4 of 4 end holds made by the clicks (2 as Tangent to the circle), 0 added; DoF 0; the sides match
AK7	Line: the 0.50 slot’s two sides, from the circle to the right side	L key, 4 MB1 clicks, MB2; 'Sketch › Constraints > Distance' 0.50 between them and 0.25 from the X axis	same	Horizontal as drawn [True, True]; 4 of 4 ends snapped to the circle or the side, 0 added; DoF 0; the sides match
AK8	Quick Trim: the Ø3.50 circle between the slot’s sides, MB2	T key, MB1 on the circle inside the slot, MB2	same	1 arc R1.75, full circle left False; its ends held to the slot’s sides 2 of 2; DoF 0 ('Fully constrained'); geometry 10 → 10; 1 tangency FreeCAD’s trim dropped put back by NX-Style
AK9	Line: one arm of the cross, 0.25 wide, from the Ø0.75 circle to the Ø2.76 circle	L key, 4 MB1 clicks, MB2; 'Sketch › Constraints > Distance' 0.25 between the lines and 0.125 from the X axis	same	4 of 4 ends snapped to the circles, 0 added; DoF 0; the arm matches
AK10	Rotate Curve: the arm, 3 copies 90° apart, about the origin (NX: Pattern Curve, circular)	2 lines selected + ribbon 'Sketch › Edit Curve > Rotate Curve', Copies 3, MB1 at the origin, 0° and 270° typed in the on-view fields	same	6 copies made; largest error 4.5e-07 mm; DoF 21
AK11	Profile: the lug at 180°, a side, the tangent end arc, the other side	Z key, 4 MB1 clicks (M 3x before the arc’s end), MB2	same	curves ['line', 'arc', 'line']; tangent joints 2
AK12	The lug: centre on the bolt circle and the X axis, R0.38, the sides 1.00 apart and Equal	centre + bolt circle / X axis + 'Point on Curve', arc + 'Radius / Diameter' R0.38, the ends + 'Sketch › Constraints > Distance' 1.00, the sides + 'Equal'	same	centre on the bolt circle; centre on the X axis; R0.38; 1.00 between the sides' ends; sides Equal; 1 of 2 side ends snapped to the circle, 1 added; DoF 21 ('Under-constrained: / 21 Degrees of Freedom'); the lug matches
AK13	Circle: the Ø0.38 hole about the lug’s centre	O key, MB1 on the arc’s centre and on the rim, MB2; Diameter 0.38	same	centre snapped to the arc’s centre; error 0.0e+00 mm; DoF 21
AK14	Rotate Curve: the lug and its hole, 2 copies 120° apart, about the origin (NX: Pattern Curve)	4 curves selected + ribbon 'Sketch › Edit Curve > Rotate Curve', Copies 2, MB1 at the origin, 0° and 240° typed in the on-view fields	same	8 copies made; largest error 3.6e-06 mm; DoF 29
AK15	The sketch: 29 curves and the bolt circle	compared with the book’s figure	same	29 curves; all 29 match the book; DoF 29 ('Under-constrained: / 29 Degrees of Freedom')
AK16	Finish Sketch	Ctrl+Q	same	sketch edit ended True
AK17	Save the file	file name given once by script (the system file dialog is not driven); a change, then the Ctrl+S key	same	Holder.FCStd rewritten by Ctrl+S: the file holds the change and the part is unmodified afterwards (modified before the key: True); FreeCAD format, not .prt

In the book (NX)

In FreeCAD NX-Style

Result

Notes

AK1

A new part in inches (Holder)

Ctrl+N, Model template

same

new document ['Unnamed1']

AK2

Units in the New dialog (the book picks inches)

metric part kept; book sizes typed in mm

differs

FreeCAD sets units in Preferences, not in the New dialog; NXStyle defaults to millimetres (document: Standard (mm, kg, s, °); 25.4 mm shows as 25.40 mm)

AK3

Sketch on the XC-YC plane, OK

ribbon 'Home › Direct Sketch > Sketch', plane row + MB2

same

picked XY-plane (Base plane)

AK4

Circles Ø0.75, Ø2.00, Ø2.76 and Ø3.50 about the origin

O key, MB1 at the origin and on the rim, 4 times, MB2; each circle + 'Radius / Diameter' drop-down > 'Constrain diameter', biggest first

same

Ø3.50, Ø2.76, Ø2.00, Ø0.75; largest error 1.4e-14 mm (centres on the origin, diameters); DoF 0

AK5

The Ø4.50 bolt circle, a reference curve

O key, MB1 at the origin and on the rim, MB2; circle + ribbon 'Sketch › Edit Curve > Convert To/From Reference'; Diameter 4.50

same

reference True; diameter 4.5000 in; DoF 0

AK6

Profile: the rectangle’s three sides from the top of the Ø3.50 circle to its bottom, 5.50 long

Z key, 4 MB1 clicks, MB2; the ends + circle or Y axis + 'Point on Curve'; corner + Y axis + 'Sketch › Constraints > Distance' 5.50

same

Horizontal/Vertical/Horizontal [True, True, True]; 4 of 4 end holds made by the clicks (2 as Tangent to the circle), 0 added; DoF 0; the sides match

AK7

Line: the 0.50 slot’s two sides, from the circle to the right side

L key, 4 MB1 clicks, MB2; 'Sketch › Constraints > Distance' 0.50 between them and 0.25 from the X axis

same

Horizontal as drawn [True, True]; 4 of 4 ends snapped to the circle or the side, 0 added; DoF 0; the sides match

AK8

Quick Trim: the Ø3.50 circle between the slot’s sides, MB2

T key, MB1 on the circle inside the slot, MB2

same

1 arc R1.75, full circle left False; its ends held to the slot’s sides 2 of 2; DoF 0 ('Fully constrained'); geometry 10 → 10; 1 tangency FreeCAD’s trim dropped put back by NX-Style

AK9

Line: one arm of the cross, 0.25 wide, from the Ø0.75 circle to the Ø2.76 circle

L key, 4 MB1 clicks, MB2; 'Sketch › Constraints > Distance' 0.25 between the lines and 0.125 from the X axis

same

4 of 4 ends snapped to the circles, 0 added; DoF 0; the arm matches

AK10

Rotate Curve: the arm, 3 copies 90° apart, about the origin (NX: Pattern Curve, circular)

2 lines selected + ribbon 'Sketch › Edit Curve > Rotate Curve', Copies 3, MB1 at the origin, 0° and 270° typed in the on-view fields

same

6 copies made; largest error 4.5e-07 mm; DoF 21

AK11

Profile: the lug at 180°, a side, the tangent end arc, the other side

Z key, 4 MB1 clicks (M 3x before the arc’s end), MB2

same

curves ['line', 'arc', 'line']; tangent joints 2

AK12

The lug: centre on the bolt circle and the X axis, R0.38, the sides 1.00 apart and Equal

centre + bolt circle / X axis + 'Point on Curve', arc + 'Radius / Diameter' R0.38, the ends + 'Sketch › Constraints > Distance' 1.00, the sides + 'Equal'

same

centre on the bolt circle; centre on the X axis; R0.38; 1.00 between the sides' ends; sides Equal; 1 of 2 side ends snapped to the circle, 1 added; DoF 21 ('Under-constrained: / 21 Degrees of Freedom'); the lug matches

AK13

Circle: the Ø0.38 hole about the lug’s centre

O key, MB1 on the arc’s centre and on the rim, MB2; Diameter 0.38

same

centre snapped to the arc’s centre; error 0.0e+00 mm; DoF 21

AK14

Rotate Curve: the lug and its hole, 2 copies 120° apart, about the origin (NX: Pattern Curve)

4 curves selected + ribbon 'Sketch › Edit Curve > Rotate Curve', Copies 2, MB1 at the origin, 0° and 240° typed in the on-view fields

same

8 copies made; largest error 3.6e-06 mm; DoF 29

AK15

The sketch: 29 curves and the bolt circle

compared with the book’s figure

same

29 curves; all 29 match the book; DoF 29 ('Under-constrained: / 29 Degrees of Freedom')

AK16

Finish Sketch

Ctrl+Q

same

sketch edit ended True

AK17

Save the file

file name given once by script (the system file dialog is not driven); a change, then the Ctrl+S key

same

Holder.FCStd rewritten by Ctrl+S: the file holds the change and the part is unmodified afterwards (modified before the key: True); FreeCAD format, not .prt

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.

Each of the 29 curves is compared with the book’s figure, rebuilt from its dimensions.

What differs from NX

FreeCAD’s Rotate Curve takes the angle that the copies are spread over: 3 copies over 270° are 90° apart. NX’s Pattern Curve takes the count and the angle between the copies.
The copies keep their own dimensions (the R0.38 and Ø0.38, the 1.00), but they are not tied to the original, so the sketch keeps degrees of freedom. NX’s pattern stays associative.
FreeCAD’s Profile holds each end of the rectangle to the circle with two constraints: Point on Curve for the click, and Tangent because the side leaves the circle along its tangent. With the side horizontal, that pair is partly redundant: FreeCAD does not flag it, and its solver leaves the end up to 0.0001 mm from the point of contact. NX-Style leaves this pair as FreeCAD makes it: holding the end by one end-point Tangent instead would not keep the trim from dropping it (next point).
FreeCAD’s Quick Trim keeps a tangency on the trimmed circle only when OCC finds the line and the arc intersecting. A side that touches the circle at its very end, held as Profile holds it or by an end-point Tangent, is found or not by the sign of a rounding error, and FreeCAD dropped one side’s Tangent in 3 of 4 replays. NX-Style puts back each tangency the trim dropped where the line still touches the arc, as part of the same trim (one Undo takes it back); the replay reports how many it put back.