Tutorial AF: Arbor Press Base

Source	Ming C. Leu, Wenjin Tao, Amir Ghazanfari and Krishna Kolan, NX 12 for Engineering Design (Missouri University of Science and Technology), section 3.5.1
You learn	Profile with lines and an arc, geometric constraints before dimensions, Equal, Collinear, Tangent, a fully defined sketch, Extrude from a selected sketch
Sizes	from the book’s dimension figure: 130 wide, 190.94 high; the outer sides 125; the top 95 wide with a notch 65 wide and 65 deep; a slot 40 wide ending in a semicircle whose centre is the origin, 35 above the bottom edge; extruded 60 mm

Step by step

1. A new part and a sketch

Ctrl+N for a new part. Click Sketch on the Home tab, pick the XC-YC plane and press MB2.

2. Profile: lines and one arc

Press Z for Profile. Start at the bottom left and click round the outline: along the bottom to the slot, up its left side, then press M three times to switch to a tangent arc and click the slot’s right side. Where the book clicks Line in the Profile dialog, press M twice: FreeCAD would otherwise carry on with a line held tangent to the arc. Continue with lines down the slot, along the bottom, up the right side, through the notch at the top and down the left side, and click the first point: that closes the outline. MB2 ends Profile. Draw it roughly. The constraints bring it to shape. Each straight line gets Horizontal or Vertical as it is drawn, except the two slanted ones. FreeCAD has no automatic dimensions to switch off, so the book’s note about Continuous Auto Dimensioning does not apply.

3. Geometric constraints first

Point on Curve: pick the Y axis and the arc’s centre and click Point on Curve, then the X axis and the centre.
Equal: the two slanted lines, then the two long vertical lines.
The bottom lines: pick both and click Collinear, then Equal.
Tangent: the arc and the slot’s sides, where it is missing. Profile made the first one; the line after the arc needs it.
The book makes the slot’s two short sides Equal. Here FreeCAD reports that as redundant, because the tangency and the centre on the X axis already make them equal, so leave it out.
The two short top lines: Collinear and Equal, as at the bottom. The notch’s two sides are then equal too.

4. Dimensions, biggest first

Click Distance with the picks selected and type each value: the height 190.94, the width 130, the right side 125, the top 95, the notch 65 wide and 65 deep, the slot 40, and the centre 35 above the bottom. The Dialog panel then says Fully constrained and the sketch turns green.

5. Extrude 60 and save

Ctrl+Q finishes the sketch. Select the sketch, press X, type 60 and press MB2. Save with Ctrl+S.

The replay

#	In the book (NX)	In FreeCAD NX-Style	Result	Notes
AF1	Create a new file (Arborpress_base)	Ctrl+N, Model template	same	new document ['Unnamed']; the name is given when it is saved
AF2	Sketch, OK (the XC-YC plane)	ribbon 'Home › Direct Sketch > Sketch', plane row + MB2	same	picked XY-plane (Base plane); sketch Sketch
AF3	Profile (Z): lines, and an arc for the semicircle (Continuous Auto Dimensioning off)	Z key, 15 MB1 clicks (the last on the first point), M 3x before the arc’s end and 2x after it (the book clicks Line), MB2	same	14 curves (13 lines, 1 arc); closed by the last click True; Horizontal/Vertical inferred on every straight line except the two slanted ones; arc tangent to ['Edge2']; tool ended by MB2 True; DoF 17. FreeCAD has no automatic dimensions to switch off
AF4	Point on Curve: the arc’s centre on the Y axis, then on the X axis	axis + centre + ribbon 'Sketch › Constraints > Point on Curve', twice	same	centre at (-0.000, 0.000); made ['PointOnObject 2/3 -2', 'PointOnObject 2/3 -1']; DoF 15 ('Under-constrained: / 15 Degrees of Freedom')
AF5	Equal Length: the two slanted lines, then the two long vertical lines	two lines + ribbon 'Sketch › Constraints > Equal', twice	same	slanted 67.07 / 67.07, verticals 124.45 / 124.45 mm; DoF 13
AF6	Collinear, then Equal Length: the two bottom lines	two lines + ribbon 'Sketch › Constraints > Collinear'; two lines + 'Equal'	same	the bottom lines 0.0000 mm apart (Collinear added 1 point-on-curve constraint, solver 0), lengths 38.77 / 38.77 mm; DoF 11
AF7	Tangent: the arc and each vertical line at its ends (only where it is missing)	arc + line + ribbon 'Tangent' where missing	same	already tangent from Profile: ['Edge2']; added [('Edge4', 0)]; arc radius 21.670 mm about (0.000, 0.000); DoF 10
AF8	Equal Length: the slot’s two vertical lines	two lines + ribbon 'Sketch › Constraints > Equal', then Ctrl+Z	differs	FreeCAD reports it redundant (solver -2; 'Redundant constraints:'): the tangency and the centre on the X axis already make them equal, so it is undone (removed)
AF9	Collinear, then Equal: the two short lines at the top	two lines + ribbon 'Sketch › Constraints > Collinear'; two lines + 'Equal'	same	the top lines 0.0000 mm apart (Collinear added 1 point-on-curve constraint, solver 0), lengths 16.06 / 16.06 mm; DoF 8; the notch’s two sides are then equal too (the book’s last Equal is implied)
AF10	Rapid Dimension: eight dimensions, then the values, biggest first; the sketch is fully defined	picks + ribbon 'Sketch › Constraints > Distance', the value typed in FreeCAD’s dimension dialog, 8 times	differs	height 190.94, width 130, side 125, top 95, notch width 65, notch depth 65, slot 40, centre 35; DoF 0, fully constrained True ('Fully constrained'); corners within 1.5e-13 mm of the book’s figure. NX places all dimensions first and edits them; FreeCAD asks for each value as the dimension is made
AF11	Finish Sketch	Ctrl+Q	same	sketch edit ended True
AF12	Select the sketch, Extrude (X): Z direction, 60 mm, Boolean None	sketch selected + X; 'lengthEdit' = 60 mm, MB2 = OK	same	Boolean 'None' (None (a new body): ready (OK or MB2 commits one undo step)); section Sketch; same solid as the reference: 0 mm³ differ, box within 5.7e-14 mm, 16 faces (16 in the reference); controller: committed new_body, undo step 'Extrude', 1 step(s) added
AF13	Save and close the file	file name given once by script (the system file dialog is not driven); a change, then the Ctrl+S key	same	Arborpress_base.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

AF1

Create a new file (Arborpress_base)

Ctrl+N, Model template

same

new document ['Unnamed']; the name is given when it is saved

AF2

Sketch, OK (the XC-YC plane)

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

same

picked XY-plane (Base plane); sketch Sketch

AF3

Profile (Z): lines, and an arc for the semicircle (Continuous Auto Dimensioning off)

Z key, 15 MB1 clicks (the last on the first point), M 3x before the arc’s end and 2x after it (the book clicks Line), MB2

same

14 curves (13 lines, 1 arc); closed by the last click True; Horizontal/Vertical inferred on every straight line except the two slanted ones; arc tangent to ['Edge2']; tool ended by MB2 True; DoF 17. FreeCAD has no automatic dimensions to switch off

AF4

Point on Curve: the arc’s centre on the Y axis, then on the X axis

axis + centre + ribbon 'Sketch › Constraints > Point on Curve', twice

same

centre at (-0.000, 0.000); made ['PointOnObject 2/3 -2', 'PointOnObject 2/3 -1']; DoF 15 ('Under-constrained: / 15 Degrees of Freedom')

AF5

Equal Length: the two slanted lines, then the two long vertical lines

two lines + ribbon 'Sketch › Constraints > Equal', twice

same

slanted 67.07 / 67.07, verticals 124.45 / 124.45 mm; DoF 13

AF6

Collinear, then Equal Length: the two bottom lines

two lines + ribbon 'Sketch › Constraints > Collinear'; two lines + 'Equal'

same

the bottom lines 0.0000 mm apart (Collinear added 1 point-on-curve constraint, solver 0), lengths 38.77 / 38.77 mm; DoF 11

AF7

Tangent: the arc and each vertical line at its ends (only where it is missing)

arc + line + ribbon 'Tangent' where missing

same

already tangent from Profile: ['Edge2']; added [('Edge4', 0)]; arc radius 21.670 mm about (0.000, 0.000); DoF 10

AF8

Equal Length: the slot’s two vertical lines

two lines + ribbon 'Sketch › Constraints > Equal', then Ctrl+Z

differs

FreeCAD reports it redundant (solver -2; 'Redundant constraints:'): the tangency and the centre on the X axis already make them equal, so it is undone (removed)

AF9

Collinear, then Equal: the two short lines at the top

two lines + ribbon 'Sketch › Constraints > Collinear'; two lines + 'Equal'

same

the top lines 0.0000 mm apart (Collinear added 1 point-on-curve constraint, solver 0), lengths 16.06 / 16.06 mm; DoF 8; the notch’s two sides are then equal too (the book’s last Equal is implied)

AF10

Rapid Dimension: eight dimensions, then the values, biggest first; the sketch is fully defined

picks + ribbon 'Sketch › Constraints > Distance', the value typed in FreeCAD’s dimension dialog, 8 times

differs

height 190.94, width 130, side 125, top 95, notch width 65, notch depth 65, slot 40, centre 35; DoF 0, fully constrained True ('Fully constrained'); corners within 1.5e-13 mm of the book’s figure. NX places all dimensions first and edits them; FreeCAD asks for each value as the dimension is made

AF11

Finish Sketch

Ctrl+Q

same

sketch edit ended True

AF12

Select the sketch, Extrude (X): Z direction, 60 mm, Boolean None

sketch selected + X; 'lengthEdit' = 60 mm, MB2 = OK

same

Boolean 'None' (None (a new body): ready (OK or MB2 commits one undo step)); section Sketch; same solid as the reference: 0 mm³ differ, box within 5.7e-14 mm, 16 faces (16 in the reference); controller: committed new_body, undo step 'Extrude', 1 step(s) added

AF13

Save and close the file

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

same

Arborpress_base.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.

The solid is compared with the same solid built with FreeCAD’s Part API (nxstyle/geomcheck.py), and every corner of the sketch with the book’s figure.

What differs from NX

FreeCAD has no collinear constraint. NX-Style’s Collinear puts the ends of one line on the other line; both bottom lines are horizontal already, so one end is enough and only one point-on-curve constraint is added.
NX places all the dimensions first and then edits their values. FreeCAD asks for each value as the dimension is made, so the replay types them biggest first, as the book recommends.
FreeCAD’s Profile switches to an arc with M, and back to a plain line with M twice more. NX has Line and Arc buttons in the Profile toolbar.
FreeCAD rejects a constraint that is already implied, and reports it as redundant.