Tutorial AZ: Arbor Press Rack Drawing

Source	Ming C. Leu, Wenjin Tao, Amir Ghazanfari and Krishna Kolan, NX 12 for Engineering Design (Missouri University of Science and Technology), sections 5.2 (creating a drawing), 5.3 (dimensioning) and 5.4 (sectional view).
You learn	New Sheet (size, scale, projection), Base View, Projected View, dimensions, Section View
Part	tutorial AT's rack, `Arborpress_rack`. The replay runs AT first.
Sizes	the book’s, in inches, typed in millimetres: the drawing’s dimensions read 25.4 times the book’s numbers.

Step by step

1. The sheet

Open Arborpress_rack and press Ctrl+Shift+D for Drafting. Click New Sheet. In the sheet’s properties, choose the template ANSIB_Landscape.svg (B, 11 x 17 in), the scale 0.04 (1:25) and Third angle.

2. The views

Select the rack’s body and click Base View. Set the view’s direction to Front and press MB2 to place it.

Select the front view and click Projected View. Click Above and Right, then press MB2. The top view and the right side view appear lined up with the front view, at its scale. The right view shows the hole in the end of the rack as a circle.

The book now turns off Display Borders. A FreeCAD sheet starts with Show Frames off, so there is nothing to press.

3. Dimensions

Pick the two end vertices of each length in the view and click Horizontal or Vertical:

View	Length	Book (in)	Drawing (mm)
Top	the rack’s length	240	6096
Top	from the left end to the first tooth space	34.8	883.92
Front	the tooth space’s opening	6.000	152.4
Front	its floor	3.396	86.26
Front	its depth	5.034	127.86
Right	the height	20	508
Right	the width	25	635

Drag each dimension clear of its view. Where a point has no vertex (the foot of a tooth space), the replay puts a cosmetic vertex on the edge there first.

4. The section

Select the front view and click Section View. Click the Up direction and press MB2. TechDraw cuts through the middle of the view, at the height of the hole’s axis. Move the section below the front view.

Save the part with Ctrl+S; the drawing is saved in it.

The replay

#	In the book (NX)	In FreeCAD NX-Style	Result	Notes
AZ1	Open Arborpress_rack (tutorial AT’s part)	File > Open (by script)	same	tutorial AT’s rack: same solid as the reference: 0 mm³ differ, box within 2.3e-12 mm, 84 faces (84 in the reference)
AZ2	File > Drafting	Ctrl+Shift+D	same	TechDrawWorkbench
AZ3	Sheet: Standard Size B 11 x 17, Custom Scale 1:25, OK	ribbon 'Home › Drawing > New Sheet'; the sheet’s Template, Scale and Projection	differs	ANSIB_Landscape.svg: 431.8 x 279.4 mm (the book’s 17 x 11 in), scale 0.04, Third angle. NX asks for size, scale and projection in one Sheet dialog; FreeCAD’s New Sheet uses the default template and these are the sheet’s properties
AZ4	Base View: Model View to Use Front, Scale 1:25, a click to place it	body selected + ribbon 'Home › View > Base View', MB2 on the sheet; the view’s Direction Front	differs	edges span (6096.0, 508.0) mm, the Part API (6096.0, 508.0) (240 x 20 in); scale 0.04 from the sheet. NX lists the model views in the Base View dialog; TechDraw’s view takes its direction as a property
AZ5	Projected View: move the cursor above and to the right of the front view and click; Close	front view selected + ribbon 'Home › View > Projected View', Above and Right, MB2	same	{'top': {'direction': (-0.0, 0.0, 1.0), 'span': (6096.0, 635.0), 'Part API': (6096.0, 635.0), 'scale': 0.04, 'at': (175.0, 182.86)}, 'right': {'direction': (1.0, 0.0, 0.0), 'span': (635.0, 508.0), 'Part API': (635.0, 508.0), 'scale': 0.04, 'at': (329.62, 140.0)}}; the right view shows the hole as a circle (Ø254 mm): True; each lined up with the front view at its scale
AZ6	Drafting Preferences > View: Display Borders off, OK	nothing to press: the sheet’s Show Frames is off	differs	Show Frames False. NX shows the borders until this is unchecked; FreeCAD’s sheet starts with Show Frames off. Its Turn View Frames On/Off stays greyed in FreeCAD 1.1.4, so NX-Style has no Display Borders button; how the sheet looks was not measured
AZ7	Dimensions: 240 and 34.8 on the top view; 6.000, 3.396 and 5.034 on the front view; 20 and 25 on the right view; each dragged clear of its view	two vertices picked + ribbon 'Horizontal' or 'Vertical' (the inferred direction of NX’s Rapid)	differs	(view, ribbon, book in, drawing mm, model mm): [('top', 'Horizontal', 240.0, 6096.0, 6096.0), ('top', 'Horizontal', 34.8, 883.92, 883.92), ('front', 'Horizontal', 6.0, 152.4, 152.4), ('front', 'Horizontal', 3.396, 86.2644, 86.2644), ('front', 'Vertical', 5.034, 127.8636, 127.8636), ('right', 'Vertical', 20.0, 508.0, 508.0), ('right', 'Horizontal', 25.0, 635.0, 635.0)]. All are the book’s numbers x 25.4. NX infers horizontal or vertical from the pointer; here the button says which. Where the view has no vertex at a point (a slot’s foot), a cosmetic vertex is put on the edge there first, as in tutorials H and N. The book’s text puts the 240 on the front view, its figures on the top view: the figures are followed
AZ8	Section View: a click under the front view’s middle (arrows up), drag the section below it, MB1	front view selected + ribbon 'Home › View > Section View', direction 'pbUp', MB2 = OK; the section moved below the front view	differs	cut plane normal (0.0, 0.0, -1.0) through (3048.0, 317.5, 254.0) (the hole’s axis is at z = 254); the hole’s walls in the section are 254.0 apart (Ø254: the cut is through its axis); section spans (6096.0, 635.0). TechDraw cuts through the middle of the view as the book’s click does, and puts the new view on top of its base view: it is moved afterwards
AZ9	Save and close the model (the drawing is saved in the part)	file name given once by script (the system file dialog is not driven); a change, then the Ctrl+S key	same	Arborpress_rack.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

AZ1

Open Arborpress_rack (tutorial AT’s part)

File > Open (by script)

same

tutorial AT’s rack: same solid as the reference: 0 mm³ differ, box within 2.3e-12 mm, 84 faces (84 in the reference)

AZ2

File > Drafting

Ctrl+Shift+D

same

TechDrawWorkbench

AZ3

Sheet: Standard Size B 11 x 17, Custom Scale 1:25, OK

ribbon 'Home › Drawing > New Sheet'; the sheet’s Template, Scale and Projection

differs

ANSIB_Landscape.svg: 431.8 x 279.4 mm (the book’s 17 x 11 in), scale 0.04, Third angle. NX asks for size, scale and projection in one Sheet dialog; FreeCAD’s New Sheet uses the default template and these are the sheet’s properties

AZ4

Base View: Model View to Use Front, Scale 1:25, a click to place it

body selected + ribbon 'Home › View > Base View', MB2 on the sheet; the view’s Direction Front

differs

edges span (6096.0, 508.0) mm, the Part API (6096.0, 508.0) (240 x 20 in); scale 0.04 from the sheet. NX lists the model views in the Base View dialog; TechDraw’s view takes its direction as a property

AZ5

Projected View: move the cursor above and to the right of the front view and click; Close

front view selected + ribbon 'Home › View > Projected View', Above and Right, MB2

same

{'top': {'direction': (-0.0, 0.0, 1.0), 'span': (6096.0, 635.0), 'Part API': (6096.0, 635.0), 'scale': 0.04, 'at': (175.0, 182.86)}, 'right': {'direction': (1.0, 0.0, 0.0), 'span': (635.0, 508.0), 'Part API': (635.0, 508.0), 'scale': 0.04, 'at': (329.62, 140.0)}}; the right view shows the hole as a circle (Ø254 mm): True; each lined up with the front view at its scale

AZ6

Drafting Preferences > View: Display Borders off, OK

nothing to press: the sheet’s Show Frames is off

differs

Show Frames False. NX shows the borders until this is unchecked; FreeCAD’s sheet starts with Show Frames off. Its Turn View Frames On/Off stays greyed in FreeCAD 1.1.4, so NX-Style has no Display Borders button; how the sheet looks was not measured

AZ7

Dimensions: 240 and 34.8 on the top view; 6.000, 3.396 and 5.034 on the front view; 20 and 25 on the right view; each dragged clear of its view

two vertices picked + ribbon 'Horizontal' or 'Vertical' (the inferred direction of NX’s Rapid)

differs

(view, ribbon, book in, drawing mm, model mm): [('top', 'Horizontal', 240.0, 6096.0, 6096.0), ('top', 'Horizontal', 34.8, 883.92, 883.92), ('front', 'Horizontal', 6.0, 152.4, 152.4), ('front', 'Horizontal', 3.396, 86.2644, 86.2644), ('front', 'Vertical', 5.034, 127.8636, 127.8636), ('right', 'Vertical', 20.0, 508.0, 508.0), ('right', 'Horizontal', 25.0, 635.0, 635.0)]. All are the book’s numbers x 25.4. NX infers horizontal or vertical from the pointer; here the button says which. Where the view has no vertex at a point (a slot’s foot), a cosmetic vertex is put on the edge there first, as in tutorials H and N. The book’s text puts the 240 on the front view, its figures on the top view: the figures are followed

AZ8

Section View: a click under the front view’s middle (arrows up), drag the section below it, MB1

front view selected + ribbon 'Home › View > Section View', direction 'pbUp', MB2 = OK; the section moved below the front view

differs

cut plane normal (0.0, 0.0, -1.0) through (3048.0, 317.5, 254.0) (the hole’s axis is at z = 254); the hole’s walls in the section are 254.0 apart (Ø254: the cut is through its axis); section spans (6096.0, 635.0). TechDraw cuts through the middle of the view as the book’s click does, and puts the new view on top of its base view: it is moved afterwards

AZ9

Save and close the model (the drawing is saved in the part)

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

same

Arborpress_rack.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.

Every check reads the drawing back from TechDraw and compares it with the model. The views' edges must span what the Part API gives for each direction. Each dimension must equal the length the Part API’s tooth space and bar give, and the book’s number times 25.4. The section must show the hole’s walls one diameter apart, which happens only when the cut goes through the hole’s axis.

What differs from NX

NX asks for the sheet size, scale and projection in one Sheet dialog. In FreeCAD they are the sheet’s properties.
NX lists the model views in the Base View dialog. A TechDraw view takes its direction as a property.
NX places a projected view where you click round the parent. Here you click a side button. In NX a projected view follows its parent when the parent is dragged; here it stays where it was placed.
NX shows a border round each view until Display Borders is unchecked. A FreeCAD sheet starts with Show Frames off, and FreeCAD’s Turn View Frames On/Off stays greyed in 1.1.4. The replay reports the property; it did not measure how the sheet looks.
NX infers horizontal or vertical from where you move the pointer. Here you choose the Horizontal or Vertical button.
TechDraw dimensions attach to vertices. Where NX snaps to any point on an edge, the replay adds a cosmetic vertex first.
The book’s text puts the 240 on the front view, but its figures put it on the top view. The replay follows the figures.
TechDraw puts a new section view on top of its base view. You move it afterwards.