Tutorial BB: Hex Bolt Drawing

Source	Ming C. Leu, Wenjin Tao, Amir Ghazanfari and Krishna Kolan, NX 12 for Engineering Design (Missouri University of Science and Technology), section 5.6 (example).
You learn	a large sheet at an enlarging scale, Projected View, hidden lines, vertical dimensions, a Note with a leader and symbols, Radial, an isometric Base View
Part	tutorial AQ's screw, `Impeller_hexa-bolt`. The replay runs AQ first.
Sizes	the book’s, in inches, typed in millimetres.

5.7, the last section of the chapter, is an open exercise: draft the chapter 4 parts. It is not replayed; tutorials AZ and BB cover the commands it would use.

Step by step

1. Sheet and views

Open Impeller_hexa-bolt, press Ctrl+Shift+D and click New Sheet. Choose the template ANSIE_Landscape.svg (E, 34 x 44 in), the scale 8 and Third angle.

Select the screw’s bodies and click Base View, direction Front: the screw stands with its head up. Select the view, click Projected View, then Right and Above, and press MB2. The view above is the top view: the hexagon. Display Borders is already off, as in tutorial AZ.

Select the three views and turn on their Hard Hidden: hidden lines are drawn dashed. The top view now shows the shank under the head as a dashed circle.

2. Dimensions

Pick two vertices and click Vertical:

View	Length	Book (in)
Front	the whole screw, from its end to the top of the head	1.703
Front	the head	0.188
Front	from the top of the head down to where the sphere meets the hexagon’s corners	0.065
Right	the step under the head	0.016

View

Length

Book (in)

Front

the whole screw, from its end to the top of the head

1.703

Front

the head

0.188

Front

from the top of the head down to where the sphere meets the hexagon’s corners

0.065

Right

the step under the head

0.016

3. The thread note

Select an edge of the thread on the front view and click Note. Type Right Hand, click the Ø button, type 0.20 x 1.5, press Enter, type Pitch 0.05, Angle 60 and click the ° button. Set the lettering height to 7 mm and the stub length to 12.7 mm, and press MB2. The leader runs from the thread to the note.

4. Radial and the isometric view

Select the circle on top of the head in the top view and click Radial. Select the screw’s bodies again, click Base View, and set the direction to isometric.

Save the part.

The replay

#	In the book (NX)	In FreeCAD NX-Style	Result	Notes
BB1	Open Impeller_hexa-bolt (tutorial AQ’s part)	File > Open (by script)	same	tutorial AQ’s screw (3 bodies): 1.7032 in long, 0.4920 across the head (the book’s 1.7032 and 0.492); head same solid as the reference: 0 mm³ differ, box within 8e-14 mm, 9 faces (9 in the reference)
BB2	File > Drafting	Ctrl+Shift+D	same	TechDrawWorkbench
BB3	Sheet: E-34 X 44, Scale 8.0 : 1.0, OK	ribbon 'Home › Drawing > New Sheet'; the sheet’s Template, Scale and Projection	differs	ANSIE_Landscape.svg: 1118.0 x 864.0 mm (the book’s 44 x 34 in), scale 8.0, 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
BB4	Base View: Front, a click to place it	the screw’s bodies selected + ribbon 'Home › View > Base View', MB2 on the sheet; the view’s Direction Front	differs	edges span (12.4968, 43.2841) mm unscaled (the screw: 43.261 tall); scale 8.0. As in tutorial AZ, the direction is the view’s property
BB5	Add the orthographic views Right and Top	front view selected + ribbon 'Home › View > Projected View', Right and Above, MB2	same	directions {'right': (1.0, 0.0, 0.0), 'top': (-0.0, 0.0, 1.0)}
BB6	Preferences > Drafting > View: Display Borders off	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
BB7	Select the views, RMB > Settings > Hidden Lines: Process Hidden Lines, Dashed Lines, OK	the three views selected; their Hard Hidden property on	differs	the top view shows the shank under the head as a dashed circle (radius 3.175 mm among its hidden circles [2.4876, 3.175, 4.9149]). NX’s view Settings dialog; TechDraw’s Hard Hidden draws them dashed
BB8	Insert > Dimensions > Linear: vertical dimensions 1.703, 0.188 and 0.065 on the front view, 0.016 on the right view	two vertices picked + ribbon 'Vertical'	differs	(view, book in, drawing in, model in): [('front', 1.703, 1.7032, 1.7032), ('front', 0.065, 0.0647, 0.0647), ('front', 0.188, 0.1876, 0.1876), ('right', 0.016, 0.0156, 0.0156)]. The 0.065 runs to where the head’s sphere meets the hexagon’s corners. Points with no vertex of their own (the screw’s end, cut by the thread) get a cosmetic vertex on the edge there
BB9	Note: 'Right Hand Ø0.20 x 1.5', 'Pitch 0.05, Angle 60°' (Ø and ° from the Symbols tab), a leader from the threaded shaft; Settings: Lettering Height and the leader’s length increased	a thread edge of the front view selected + ribbon 'Home › Annotation > Note', the text typed with the Ø and ° buttons, Lettering height 7 and Stub length 12.7 mm, MB2	differs	note ['Right Hand Ø0.20 x 1.5', 'Pitch 0.05, Angle 60°'], height 7.0 mm; the arrow ends at model (x, z) (-3.1683, 18.8254) mm: on the shank’s thread (radius 3.175). NX drags the leader from the shaft and sets height and length in Settings afterwards; here they are fields of the dialog
BB10	Radial: click the circle of the bolt in the top view	the head’s top circle selected + ribbon 'Home › Dimension > Radial'	differs	R0.201 in (5.107310329165429 mm), the circle where the head’s sphere meets its top face (radius 0.2011 in from the model). The book’s figure labels this circle Ø0.200, the size of its radius; TechDraw’s Radial gives R
BB11	Base View: Isometric, placed beside the others	the screw’s bodies selected + ribbon 'Home › View > Base View', MB2; Direction isometric	same	direction (0.57735, -0.57735, 0.57735), 668 edges, scale 4.0 (half the sheet’s, to fit beside the views)
BB12	Save	file name given once by script (the system file dialog is not driven); a change, then the Ctrl+S key	same	Impeller_hexa-bolt.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

BB1

Open Impeller_hexa-bolt (tutorial AQ’s part)

File > Open (by script)

same

tutorial AQ’s screw (3 bodies): 1.7032 in long, 0.4920 across the head (the book’s 1.7032 and 0.492); head same solid as the reference: 0 mm³ differ, box within 8e-14 mm, 9 faces (9 in the reference)

BB2

File > Drafting

Ctrl+Shift+D

same

TechDrawWorkbench

BB3

Sheet: E-34 X 44, Scale 8.0 : 1.0, OK

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

differs

ANSIE_Landscape.svg: 1118.0 x 864.0 mm (the book’s 44 x 34 in), scale 8.0, 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

BB4

Base View: Front, a click to place it

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

differs

edges span (12.4968, 43.2841) mm unscaled (the screw: 43.261 tall); scale 8.0. As in tutorial AZ, the direction is the view’s property

BB5

Add the orthographic views Right and Top

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

same

directions {'right': (1.0, 0.0, 0.0), 'top': (-0.0, 0.0, 1.0)}

BB6

Preferences > Drafting > View: Display Borders off

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

BB7

Select the views, RMB > Settings > Hidden Lines: Process Hidden Lines, Dashed Lines, OK

the three views selected; their Hard Hidden property on

differs

the top view shows the shank under the head as a dashed circle (radius 3.175 mm among its hidden circles [2.4876, 3.175, 4.9149]). NX’s view Settings dialog; TechDraw’s Hard Hidden draws them dashed

BB8

Insert > Dimensions > Linear: vertical dimensions 1.703, 0.188 and 0.065 on the front view, 0.016 on the right view

two vertices picked + ribbon 'Vertical'

differs

(view, book in, drawing in, model in): [('front', 1.703, 1.7032, 1.7032), ('front', 0.065, 0.0647, 0.0647), ('front', 0.188, 0.1876, 0.1876), ('right', 0.016, 0.0156, 0.0156)]. The 0.065 runs to where the head’s sphere meets the hexagon’s corners. Points with no vertex of their own (the screw’s end, cut by the thread) get a cosmetic vertex on the edge there

BB9

Note: 'Right Hand Ø0.20 x 1.5', 'Pitch 0.05, Angle 60°' (Ø and ° from the Symbols tab), a leader from the threaded shaft; Settings: Lettering Height and the leader’s length increased

a thread edge of the front view selected + ribbon 'Home › Annotation > Note', the text typed with the Ø and ° buttons, Lettering height 7 and Stub length 12.7 mm, MB2

differs

note ['Right Hand Ø0.20 x 1.5', 'Pitch 0.05, Angle 60°'], height 7.0 mm; the arrow ends at model (x, z) (-3.1683, 18.8254) mm: on the shank’s thread (radius 3.175). NX drags the leader from the shaft and sets height and length in Settings afterwards; here they are fields of the dialog

BB10

Radial: click the circle of the bolt in the top view

the head’s top circle selected + ribbon 'Home › Dimension > Radial'

differs

R0.201 in (5.107310329165429 mm), the circle where the head’s sphere meets its top face (radius 0.2011 in from the model). The book’s figure labels this circle Ø0.200, the size of its radius; TechDraw’s Radial gives R

BB11

Base View: Isometric, placed beside the others

the screw’s bodies selected + ribbon 'Home › View > Base View', MB2; Direction isometric

same

direction (0.57735, -0.57735, 0.57735), 668 edges, scale 4.0 (half the sheet’s, to fit beside the views)

BB12

Save

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

same

Impeller_hexa-bolt.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 views' directions are checked, and the top view must show a hidden circle of the shank’s radius. Each dimension is compared with the screw’s own geometry: its height, the head, the step, and where the head’s sphere meets the hexagon. It must also match the book’s number to its three decimals. The note’s arrow is traced back from the sheet into the model and must end on the threaded shank.

What differs from NX

As in tutorial AZ, the sheet’s size, scale and projection are properties, and a view’s direction is a property.
NX sets the hidden line style in the views' Settings dialog. TechDraw’s Hard Hidden draws hidden lines dashed.
NX drags the leader from the shaft and sets the lettering height and leader length in Settings afterwards. Here they are fields of the Note dialog.
The note’s text is the book’s. It gives Ø0.20, while AQ’s thread is the book’s 1/4-20 UNC on a Ø0.25 shank.
The book’s figure labels the circle on top of the head Ø0.200, which is the size of its radius (0.201). TechDraw’s Radial shows it as a radius.
TechDraw computes hidden lines for the detailed thread, so these views take longer to appear than plain ones.