Tutorial F: Dryer Housing

Book	Shih, Parametric Modeling with Siemens NX, ch. 12
You learn	Shell, Edge Blend, a pattern leader, Pattern Feature in two directions
Sizes	The text gives R6.35, 12.7, 139.7, R3.81, 3.175 and 3.81 mm and the pattern (5 × −14.73 mm, 10 × −6.35 mm), the book’s inch values typed in mm. Every profile is in figures only, so the housing is a simplified one: an R50.8 × 31.75 mm drum, a 19.05 mm wide handle, an R19.05 half nozzle.

In short

The drum by Revolve, the handle and the nozzle by Extrude.
Shell (3.175 mm walls), then Edge Blend on the handle.
A vent as the pattern leader; Pattern Feature with Direction 2 ticked: 5 × 10.

The swept cut along the rim (F27) is skipped: its guide and section are in figures only.

Step by step

#	In the book (NX)	In FreeCAD NX-Style	Result	Notes
F1	File > New, Model template	Ctrl+N	same
F2	Revolve, YZ plane of the datum CSYS	ribbon 'Home › Feature > Revolve', plane row + MB2	same	picked YZ-plane (Base plane)
F3	Profile, then Fillet R0.25 between the top line and the side	Z key + MB1 clicks + MB2, F key; sizes applied	differs	the book’s profile (an arc and stepped lines) is figure-only; a filleted rectangle stands in. The fillet radius is typed after picking in FreeCAD
F4	Specify Vector = Z axis, 0..360°, OK	axis 'Base Z-axis', MB2 = OK	same	volume 254722.5 mm^3, expected 254722.5; 1 solid(s)
F5	Dryer handle: Extrude (X), XY plane	X key, plane row + MB2	same	picked XY-plane (Base plane)
F6	Handle outline, seven dimensions	R key + 2 MB1 clicks + MB2; sizes applied	differs	the book’s handle (three inclined lines, seven dimensions) is figure-only; a 0.75 x 3.5 bar stands in
F7	Boolean Unite, End = 0.5, OK	'lengthEdit' = 12.7 mm, MB2 = OK	same	volume 273230.4 mm^3, expected 273230.4; 1 solid(s)
F8	Sketch on the YZ plane	ribbon 'Home › Direct Sketch > Sketch', plane row + MB2	same	picked YZ-plane (Base plane)
F9	Arc by centre and endpoints (180°), then a Line closing it	A key + 3 MB1 clicks + MB2, L key + 2 MB1 clicks + MB2; sizes applied	same	arc tool True, line tool True; the book projects the bottom edge first (shown in tutorial E); here the arc sits on the bottom line by its coordinates
F10	Reverse Direction, End 5.5, Boolean Unite, OK	sketch selected + ribbon 'Home › Feature > Extrude', 'checkBoxReversed' on, 'lengthEdit' = 139.7 mm, MB2 = OK	same	volume 324426.0 mm^3, expected 324425.9; 1 solid(s)
F11	Edge Blend, Circular, select the handle’s edges	4 edges selected + ribbon 'Home › Feature > Edge Blend'	differs	the book’s 13 edges are picked from a figure; the outer edges of the handle’s end stand in (FreeCAD’s unrefined shape may split one). FreeCAD takes the edges selected before the command
F12	Radius 1 = 0.15, OK	'filletRadius' = 3.81 mm, MB2 = OK	same	volume 324249.4 mm^3, expected 324249.3; 1 solid(s)
F13	Shell: pick the two flat open faces	bottom ['Face2'] + nozzle end ['Face9'] selected + ribbon 'Home › Feature > Shell'	same	FreeCAD calls Shell 'Thickness'
F14	Thickness 0.125, OK	'Value' = 3.175 mm, 'Make thickness inwards' on (default), MB2 = OK	limit	FreeCAD 1.1.4 does not shell the part after the edge blend (FreeCAD: 'Input error: Failed to make thick solid'); the same faces and thickness work before the blend (next steps). NX shells it in the book’s order
F15	Workaround: undo the shell and the blend	Ctrl+Z x2	differs	back to the part before the edge blend
F16	Workaround: Shell first, the same two faces	bottom ['Face10'] + nozzle end ['Face9'] selected + ribbon 'Home › Feature > Shell'	same	FreeCAD calls Shell 'Thickness'
F17	Thickness 0.125, OK (before the blend)	'Value' = 3.175 mm, 'Make thickness inwards' on (default), MB2 = OK	same	volume 75365.9 mm^3 (solid 324425.9); outer box kept True; 1.6 mm inside each wall is material [True, True, True, True], deeper in is hollow [True, True, True, True, True]
F18	Workaround: Edge Blend after the shell, the handle’s outer end edges	4 edges selected + ribbon 'Home › Feature > Edge Blend'	differs	the book’s 13 edges are picked from a figure; the outer edges of the handle’s end stand in (FreeCAD’s unrefined shape may split one). FreeCAD takes the edges selected before the command
F19	Radius 1 = 0.15, OK (after the shell)	'filletRadius' = 3.81 mm, MB2 = OK	limit	volume 75352.7 mm^3, 13.24 mm^3 rounded off; inside the previous box True; feature valid False; no Part API reference (it failed: class StdFail_NotDone BRep_API: command not done); FreeCAD 1.1.4 refuses this round on the shelled walls
F20	Workaround: Edge Blend again with a smaller radius	4 edges selected + ribbon 'Home › Feature > Edge Blend'	differs	the book’s 13 edges are picked from a figure; the outer edges of the handle’s end stand in (FreeCAD’s unrefined shape may split one). FreeCAD takes the edges selected before the command
F21	Radius 1 = 0.10, OK (after the shell)	'filletRadius' = 2.54 mm, MB2 = OK	differs	volume 75284.3 mm^3, expected 75284.3; 1 solid(s); the workaround changes the design: R0.10 instead of the book’s R0.15
F22	Pattern leader: Extrude on the top face, Subtract	select ['Face26'] + ribbon 'Home › Feature > Extrude (Subtract)'	differs	the book orients the view to Top first; FreeCAD’s sketch opens looking at the face
F23	Rectangle to the right of the CSYS: the small vent	R key + 2 MB1 clicks + MB2; sizes applied	same	the slot size is figure-only: 0.20 x 0.08 here
F24	Reverse Direction into the solid, End 0.15, OK	'lengthEdit' = 3.81 mm, MB2 = OK	same	volume 75251.5 mm^3, expected 75251.5; 1 solid(s); no Reverse needed: the subtracting extrude cuts inwards
F25	Pattern Feature, Layout = Linear, select the cut, MB2	leader selected + ribbon 'Home › Pattern > Pattern Feature'	differs	FreeCAD’s Linear Pattern is the Linear layout of NX’s Pattern Feature
F26	Direction 1: X, Count 5, Pitch -0.58; Use Direction 2: Y, Count 10, Pitch -0.25; OK	X axis {'axis': 'Base X-axis', 'mode': 'Spacing', 'count typed': 5, 'spacing': 0.58, 'reversed': True}; 'enableCheckbox'; Y axis {'axis': 'Base Y-axis', 'mode': 'Spacing', 'count typed': 10, 'spacing': 0.25, 'reversed': True}; MB2 = OK	same	volume 73645.6 mm^3, expected 73645.6; 1 solid(s); feature counts {'Occurrences': 5, 'Occurrences2': 10, 'Offset': 14.732, 'Offset2': 6.35, 'SpacingPattern': '[14.732]', 'SpacingPattern2': '[6.35]', 'Spacings': '[-1.0, -1.0, -1.0, -1.0]', 'Spacings2': '[-1.0, -1.0, -1.0, -1.0, -1.0, -1.0, -1.0, -1.0, -1.0]'}; NX’s negative pitch is FreeCAD’s spacing with Reverse
F27	Swept cut along the rim (section rectangle, Line-Arc guide), Subtract	-	skipped	the guide curves and section sizes are figure-only
F28	The finished part is shown in the graphics window	render of the graphics window	same	8.3% 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

Revolve, YZ plane of the datum CSYS

ribbon 'Home › Feature > Revolve', plane row + MB2

same

picked YZ-plane (Base plane)

Profile, then Fillet R0.25 between the top line and the side

Z key + MB1 clicks + MB2, F key; sizes applied

differs

the book’s profile (an arc and stepped lines) is figure-only; a filleted rectangle stands in. The fillet radius is typed after picking in FreeCAD

Specify Vector = Z axis, 0..360°, OK

axis 'Base Z-axis', MB2 = OK

same

volume 254722.5 mm^3, expected 254722.5; 1 solid(s)

Dryer handle: Extrude (X), XY plane

X key, plane row + MB2

same

picked XY-plane (Base plane)

Handle outline, seven dimensions

R key + 2 MB1 clicks + MB2; sizes applied

differs

the book’s handle (three inclined lines, seven dimensions) is figure-only; a 0.75 x 3.5 bar stands in

Boolean Unite, End = 0.5, OK

'lengthEdit' = 12.7 mm, MB2 = OK

same

volume 273230.4 mm^3, expected 273230.4; 1 solid(s)

Sketch on the YZ plane

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

same

picked YZ-plane (Base plane)

Arc by centre and endpoints (180°), then a Line closing it

A key + 3 MB1 clicks + MB2, L key + 2 MB1 clicks + MB2; sizes applied

same

arc tool True, line tool True; the book projects the bottom edge first (shown in tutorial E); here the arc sits on the bottom line by its coordinates

F10

Reverse Direction, End 5.5, Boolean Unite, OK

sketch selected + ribbon 'Home › Feature > Extrude', 'checkBoxReversed' on, 'lengthEdit' = 139.7 mm, MB2 = OK

same

volume 324426.0 mm^3, expected 324425.9; 1 solid(s)

F11

Edge Blend, Circular, select the handle’s edges

4 edges selected + ribbon 'Home › Feature > Edge Blend'

differs

the book’s 13 edges are picked from a figure; the outer edges of the handle’s end stand in (FreeCAD’s unrefined shape may split one). FreeCAD takes the edges selected before the command

F12

Radius 1 = 0.15, OK

'filletRadius' = 3.81 mm, MB2 = OK

same

volume 324249.4 mm^3, expected 324249.3; 1 solid(s)

F13

Shell: pick the two flat open faces

bottom ['Face2'] + nozzle end ['Face9'] selected + ribbon 'Home › Feature > Shell'

same

FreeCAD calls Shell 'Thickness'

F14

Thickness 0.125, OK

'Value' = 3.175 mm, 'Make thickness inwards' on (default), MB2 = OK

limit

FreeCAD 1.1.4 does not shell the part after the edge blend (FreeCAD: 'Input error: Failed to make thick solid'); the same faces and thickness work before the blend (next steps). NX shells it in the book’s order

F15

Workaround: undo the shell and the blend

Ctrl+Z x2

differs

back to the part before the edge blend

F16

Workaround: Shell first, the same two faces

bottom ['Face10'] + nozzle end ['Face9'] selected + ribbon 'Home › Feature > Shell'

same

FreeCAD calls Shell 'Thickness'

F17

Thickness 0.125, OK (before the blend)

'Value' = 3.175 mm, 'Make thickness inwards' on (default), MB2 = OK

same

volume 75365.9 mm^3 (solid 324425.9); outer box kept True; 1.6 mm inside each wall is material [True, True, True, True], deeper in is hollow [True, True, True, True, True]

F18

Workaround: Edge Blend after the shell, the handle’s outer end edges

4 edges selected + ribbon 'Home › Feature > Edge Blend'

differs

the book’s 13 edges are picked from a figure; the outer edges of the handle’s end stand in (FreeCAD’s unrefined shape may split one). FreeCAD takes the edges selected before the command

F19

Radius 1 = 0.15, OK (after the shell)

'filletRadius' = 3.81 mm, MB2 = OK

limit

volume 75352.7 mm^3, 13.24 mm^3 rounded off; inside the previous box True; feature valid False; no Part API reference (it failed: class StdFail_NotDone BRep_API: command not done); FreeCAD 1.1.4 refuses this round on the shelled walls

F20

Workaround: Edge Blend again with a smaller radius

4 edges selected + ribbon 'Home › Feature > Edge Blend'

differs

the book’s 13 edges are picked from a figure; the outer edges of the handle’s end stand in (FreeCAD’s unrefined shape may split one). FreeCAD takes the edges selected before the command

F21

Radius 1 = 0.10, OK (after the shell)

'filletRadius' = 2.54 mm, MB2 = OK

differs

volume 75284.3 mm^3, expected 75284.3; 1 solid(s); the workaround changes the design: R0.10 instead of the book’s R0.15

F22

Pattern leader: Extrude on the top face, Subtract

select ['Face26'] + ribbon 'Home › Feature > Extrude (Subtract)'

differs

the book orients the view to Top first; FreeCAD’s sketch opens looking at the face

F23

Rectangle to the right of the CSYS: the small vent

R key + 2 MB1 clicks + MB2; sizes applied

same

the slot size is figure-only: 0.20 x 0.08 here

F24

Reverse Direction into the solid, End 0.15, OK

'lengthEdit' = 3.81 mm, MB2 = OK

same

volume 75251.5 mm^3, expected 75251.5; 1 solid(s); no Reverse needed: the subtracting extrude cuts inwards

F25

Pattern Feature, Layout = Linear, select the cut, MB2

leader selected + ribbon 'Home › Pattern > Pattern Feature'

differs

FreeCAD’s Linear Pattern is the Linear layout of NX’s Pattern Feature

F26

Direction 1: X, Count 5, Pitch -0.58; Use Direction 2: Y, Count 10, Pitch -0.25; OK

X axis {'axis': 'Base X-axis', 'mode': 'Spacing', 'count typed': 5, 'spacing': 0.58, 'reversed': True}; 'enableCheckbox'; Y axis {'axis': 'Base Y-axis', 'mode': 'Spacing', 'count typed': 10, 'spacing': 0.25, 'reversed': True}; MB2 = OK

same

volume 73645.6 mm^3, expected 73645.6; 1 solid(s); feature counts {'Occurrences': 5, 'Occurrences2': 10, 'Offset': 14.732, 'Offset2': 6.35, 'SpacingPattern': '[14.732]', 'SpacingPattern2': '[6.35]', 'Spacings': '[-1.0, -1.0, -1.0, -1.0]', 'Spacings2': '[-1.0, -1.0, -1.0, -1.0, -1.0, -1.0, -1.0, -1.0, -1.0]'}; NX’s negative pitch is FreeCAD’s spacing with Reverse

F27

Swept cut along the rim (section rectangle, Line-Arc guide), Subtract

skipped

the guide curves and section sizes are figure-only

F28

The finished part is shown in the graphics window

render of the graphics window

same

8.3% 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.

FreeCAD limits met here

With the handle’s edges rounded first, as the book does, Shell fails in FreeCAD 1.1.4. Shell first, then round.
Rounding the handle’s outer edges at the book’s R3.81 mm on 3.175 mm walls fails; R2.54 mm works.
NX’s negative pitch is FreeCAD’s spacing with Reverse.

See Known issues.