Tutorial AE: One Extrude, every way

Source	Our design. It is the acceptance case of NX-Style’s Extrude command (Extrude), not a book exercise
You learn	the Extrude dialog’s Boolean list, what Cancel and Esc leave behind (nothing), one undo step per command, Edit Parameters from the MB3 menu and the ribbon
Sizes	a 40 × 30 × 20 block; an 8 mm radius boss 10 high on top; an 8 × 6 pocket 5 deep in the top; a separate 6 mm radius cylinder 15 long, 100 mm away

Step by step

1. The block: Boolean None (a new body)

Ctrl+N, then X with nothing selected. Pick the XC-YC plane and draw a 40 × 30 rectangle from the origin (R). Ctrl+Q opens the Extrude dialog. The part has no solid yet, so the Boolean is None: a new body. Type 20 for the distance and press MB2.

2. The boss: Unite

Select the top face and press X. The sketch opens on the face. Draw an 8 mm radius circle in the middle (O) and press Ctrl+Q. The Boolean is now Unite, because the part has a solid. Intersect is in the list but greyed out. Choosing it anyway changes nothing, and the dialog says why. Type 10 and press MB2.

3. The pocket: Subtract

Select the top face again and press X. Draw an 8 × 6 rectangle near a corner, then Ctrl+Q. Choose Subtract in the Boolean list. The preview changes from adding material to cutting it, and no undo step is added. Type 5 and press MB2. The pocket cuts into the part.

4. A separate body: Boolean None

X with nothing selected. Pick the XC-ZC plane and draw a 6 mm radius circle 100 mm from the part. The Boolean Unite is inferred, but the circle misses the part. The dialog shows the error and OK is unavailable, so MB2 does nothing. Choose None, type 15 and press MB2. The cylinder is a second Body. The first one is unchanged.

5. Edit, Cancel, edit, OK

MB3 on the first extrude in the Part Navigator, then Edit Parameters. Type 35: the preview grows. Press Cancel. The distance is 20 again, and the undo list is unchanged. Select the extrude again and click Edit Parameters on the ribbon. Type 25 and press MB2. The boss and the pocket move up with the top face. This edit is one undo step, Edit Extrude.

6. Undo, Redo, reopen

Ctrl+Z takes back the edit. A second Ctrl+Z takes back the whole new-body extrude: the Body, its binder and the Pad go together. Ctrl+Y twice brings both back.

Type Extrude (Subtract) into the Command Finder and press Enter. The plane pick appears; Cancel it. Nothing is added to the part or to the undo list.

Save (Ctrl+S), close and reopen the part. Then Edit Parameters on the pocket: the Boolean reads Subtract. Type 12 and press Esc, which leaves the pocket as it was.

The replay

#	In the book (NX)	In FreeCAD NX-Style	Result	Notes
AE1	File > New (Ctrl+N), Model template	Ctrl+N	same	new document ['Unnamed']
AE2	Extrude (X) with nothing selected, pick the XC-YC plane	X key, plane row + MB2	same	picked XY-plane (Base plane); command controller started: True
AE3	Rectangle ® 40 x 30 from the origin, MB2	R key + 2 MB1 clicks + MB2; sizes applied	same	tool True; 4 curves; ended True
AE4	Finish Sketch: the Extrude dialog, Boolean inferred None (New Body)	Ctrl+Q; the NX command box above FreeCAD’s Pad panel	same	Boolean 'None' (list enabled True); Intersect offered but disabled True; status 'None (a new body): ready (OK or MB2 commits one undo step)'; OK enabled True; not supported shown: True
AE5	End = Value 20, OK	'lengthEdit' = 20 mm, MB2 = OK	same	same solid as the reference: 0 mm³ differ, box within 0 mm, 6 faces (6 in the reference); controller: committed new_body, undo step 'Extrude', 1 step(s) added
AE6	Top face selected, Extrude (X): circle 8 mm radius	select face + X; O key + 2 MB1 clicks + MB2; size applied	same	sketch on [(<PartDesign::Pad>, ('Face6',))]
AE7	Boolean inferred Unite (the part has a solid)	the NX command box	same	Boolean 'Unite'; status 'Unite: ready (OK or MB2 commits one undo step)'; OK True
AE8	Boolean Intersect	chose 'Intersect' in the Boolean list	differs	refused in the panel, not approximated: 'Intersect refused: Intersect is not offered: PartDesign has no intersecting extrude, and NX-Style does not approximate it.'; Boolean back to 'Unite', the Pad unchanged True
AE9	End = Value 10, Boolean Unite, OK	'lengthEdit' = 10 mm, MB2 = OK	same	same solid as the reference: 0 mm³ differ, box within 0 mm, 8 faces (8 in the reference); controller: committed unite, undo step 'Extrude', 1 step(s) added
AE10	Top face, Extrude (X): rectangle 8 x 6 near the corner	select face + X; R key + 2 MB1 clicks + MB2; sizes applied	same	tool True; 4 curves
AE11	Boolean Subtract (was inferred Unite)	'Subtract' in the Boolean list	same	Boolean 'Unite' → 'Subtract'; the preview Pad replaced by a Pocket (2 Pads left), no undo step added (0); status 'Subtract: ready (OK or MB2 commits one undo step)'
AE12	End = Value 5 into the part, OK	'lengthEdit' = 5 mm, MB2 = OK	same	same solid as the reference: 0 mm³ differ, box within 0 mm, 13 faces (13 in the reference); controller: committed subtract, undo step 'Extrude', 1 step(s) added; Subtract cuts against the sketch normal unless Reversed (NX keeps the direction and you reverse it)
AE13	Extrude (X), pick the XC-ZC plane (Type Filter set to Edge before)	X key, plane row + MB2	same	picked XZ-plane (Base plane); Type Filter during the command: 'Edge', gate None, enabled False
AE14	Circle 6 mm radius, 100 mm from the part	O key + 2 MB1 clicks + MB2; size applied	same	tool True; 1 curves
AE15	Inferred Unite with a section that misses the part; MB2	MB2 = OK	same	error shown: 'Unite would leave a separate solid: the extrusion does not touch the part (choose None for a new body)'; OK enabled False; dialog still open after MB2 True (NX: 'tool body does not intersect the target')
AE16	Boolean None (a new body)	'None' in the Boolean list	same	bodies ['Body', 'Body001']; status 'None (a new body): ready (OK or MB2 commits one undo step)'; OK True
AE17	End = Value 15, Boolean None (a new body), OK	'lengthEdit' = 15 mm, MB2 = OK	same	new body Body001: same solid as the reference: 0 mm³ differ, box within 0 mm, 3 faces (3 in the reference); the first body unchanged: same solid as the reference: 0 mm³ differ, box within 0 mm, 13 faces (13 in the reference); controller: committed new_body, undo step 'Extrude', 1 step(s) added; made of ['SubShapeBinder', 'Pad']; active Body still Body; Type Filter afterwards 'Edge', gate edge, enabled True
AE18	MB3 on the first Extrude in the Part Navigator > Edit Parameters	MB3 menu entry	same	menu entries ['Edit Pad', 'Set Face Colors', 'Suppressed', 'Set Tip', 'Move Object To…', 'Move Feature After…', 'Toggle Freeze', 'Placement', 'Edit Parameters', 'Toggle Visibility', 'Show Selection', 'Hide Selection']; panel open True; Boolean 'None' locked True (changing it would replace the feature)
AE19	Preview 35 mm, then Cancel	'lengthEdit' = 35 mm, Cancel button	same	preview showed Length 35 mm (top at 35 mm); after Cancel Length 20 mm, same solid as the reference: 0 mm³ differ, box within 0 mm, 13 faces (13 in the reference); undo steps added 0; objects left to recompute []
AE20	Design change: Edit Parameters, End 20 → 25, OK	ribbon 'Home › Edit Feature > Edit Parameters' (panel True), 'lengthEdit' = 25 mm, MB2 = OK	same	same solid as the reference: 0 mm³ differ, box within 0 mm, 13 faces (13 in the reference); the boss and the pocket follow the top face; the separate body unchanged True; controller: committed new_body, undo step 'Edit Extrude', 1 step(s) added
AE21	Undo (Ctrl+Z) twice, Redo (Ctrl+Y) twice	Ctrl+Z, Ctrl+Z, Ctrl+Y, Ctrl+Y	same	first undo takes back the edit (same solid as the reference: 0 mm³ differ, box within 0 mm, 13 faces (13 in the reference)); the second the whole New Body extrude (1 body left, binders left []); redo restores both (same solid as the reference: 0 mm³ differ, box within 0 mm, 13 faces (13 in the reference); cylinder True)
AE22	Command Finder: 'Extrude (Subtract)', Enter; Cancel the plane pick	typed into the Command Finder + Enter; Cancel button	same	command started True (Boolean asked: None); ended cancelled: no section: the plane pick was cancelled; objects +0, undo steps +0
AE23	Save (Ctrl+S)	file name given once by script (the system file dialog is not driven); a change, then the Ctrl+S key	same	ExtrudeAE.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
AE24	Reopen the part	close, File > Open (by script)	same	part: same solid as the reference: 0 mm³ differ, box within 0 mm, 13 faces (13 in the reference); cylinder: same solid as the reference: 0 mm³ differ, box within 3.6e-15 mm, 3 faces (3 in the reference); Extrudes read back as ['new_body', 'unite', 'subtract', 'new_body']
AE25	Reopened part: Edit Parameters on the pocket, 12 mm, Esc	ribbon 'Home › Edit Feature', typed 12, Esc	same	Boolean read back 'Subtract'; after Esc depth 5 mm, same solid as the reference: 0 mm³ differ, box within 0 mm, 13 faces (13 in the reference); undo steps added 0

In the book (NX)

In FreeCAD NX-Style

Result

Notes

AE1

File > New (Ctrl+N), Model template

Ctrl+N

same

new document ['Unnamed']

AE2

Extrude (X) with nothing selected, pick the XC-YC plane

X key, plane row + MB2

same

picked XY-plane (Base plane); command controller started: True

AE3

Rectangle ® 40 x 30 from the origin, MB2

R key + 2 MB1 clicks + MB2; sizes applied

same

tool True; 4 curves; ended True

AE4

Finish Sketch: the Extrude dialog, Boolean inferred None (New Body)

Ctrl+Q; the NX command box above FreeCAD’s Pad panel

same

Boolean 'None' (list enabled True); Intersect offered but disabled True; status 'None (a new body): ready (OK or MB2 commits one undo step)'; OK enabled True; not supported shown: True

AE5

End = Value 20, OK

'lengthEdit' = 20 mm, MB2 = OK

same

same solid as the reference: 0 mm³ differ, box within 0 mm, 6 faces (6 in the reference); controller: committed new_body, undo step 'Extrude', 1 step(s) added

AE6

Top face selected, Extrude (X): circle 8 mm radius

select face + X; O key + 2 MB1 clicks + MB2; size applied

same

sketch on [(<PartDesign::Pad>, ('Face6',))]

AE7

Boolean inferred Unite (the part has a solid)

the NX command box

same

Boolean 'Unite'; status 'Unite: ready (OK or MB2 commits one undo step)'; OK True

AE8

Boolean Intersect

chose 'Intersect' in the Boolean list

differs

refused in the panel, not approximated: 'Intersect refused: Intersect is not offered: PartDesign has no intersecting extrude, and NX-Style does not approximate it.'; Boolean back to 'Unite', the Pad unchanged True

AE9

End = Value 10, Boolean Unite, OK

'lengthEdit' = 10 mm, MB2 = OK

same

same solid as the reference: 0 mm³ differ, box within 0 mm, 8 faces (8 in the reference); controller: committed unite, undo step 'Extrude', 1 step(s) added

AE10

Top face, Extrude (X): rectangle 8 x 6 near the corner

select face + X; R key + 2 MB1 clicks + MB2; sizes applied

same

tool True; 4 curves

AE11

Boolean Subtract (was inferred Unite)

'Subtract' in the Boolean list

same

Boolean 'Unite' → 'Subtract'; the preview Pad replaced by a Pocket (2 Pads left), no undo step added (0); status 'Subtract: ready (OK or MB2 commits one undo step)'

AE12

End = Value 5 into the part, OK

'lengthEdit' = 5 mm, MB2 = OK

same

same solid as the reference: 0 mm³ differ, box within 0 mm, 13 faces (13 in the reference); controller: committed subtract, undo step 'Extrude', 1 step(s) added; Subtract cuts against the sketch normal unless Reversed (NX keeps the direction and you reverse it)

AE13

Extrude (X), pick the XC-ZC plane (Type Filter set to Edge before)

X key, plane row + MB2

same

picked XZ-plane (Base plane); Type Filter during the command: 'Edge', gate None, enabled False

AE14

Circle 6 mm radius, 100 mm from the part

O key + 2 MB1 clicks + MB2; size applied

same

tool True; 1 curves

AE15

Inferred Unite with a section that misses the part; MB2

MB2 = OK

same

error shown: 'Unite would leave a separate solid: the extrusion does not touch the part (choose None for a new body)'; OK enabled False; dialog still open after MB2 True (NX: 'tool body does not intersect the target')

AE16

Boolean None (a new body)

'None' in the Boolean list

same

bodies ['Body', 'Body001']; status 'None (a new body): ready (OK or MB2 commits one undo step)'; OK True

AE17

End = Value 15, Boolean None (a new body), OK

'lengthEdit' = 15 mm, MB2 = OK

same

new body Body001: same solid as the reference: 0 mm³ differ, box within 0 mm, 3 faces (3 in the reference); the first body unchanged: same solid as the reference: 0 mm³ differ, box within 0 mm, 13 faces (13 in the reference); controller: committed new_body, undo step 'Extrude', 1 step(s) added; made of ['SubShapeBinder', 'Pad']; active Body still Body; Type Filter afterwards 'Edge', gate edge, enabled True

AE18

MB3 on the first Extrude in the Part Navigator > Edit Parameters

MB3 menu entry

same

menu entries ['Edit Pad', 'Set Face Colors', 'Suppressed', 'Set Tip', 'Move Object To…', 'Move Feature After…', 'Toggle Freeze', 'Placement', 'Edit Parameters', 'Toggle Visibility', 'Show Selection', 'Hide Selection']; panel open True; Boolean 'None' locked True (changing it would replace the feature)

AE19

Preview 35 mm, then Cancel

'lengthEdit' = 35 mm, Cancel button

same

preview showed Length 35 mm (top at 35 mm); after Cancel Length 20 mm, same solid as the reference: 0 mm³ differ, box within 0 mm, 13 faces (13 in the reference); undo steps added 0; objects left to recompute []

AE20

Design change: Edit Parameters, End 20 → 25, OK

ribbon 'Home › Edit Feature > Edit Parameters' (panel True), 'lengthEdit' = 25 mm, MB2 = OK

same

same solid as the reference: 0 mm³ differ, box within 0 mm, 13 faces (13 in the reference); the boss and the pocket follow the top face; the separate body unchanged True; controller: committed new_body, undo step 'Edit Extrude', 1 step(s) added

AE21

Undo (Ctrl+Z) twice, Redo (Ctrl+Y) twice

Ctrl+Z, Ctrl+Z, Ctrl+Y, Ctrl+Y

same

first undo takes back the edit (same solid as the reference: 0 mm³ differ, box within 0 mm, 13 faces (13 in the reference)); the second the whole New Body extrude (1 body left, binders left []); redo restores both (same solid as the reference: 0 mm³ differ, box within 0 mm, 13 faces (13 in the reference); cylinder True)

AE22

Command Finder: 'Extrude (Subtract)', Enter; Cancel the plane pick

typed into the Command Finder + Enter; Cancel button

same

command started True (Boolean asked: None); ended cancelled: no section: the plane pick was cancelled; objects +0, undo steps +0

AE23

Save (Ctrl+S)

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

same

ExtrudeAE.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

AE24

Reopen the part

close, File > Open (by script)

same

part: same solid as the reference: 0 mm³ differ, box within 0 mm, 13 faces (13 in the reference); cylinder: same solid as the reference: 0 mm³ differ, box within 3.6e-15 mm, 3 faces (3 in the reference); Extrudes read back as ['new_body', 'unite', 'subtract', 'new_body']

AE25

Reopened part: Edit Parameters on the pocket, 12 mm, Esc

ribbon 'Home › Edit Feature', typed 12, Esc

same

Boolean read back 'Subtract'; after Esc depth 5 mm, same solid as the reference: 0 mm³ differ, box within 0 mm, 13 faces (13 in the reference); undo steps added 0

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 solid is compared with the same solid built with FreeCAD’s Part API (nxstyle/geomcheck.py). Equal volume alone would not show that a pocket is in the wrong place.

What differs from NX

The dialog has two parts: the NX command box (section, body, Boolean, errors) above FreeCAD’s own Pad or Pocket panel (limits, direction, draft).
Subtract cuts into the part by default. NX keeps the sketch normal for every Boolean, so there you reverse the direction.
Unite and Subtract work on the Body that holds the sketch. NX lets you pick the target body.
A sketch made inside Extrude stays as its own undo steps. Undoing the extrude leaves the sketch.