Tutorial AO: Impeller Lower Casing, Extrude and Revolve

Source	Ming C. Leu, Wenjin Tao, Amir Ghazanfari and Krishna Kolan, NX 12 for Engineering Design (Missouri University of Science and Technology), section 4.4 (Swept Features). It continues the casing sketch of section 3.5.2, tutorial AG; tutorial AX turns it into the upper casing.
You learn	the Curve Rule (Single Curve), Revolve with Specify Vector, Specify Point and the angle limits, Extrude of picked curves as a body of its own, QuickPick for curves that lie on a solid, Mirror Feature
Sizes	the book’s, in inches, typed in millimetres. The wall and the flange revolved about XC through (0, 0, 0) from 0 to 180°. The edge extruded 0.5 (12.7 mm) along -ZC.

The replay runs tutorial AG first and opens the part it saved.

Step by step

1. The wall

Open Impeller_lower_casing, the part of tutorial AG. Click Revolve. FreeCAD first offers its list of sketch planes; you don’t need it, because picking a curve of the sketch closes the list and opens the Revolve dialog with that curve.

Set the Curve Rule on the Top Border Bar (beside the Selection Filter) to Single Curve. The default, Inferred Curves, would take the whole sketch, which is not one closed profile. Click the 10 curves of the wall: the inner curve’s four, the four of the curve 0.5 above it, and the two short lines that close its ends.

In the dialog choose XC in Specify Vector, keep Specify Point at (0, 0, 0), and type Start 0 and End 180. Click OK.

2. The edge

Click Extrude, keep Single Curve, and click the 10 curves of the edge: the inner curve’s four again, the four of the curve 1.5 below it, and the two lines that close its ends. Most of these curves now lie on a face or an edge of the wall as well. Press and hold MB1 on the curve, as the book’s note says, and choose the sketch curve in QuickPick.

Keep Boolean None. Type 12.7 mm (0.5 in) as the length and tick Reversed in FreeCAD’s panel, which turns the extrusion to -ZC. Click OK.

The edge becomes a body of its own. With Unite it would touch the wall only along a line, which would leave two solids in one body, so the dialog does not allow it.

The edge extruded down from the sketch plane

3. The edge on the other side

Make the edge’s body the work body, select its Extrude in the Part Navigator, and click Mirror Feature (Home › Pattern). Choose the plane XZ, the plane through the casing’s centre line, and press MB2.

The edge mirrored to the other side of the casing

4. The flange

Click Revolve again and, with Single Curve, click the 4 sides of the flange at the casing’s smaller opening. Two of them lie on lines of the wall and of the edge: QuickPick lists both, and you choose the flange’s. Choose XC, keep (0, 0, 0), and type Start 0 and End 180. The Boolean is Unite, with the wall, by itself; click OK.

Save the part.

The replay

#	In the book (NX)	In FreeCAD NX-Style	Result	Notes
AO1	Open Impeller_lower_casing (tutorial AG’s part)	File > Open (by script)	same	the sketch with 19 of the 19 curves of the book’s figure; shown True
AO2	Revolve, Selection Filter Single Curve, the 10 curves of the wall	ribbon 'Home › Feature > Revolve' (FreeCAD asks for a plane: True), Curve Rule 'Single Curve', MB1 on each curve: 10 by click	same	the section holds 10 curves, the wall’s True; the first pick closes FreeCAD’s plane list and opens the dialog with it
AO3	Axis: Specify Vector XC, Specify Point (0, 0, 0); Start 0, End 180	'XC' chosen, X, Y, Z and the angles typed in the box	same	axis {'vector': 'XC', 'point': (0.0, 0.0, 0.0)}, limits (0.0, 180.0)
AO4	OK: the revolved wall	OK clicked	same	volume 10035706.5 mm^3, expected 10035706.5; 1 solid(s); Profile the 10 curves True; below the sketch plane True; one undo step True (['Revolve'])
AO5	Extrude, Single Curve, the outer curves of the casing (its edge)	ribbon 'Home › Feature > Extrude' (plane asked: True), Curve Rule 'Single Curve', MB1 on each curve: 9 by QuickPick, 1 by click	same	the section holds 10 curves, the edge’s True; where a curve lies on the wall’s face, QuickPick lists it (the book’s note: press and hold MB1)
AO6	Extrude it 0.5 in along -ZC, OK	Boolean 'None' in the box; 'lengthEdit' = 12.7 mm and Reversed clicked (True) in FreeCAD’s panel; OK clicked	same	volume 381783.6 mm^3, expected 381783.6; z -12.70 to 0.00 mm; its own body (2 bodies): with Unite it would touch the wall only along a line, two solids in one body, so the edge is a body of its own, as the book’s Solid Body filter in the next step shows
AO7	Mirror the edge through the centre plane, Copy	the edge’s body made the work body and its Extrude selected (Part Navigator) + ribbon 'Home › Pattern > Mirror Feature', plane 'Base XZ-plane', MB2 = OK	differs	the edge’s body holds 2 solids, 763567.1 mm^3 (twice 381783.6), symmetric about XZ (y -419.1 to 419.1 mm). NX’s Edit > Transform copies the solid unparametrised; Mirror Feature keeps the copy following the edge
AO8	Revolve, Single Curve, the 4 curves of the flange	ribbon 'Home › Feature > Revolve' (plane asked: True), Curve Rule 'Single Curve', MB1 on each curve: 4 by QuickPick	same	the section holds 4 curves, the flange’s True; two of them lie on the wall’s and the edge’s lines, and QuickPick tells them apart
AO9	XC through the origin, Start 0, End 180, as for the casing	'XC', X, Y, Z and the angles typed; Boolean Unite by itself	same	axis {'vector': 'XC', 'point': (0.0, 0.0, 0.0)}, limits (0.0, 180.0), Boolean unite
AO10	OK: the flange, united with the wall	OK clicked	same	volume 10377414.8 mm^3, expected 10377414.8; 1 solid(s); the flange’s volume added to the wall’s
AO11	The lower casing: the wall with its flange, the edge on both sides	compared with the book’s curves revolved and extruded by the Part API	same	wall and flange: same solid as the reference: 0 mm³ differ, box within 0 mm, 14 faces (14 in the reference); edges: same solid as the reference: 0 mm³ differ, box within 0 mm, 24 faces (24 in the reference)
AO12	Save the model	file name given once by script (the system file dialog is not driven); a change, then the Ctrl+S key	same	Impeller_lower_casing.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

AO1

Open Impeller_lower_casing (tutorial AG’s part)

File > Open (by script)

same

the sketch with 19 of the 19 curves of the book’s figure; shown True

AO2

Revolve, Selection Filter Single Curve, the 10 curves of the wall

ribbon 'Home › Feature > Revolve' (FreeCAD asks for a plane: True), Curve Rule 'Single Curve', MB1 on each curve: 10 by click

same

the section holds 10 curves, the wall’s True; the first pick closes FreeCAD’s plane list and opens the dialog with it

AO3

Axis: Specify Vector XC, Specify Point (0, 0, 0); Start 0, End 180

'XC' chosen, X, Y, Z and the angles typed in the box

same

axis {'vector': 'XC', 'point': (0.0, 0.0, 0.0)}, limits (0.0, 180.0)

AO4

OK: the revolved wall

OK clicked

same

volume 10035706.5 mm^3, expected 10035706.5; 1 solid(s); Profile the 10 curves True; below the sketch plane True; one undo step True (['Revolve'])

AO5

Extrude, Single Curve, the outer curves of the casing (its edge)

ribbon 'Home › Feature > Extrude' (plane asked: True), Curve Rule 'Single Curve', MB1 on each curve: 9 by QuickPick, 1 by click

same

the section holds 10 curves, the edge’s True; where a curve lies on the wall’s face, QuickPick lists it (the book’s note: press and hold MB1)

AO6

Extrude it 0.5 in along -ZC, OK

Boolean 'None' in the box; 'lengthEdit' = 12.7 mm and Reversed clicked (True) in FreeCAD’s panel; OK clicked

same

volume 381783.6 mm^3, expected 381783.6; z -12.70 to 0.00 mm; its own body (2 bodies): with Unite it would touch the wall only along a line, two solids in one body, so the edge is a body of its own, as the book’s Solid Body filter in the next step shows

AO7

Mirror the edge through the centre plane, Copy

the edge’s body made the work body and its Extrude selected (Part Navigator) + ribbon 'Home › Pattern > Mirror Feature', plane 'Base XZ-plane', MB2 = OK

differs

the edge’s body holds 2 solids, 763567.1 mm^3 (twice 381783.6), symmetric about XZ (y -419.1 to 419.1 mm). NX’s Edit > Transform copies the solid unparametrised; Mirror Feature keeps the copy following the edge

AO8

Revolve, Single Curve, the 4 curves of the flange

ribbon 'Home › Feature > Revolve' (plane asked: True), Curve Rule 'Single Curve', MB1 on each curve: 4 by QuickPick

same

the section holds 4 curves, the flange’s True; two of them lie on the wall’s and the edge’s lines, and QuickPick tells them apart

AO9

XC through the origin, Start 0, End 180, as for the casing

'XC', X, Y, Z and the angles typed; Boolean Unite by itself

same

axis {'vector': 'XC', 'point': (0.0, 0.0, 0.0)}, limits (0.0, 180.0), Boolean unite

AO10

OK: the flange, united with the wall

OK clicked

same

volume 10377414.8 mm^3, expected 10377414.8; 1 solid(s); the flange’s volume added to the wall’s

AO11

The lower casing: the wall with its flange, the edge on both sides

compared with the book’s curves revolved and extruded by the Part API

same

wall and flange: same solid as the reference: 0 mm³ differ, box within 0 mm, 14 faces (14 in the reference); edges: same solid as the reference: 0 mm³ differ, box within 0 mm, 24 faces (24 in the reference)

AO12

Save the model

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

same

Impeller_lower_casing.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 finished casing is compared with the book’s curves revolved and extruded by FreeCAD’s Part API: the wall with its flange, and the edge on both sides.

What differs from NX

NX’s Revolve and Extrude start with the Section selection. In FreeCAD a feature without a sketch first offers the sketch planes; picking a curve instead closes that list.
NX’s Extrude limits give the direction. Here the length and the direction are set in FreeCAD’s panel under the NX dialog: 12.7 mm with Reversed is NX’s 0.5 in along -ZC.
The book mirrors the edge with Edit > Transform > Mirror Through a Plane and Copy, which makes an unparametrised copy. NX-Style uses Mirror Feature, so the copy follows the edge when it changes.
Mirror Feature mirrors a feature inside its body: the edge’s body then holds both edges, two separate solids.