Tutorial AU: Impeller, the solid

Source	Ming C. Leu, Wenjin Tao, Amir Ghazanfari and Krishna Kolan, NX 12 for Engineering Design (Missouri University of Science and Technology), section 4.7.5 (Impeller). It continues the blade sketch of section 3.5.3, tutorial AH.
You learn	Cone with a typed point and a vector, Extrude with Unite, Pattern Feature with a circular layout, Cylinder with Subtract
Sizes	the book’s, in inches, typed in millimetres. A cone along −XC from (14, 0, 0), Ø15 to Ø8, 16.25 long. The blade extruded 12 along ZC. Five blades, 72° apart about XC. A hole Ø4 × 16 into the large end and Ø0.275 × 0.25 into the small end.

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

Step by step

1. The cone

Open Impeller_impeller, the part of tutorial AH. Click Cone, keep Diameters and Height and choose −XC. Type the point (355.6, 0, 0) mm, which is (14, 0, 0) in. Then type Base Diameter 381, Top Diameter 203.2 and Height 412.75 mm (15, 8 and 16.25 in). Click OK.

2. The blade

Click Extrude and click one of the blade’s arcs: with the Curve Rule on Inferred Curves the pick takes the whole closed outline. Choose Unite, type 304.8 mm (12 in) and click OK.

3. Five blades

Select the Extrude and click Circular Pattern (Home › Pattern). Choose the X axis, 5 occurrences over 360° (72° apart), and press MB2.

4. The holes

Click Cylinder, choose −XC, type the point (14, 0, 0) in, and type Diameter 4 and Height 16. Choose Subtract, and click OK. Click Cylinder again, choose XC, type the point (−2.25, 0, 0) in at the small end, and type Diameter 0.275 and Height 0.25. Choose Subtract, and click OK.

The impeller: the cone with five blades and the hole in its end

Save the part.

The replay

#	In the book (NX)	In FreeCAD NX-Style	Result	Notes
AU1	Open Impeller_impeller (tutorial AH’s part)	File > Open (by script)	same	the blade sketch, 4 curves in a closed loop
AU2	Cone: Diameters and Height, -XC, Point Dialog (14, 0, 0), Base 15, Top 8, Height 16.25, OK	ribbon 'Home › Feature', Type 'Diameters and Height', Specify Vector '-XC', XC/YC/ZC 355.6/0/0 typed, Base 381, Top 203.2, Height 412.75 typed, Boolean 'None', OK	same	same solid as the reference: 0 mm³ differ, box within 5.7e-14 mm, 3 faces (3 in the reference); origin (355.6, 0.0, 0.0); one undo step ['Cone']
AU3	Extrude the airfoil 12 along ZC, Boolean Unite with the cone	ribbon 'Home › Feature > Extrude', a side picked (QuickPick; Curve Rule Inferred Curves), dialog opened True; Boolean 'Unite', 'lengthEdit' = 304.8 mm; OK clicked	same	same solid as the reference: 0 mm³ differ, box within 1.8e-13 mm, 8 faces (8 in the reference)
AU4	Pattern Feature: the blade, Circular, XC through the origin, Count 5, Pitch Angle 72, OK	the Extrude selected + ribbon 'Home › Pattern > Circular Pattern', axis 'Base X-axis', 'spinOccurrences' = 5 over 360° (72° apart), MB2 = OK	same	same solid as the reference: 0 mm³ differ, box within 1.8e-13 mm, 28 faces (28 in the reference)
AU5	Cylinder Ø4 x 16 into the cone’s large end, Subtract	ribbon 'Home › Feature', Type 'Axis, Diameter, and Height', Specify Vector '-XC', XC/YC/ZC 355.6/0/0 typed, Diameter 101.6 and Height 406.4 typed, Boolean 'Subtract', OK	same	same solid as the reference: 0 mm³ differ, box within 2.9e-13 mm, 30 faces (30 in the reference); origin (355.6, 0.0, 0.0); one undo step ['Cylinder']; with Body
AU6	Cylinder Ø0.275 x 0.25 into the cone’s small end, Subtract	ribbon 'Home › Feature', Type 'Axis, Diameter, and Height', Specify Vector 'XC', XC/YC/ZC -57.15/0/0 typed, Diameter 6.985 and Height 6.35 typed, Boolean 'Subtract', OK	same	same solid as the reference: 0 mm³ differ, box within 3.4e-13 mm, 31 faces (31 in the reference); origin (-57.15, 0.0, 0.0); one undo step ['Cylinder']; with Body
AU7	The impeller	compared with the book’s dimensions built by the Part API	same	same solid as the reference: 0 mm³ differ, box within 3.4e-13 mm, 31 faces (31 in the reference)
AU8	Save and close the part	file name given once by script (the system file dialog is not driven); a change, then the Ctrl+S key	same	Impeller_impeller.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

AU1

Open Impeller_impeller (tutorial AH’s part)

File > Open (by script)

same

the blade sketch, 4 curves in a closed loop

AU2

Cone: Diameters and Height, -XC, Point Dialog (14, 0, 0), Base 15, Top 8, Height 16.25, OK

ribbon 'Home › Feature', Type 'Diameters and Height', Specify Vector '-XC', XC/YC/ZC 355.6/0/0 typed, Base 381, Top 203.2, Height 412.75 typed, Boolean 'None', OK

same

same solid as the reference: 0 mm³ differ, box within 5.7e-14 mm, 3 faces (3 in the reference); origin (355.6, 0.0, 0.0); one undo step ['Cone']

AU3

Extrude the airfoil 12 along ZC, Boolean Unite with the cone

ribbon 'Home › Feature > Extrude', a side picked (QuickPick; Curve Rule Inferred Curves), dialog opened True; Boolean 'Unite', 'lengthEdit' = 304.8 mm; OK clicked

same

same solid as the reference: 0 mm³ differ, box within 1.8e-13 mm, 8 faces (8 in the reference)

AU4

Pattern Feature: the blade, Circular, XC through the origin, Count 5, Pitch Angle 72, OK

the Extrude selected + ribbon 'Home › Pattern > Circular Pattern', axis 'Base X-axis', 'spinOccurrences' = 5 over 360° (72° apart), MB2 = OK

same

same solid as the reference: 0 mm³ differ, box within 1.8e-13 mm, 28 faces (28 in the reference)

AU5

Cylinder Ø4 x 16 into the cone’s large end, Subtract

ribbon 'Home › Feature', Type 'Axis, Diameter, and Height', Specify Vector '-XC', XC/YC/ZC 355.6/0/0 typed, Diameter 101.6 and Height 406.4 typed, Boolean 'Subtract', OK

same

same solid as the reference: 0 mm³ differ, box within 2.9e-13 mm, 30 faces (30 in the reference); origin (355.6, 0.0, 0.0); one undo step ['Cylinder']; with Body

AU6

Cylinder Ø0.275 x 0.25 into the cone’s small end, Subtract

ribbon 'Home › Feature', Type 'Axis, Diameter, and Height', Specify Vector 'XC', XC/YC/ZC -57.15/0/0 typed, Diameter 6.985 and Height 6.35 typed, Boolean 'Subtract', OK

same

same solid as the reference: 0 mm³ differ, box within 3.4e-13 mm, 31 faces (31 in the reference); origin (-57.15, 0.0, 0.0); one undo step ['Cylinder']; with Body

AU7

The impeller

compared with the book’s dimensions built by the Part API

same

same solid as the reference: 0 mm³ differ, box within 3.4e-13 mm, 31 faces (31 in the reference)

AU8

Save and close the part

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

same

Impeller_impeller.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.

Each step is compared with the book’s dimensions built by FreeCAD’s Part API.

What differs from NX

NX has one Pattern Feature with a Layout list. FreeCAD has separate buttons; the circular one is Circular Pattern.
The book places the two holes "on the side" of the cone. Here their points are typed at the cone’s two ends.