Tutorial AN: Arbor Press Plate

Source	Ming C. Leu, Wenjin Tao, Amir Ghazanfari and Krishna Kolan, NX 12 for Engineering Design (Missouri University of Science and Technology), sections 4.2.1 (Model a Block), 4.3 (Reference Features) and 4.5.1 (General Hole). The book builds the plate in three visits; here they follow one another.
You learn	Block with Origin and Edge Lengths, Fit and Trimetric, Datum Plane at an offset, Datum Axis through two points, Hole with its points sketched on a face
Sizes	the book’s, in inches, typed in millimetres. A block 65 × 85 × 20 with its origin at (0, 0, 0). A datum plane 15 above the top face. Six simple holes Ø8, 25 deep with a 118° tip, at (11.25, 10), (32.5, 23.5), (53.75, 10), (11.25, 75), (32.5, 61.5) and (53.75, 75).

The book’s figure picks the datum axis’s points without coordinates: a bottom corner and the opposite top corner of the front face. Here they are (65, 0, 0) and (0, 0, 20), so the axis is the front face’s diagonal. The plate is 20 thick, so holes 25 deep go through it.

Step by step

1. The block

Ctrl+N, then Block (Home › Feature). In the Block dialog keep Origin and Edge Lengths, leave XC, YC and ZC at 0, and type Length 65, Width 85 and Height 20. Click OK.

Ctrl+F fits the view, and Home turns it to Trimetric (NX: MB3 > Orient View > Trimetric). Save the part as Arborpress_plate.

2. A datum plane and a datum axis

Select the block’s top face and choose Datum > Datum Plane. FreeCAD attaches the plane to the face; in the Dialog panel type 15 in the offset along Z and press MB2.

Select two corners of the block, here (65, 0, 0) and (0, 0, 20), and choose Datum > Datum Axis. FreeCAD takes the axis through the two points, as NX’s Inferred type does; press MB2.

The datum plane above the top face and the datum axis along the front face’s diagonal

3. The holes

Select the top face and click Hole. NX-Style starts a sketch on the face, which is NX’s Sketch Section in the Hole dialog’s Position group. Click Point (Sketch › Curve), then for each of the six points type XC and YC in the fields beside the pointer, pressing Enter after each. Press MB2, then Ctrl+Q.

The Hole dialog opens. Keep the simple hole, and type Diameter 8, Depth 25 and the tip angle 118°. Press MB2.

Save the part.

The replay

#	In the book (NX)	In FreeCAD NX-Style	Result	Notes
AN1	Create a new file (Arborpress_plate)	Ctrl+N, Model template	same	new document ['Unnamed']
AN2	Units in the New dialog (the book picks inches)	metric part kept; book sizes typed in mm	differs	FreeCAD sets units in Preferences, not in the New dialog; NXStyle defaults to millimetres (document: Standard (mm, kg, s, °); 25.4 mm shows as 25.40 mm)
AN3	Block: Origin and Edge Lengths, Point Dialog at (0, 0, 0), Length 65, Width 85, Height 20, OK	ribbon 'Home › Feature > Block', Type 'Origin and Edge Lengths', XC/YC/ZC 0 and the lengths typed (1651, 2159, 508 mm), OK	same	Boolean None; block 1651.0 x 2159.0 x 508.0 mm from (0, 0, 0); one undo step ['Block']. The Point Dialog’s XC, YC, ZC are fields in the Block dialog (NX opens it as its own window)
AN4	Fit (Ctrl+F), Orient View > Trimetric	Ctrl+F, Home (NX’s Trimetric key)	same	view direction (-0.4096, 0.7094, -0.5736) (trimetric 1.000000); all eight corners of the block in the window True
AN5	Save the part	file name given once by script (the system file dialog is not driven); a change, then the Ctrl+S key	same	Arborpress_plate.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
AN6	Datum Plane (Inferred): the top face of the block	top face (Face6) selected + ribbon 'Home > Datum > Datum Plane'	same	the plane is attached to the face; FreeCAD’s attachment dialog opens with it
AN7	Offset Distance 15, OK	'attachmentOffsetZ' = 381 mm, MB2 = OK	same	datum plane at z = 889.00 mm (top face 508 + 381), normal (0.0, 0.0, 1.0)
AN8	Datum Axis: the two points on the block	Vertex6 and Vertex1 selected + ribbon 'Home > Datum > Datum Axis'	same	FreeCAD infers Through Two Points from the two vertices, as NX’s Inferred does
AN9	OK: the Datum Axis is the diagonal	MB2 = OK	same	mode TwoPointLine; direction (-0.9558, 0.0, 0.2941) along the diagonal of the front face (65 x 20); through the first point within 6e-14 mm
AN10	Hole: General Hole, Position > Sketch on the top face	top face selected + ribbon 'Home › Feature > Hole'	same	the Hole starts a sketch on the face, and Finish Sketch carries on into the Hole dialog, as NX’s Sketch Section in the Position group
AN11	Point Dialog: the six points of the table, each OK	ribbon 'Sketch › Curve > Point', XC and YC typed in the on-view fields for each point, MB2	same	6 points; all at the table coordinates; sketch on the top face (z = 508.0 mm)
AN12	Simple Hole: Diameter 8, Depth 25, Tip Angle 118°, Boolean Subtract, OK	dialog open True; 'Diameter' = 203.2 mm, 'Dimension', 'Depth' = 635 mm, 'DrillPointAngle' = 118°, MB2 = OK	same	volume 1711926130.6 mm^3, expected 1711926130.6; 1 solid(s); the plate is 20 thick, so the holes go through it; values as typed True; FreeCAD’s Hole always subtracts from its body
AN13	The plate: the block with its six holes	compared with the book’s dimensions	same	same solid as the reference: 0 mm³ differ, box within 0 mm, 12 faces (12 in the reference)
AN14	Save the part	file name given once by script (the system file dialog is not driven); a change, then the Ctrl+S key	same	Arborpress_plate.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

AN1

Create a new file (Arborpress_plate)

Ctrl+N, Model template

same

new document ['Unnamed']

AN2

Units in the New dialog (the book picks inches)

metric part kept; book sizes typed in mm

differs

FreeCAD sets units in Preferences, not in the New dialog; NXStyle defaults to millimetres (document: Standard (mm, kg, s, °); 25.4 mm shows as 25.40 mm)

AN3

Block: Origin and Edge Lengths, Point Dialog at (0, 0, 0), Length 65, Width 85, Height 20, OK

ribbon 'Home › Feature > Block', Type 'Origin and Edge Lengths', XC/YC/ZC 0 and the lengths typed (1651, 2159, 508 mm), OK

same

Boolean None; block 1651.0 x 2159.0 x 508.0 mm from (0, 0, 0); one undo step ['Block']. The Point Dialog’s XC, YC, ZC are fields in the Block dialog (NX opens it as its own window)

AN4

Fit (Ctrl+F), Orient View > Trimetric

Ctrl+F, Home (NX’s Trimetric key)

same

view direction (-0.4096, 0.7094, -0.5736) (trimetric 1.000000); all eight corners of the block in the window True

AN5

Save the part

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

same

Arborpress_plate.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

AN6

Datum Plane (Inferred): the top face of the block

top face (Face6) selected + ribbon 'Home > Datum > Datum Plane'

same

the plane is attached to the face; FreeCAD’s attachment dialog opens with it

AN7

Offset Distance 15, OK

'attachmentOffsetZ' = 381 mm, MB2 = OK

same

datum plane at z = 889.00 mm (top face 508 + 381), normal (0.0, 0.0, 1.0)

AN8

Datum Axis: the two points on the block

Vertex6 and Vertex1 selected + ribbon 'Home > Datum > Datum Axis'

same

FreeCAD infers Through Two Points from the two vertices, as NX’s Inferred does

AN9

OK: the Datum Axis is the diagonal

MB2 = OK

same

mode TwoPointLine; direction (-0.9558, 0.0, 0.2941) along the diagonal of the front face (65 x 20); through the first point within 6e-14 mm

AN10

Hole: General Hole, Position > Sketch on the top face

top face selected + ribbon 'Home › Feature > Hole'

same

the Hole starts a sketch on the face, and Finish Sketch carries on into the Hole dialog, as NX’s Sketch Section in the Position group

AN11

Point Dialog: the six points of the table, each OK

ribbon 'Sketch › Curve > Point', XC and YC typed in the on-view fields for each point, MB2

same

6 points; all at the table coordinates; sketch on the top face (z = 508.0 mm)

AN12

Simple Hole: Diameter 8, Depth 25, Tip Angle 118°, Boolean Subtract, OK

dialog open True; 'Diameter' = 203.2 mm, 'Dimension', 'Depth' = 635 mm, 'DrillPointAngle' = 118°, MB2 = OK

same

volume 1711926130.6 mm^3, expected 1711926130.6; 1 solid(s); the plate is 20 thick, so the holes go through it; values as typed True; FreeCAD’s Hole always subtracts from its body

AN13

The plate: the block with its six holes

compared with the book’s dimensions

same

same solid as the reference: 0 mm³ differ, box within 0 mm, 12 faces (12 in the reference)

AN14

Save the part

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

same

Arborpress_plate.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 plate is compared with the book’s, built from its dimensions: the block less six holes through it.

What differs from NX

NX’s Point Dialog opens as its own window. In NX-Style’s Block dialog its XC, YC and ZC are fields of the dialog itself.
NX’s Datum Plane dialog offers the offset as soon as you pick the face. FreeCAD attaches the plane to the face and takes the offset as the attachment’s Z offset.
NX places a hole’s points with the Point Dialog in the hole’s sketch. FreeCAD’s Hole drills at the sketch’s points, and the points are typed in the on-view fields, which are NX’s XC and YC boxes.
FreeCAD’s Hole always subtracts from its body; NX’s Hole has a Boolean group.