Tutorial H: GD&T plate drawing

Book	Cogorno, Geometric Dimensioning and Tolerancing for Mechanical Design, 3rd ed., ch. 12.2 and ch. 8 (Prob. 12-3)
You learn	Datum Feature Symbol, Feature Control Frame, basic dimensions, a hole note with limits, the ASME standard
Sizes	A 101.6 × 101.6 × 12.7 mm plate (its size is in a figure only) with 4X Ø12.954–13.716 holes; basic 25.4 and 50.8 mm from B and C. The book’s inch values are converted exactly: Ø0.254 position, 0.102 perpendicularity, 0.051 flatness.

In short

Ctrl+Shift+D, New Sheet; set Preferences › TechDraw › Dimensions › Standard and Style to ASME Inlined.
Base View of the plate’s face; a second Base View for its edge.
A cosmetic vertex on each hole centre, then Horizontal and Vertical dimensions; tick Theoretical Exact for basic ones.
Diameter on a hole: 4X and ±0.381 in its properties.
Select an edge, Datum Feature Symbol: A on the back face, B on the bottom edge, C on the left edge.
Feature Control Frame: flatness 0.051 on A; perpendicularity 0.102 to A on B; position Ø0.254 at MMC to A|B|C under the hole note.

Step by step

#	In the book (NX)	In FreeCAD NX-Style	Result	Notes
H1	The plate: 101.6 x 101.6 x 12.7 mm, 4 holes on a 50.8 mm square	modelled by script (the exercise is the drawing)	same	volume 124001.7 mm^3; back face (z = 0) is datum A, bottom edge (y = 0) B, left edge (x = 0) C
H2	File > Drafting, New Sheet	Ctrl+Shift+D + ribbon 'Home › Drawing > New Sheet'	same
H3	Drafting Preferences: ASME standard	Preferences > TechDraw > Dimensions > Standard and Style = ASME Inlined	differs	was ISO Oriented; NX sets the drafting standard in Drafting Preferences
H4	Base View: the plate’s face, scale 1:1	body selected + ribbon 'Home › View > Base View', MB2 on the sheet	same	direction set to look at the face (the book’s front view)
H5	Projected view to the right: the plate’s edge, back face A	second Base View, MB2	differs	as in tutorial D, a second Base View stands in for a view projected off the base view
H6	Arc centres for the dimensions	cosmetic vertex on each hole centre	differs	4 holes, 4 cosmetic vertices, found as ['Vertex6', 'Vertex9', 'Vertex12', 'Vertex15']; NX snaps dimensions to arc centres, TechDraw needs vertices there first
H7	Basic dimension 25.4 (C to the hole)	two vertices + ribbon 'Home › Dimension > Horizontal', then basic	differs	measured 25.4; NX: Basic is a Tolerance type in the dimension dialog, TechDraw: the Theoretical Exact property draws the box
H8	Basic dimension 50.8 (hole spacing)	two vertices + ribbon 'Home › Dimension > Horizontal', then basic	differs	measured 50.800000000000004; NX: Basic is a Tolerance type in the dimension dialog, TechDraw: the Theoretical Exact property draws the box
H9	Basic dimension 25.4 (B to the hole)	two vertices + ribbon 'Home › Dimension > Vertical', then basic	differs	measured 25.4; NX: Basic is a Tolerance type in the dimension dialog, TechDraw: the Theoretical Exact property draws the box
H10	Basic dimension 50.8 (hole spacing)	two vertices + ribbon 'Home › Dimension > Vertical', then basic	differs	measured 50.800000000000004; NX: Basic is a Tolerance type in the dimension dialog, TechDraw: the Theoretical Exact property draws the box
H11	Hole note: 4X Ø12.954-13.716 (.510-.540 in)	hole edge + ribbon 'Home › Dimension > Diameter'; 4X and ±0.381 in the dimension’s properties	differs	diameter 13.335; FreeCAD shows Ø13.335 ±0.381 (NX can also show the limits 13.716/12.954)
H12	Datum Feature Symbol A on the back face (right edge of the edge view)	edge Edge2 + ribbon 'Home › Annotation > Datum Feature Symbol', 'A', MB2 = OK	differs	triangle 0.0 mm from the edge; editable letter ['A']; FreeCAD 1.1 has no datum feature symbol, NXStyle adds NX’s
H13	Datum Feature Symbol B on the bottom edge	edge Edge0 + ribbon 'Home › Annotation > Datum Feature Symbol', 'B', MB2 = OK	differs	triangle 0.0 mm from the edge; editable letter ['B']; FreeCAD 1.1 has no datum feature symbol, NXStyle adds NX’s
H14	Datum Feature Symbol C on the left edge	edge Edge3 + ribbon 'Home › Annotation > Datum Feature Symbol', 'C', MB2 = OK	differs	triangle 0.0 mm from the edge; editable letter ['C']; FreeCAD 1.1 has no datum feature symbol, NXStyle adds NX’s
H15	Flatness 0.051 on datum A (.002 in, Prob. 12-3)	selection + ribbon 'Home › Annotation > Feature Control Frame'; dialog filled; MB2 = OK	differs	frame 'flatness \| 0.051'; editable values ['0.051']; FreeCAD 1.1 has only fixed GD&T pictures, NXStyle adds NX’s Feature Control Frame dialog
H16	Perpendicularity 0.102 to A on datum B (.004 in)	selection + ribbon 'Home › Annotation > Feature Control Frame'; dialog filled; MB2 = OK	differs	frame 'perpendicularity \| 0.102 \| A'; editable values ['0.102', 'A']; FreeCAD 1.1 has only fixed GD&T pictures, NXStyle adds NX’s Feature Control Frame dialog
H17	Position Ø0.254 (M) to A, B, C under the hole note (.010 in at MMC)	selection + ribbon 'Home › Annotation > Feature Control Frame'; dialog filled; MB2 = OK	differs	frame 'position \| Ø0.254 (M) \| A \| B \| C'; editable values ['0.254', 'A', 'B', 'C']; FreeCAD 1.1 has only fixed GD&T pictures, NXStyle adds NX’s Feature Control Frame dialog

In the book (NX)

In FreeCAD NX-Style

Result

Notes

The plate: 101.6 x 101.6 x 12.7 mm, 4 holes on a 50.8 mm square

modelled by script (the exercise is the drawing)

same

volume 124001.7 mm^3; back face (z = 0) is datum A, bottom edge (y = 0) B, left edge (x = 0) C

File > Drafting, New Sheet

Ctrl+Shift+D + ribbon 'Home › Drawing > New Sheet'

same

Drafting Preferences: ASME standard

Preferences > TechDraw > Dimensions > Standard and Style = ASME Inlined

differs

was ISO Oriented; NX sets the drafting standard in Drafting Preferences

Base View: the plate’s face, scale 1:1

body selected + ribbon 'Home › View > Base View', MB2 on the sheet

same

direction set to look at the face (the book’s front view)

Projected view to the right: the plate’s edge, back face A

second Base View, MB2

differs

as in tutorial D, a second Base View stands in for a view projected off the base view

Arc centres for the dimensions

cosmetic vertex on each hole centre

differs

4 holes, 4 cosmetic vertices, found as ['Vertex6', 'Vertex9', 'Vertex12', 'Vertex15']; NX snaps dimensions to arc centres, TechDraw needs vertices there first

Basic dimension 25.4 (C to the hole)

two vertices + ribbon 'Home › Dimension > Horizontal', then basic

differs

measured 25.4; NX: Basic is a Tolerance type in the dimension dialog, TechDraw: the Theoretical Exact property draws the box

Basic dimension 50.8 (hole spacing)

two vertices + ribbon 'Home › Dimension > Horizontal', then basic

differs

measured 50.800000000000004; NX: Basic is a Tolerance type in the dimension dialog, TechDraw: the Theoretical Exact property draws the box

Basic dimension 25.4 (B to the hole)

two vertices + ribbon 'Home › Dimension > Vertical', then basic

differs

measured 25.4; NX: Basic is a Tolerance type in the dimension dialog, TechDraw: the Theoretical Exact property draws the box

H10

Basic dimension 50.8 (hole spacing)

two vertices + ribbon 'Home › Dimension > Vertical', then basic

differs

measured 50.800000000000004; NX: Basic is a Tolerance type in the dimension dialog, TechDraw: the Theoretical Exact property draws the box

H11

Hole note: 4X Ø12.954-13.716 (.510-.540 in)

hole edge + ribbon 'Home › Dimension > Diameter'; 4X and ±0.381 in the dimension’s properties

differs

diameter 13.335; FreeCAD shows Ø13.335 ±0.381 (NX can also show the limits 13.716/12.954)

H12

Datum Feature Symbol A on the back face (right edge of the edge view)

edge Edge2 + ribbon 'Home › Annotation > Datum Feature Symbol', 'A', MB2 = OK

differs

triangle 0.0 mm from the edge; editable letter ['A']; FreeCAD 1.1 has no datum feature symbol, NXStyle adds NX’s

H13

Datum Feature Symbol B on the bottom edge

edge Edge0 + ribbon 'Home › Annotation > Datum Feature Symbol', 'B', MB2 = OK

differs

triangle 0.0 mm from the edge; editable letter ['B']; FreeCAD 1.1 has no datum feature symbol, NXStyle adds NX’s

H14

Datum Feature Symbol C on the left edge

edge Edge3 + ribbon 'Home › Annotation > Datum Feature Symbol', 'C', MB2 = OK

differs

triangle 0.0 mm from the edge; editable letter ['C']; FreeCAD 1.1 has no datum feature symbol, NXStyle adds NX’s

H15

Flatness 0.051 on datum A (.002 in, Prob. 12-3)

selection + ribbon 'Home › Annotation > Feature Control Frame'; dialog filled; MB2 = OK

differs

frame 'flatness | 0.051'; editable values ['0.051']; FreeCAD 1.1 has only fixed GD&T pictures, NXStyle adds NX’s Feature Control Frame dialog

H16

Perpendicularity 0.102 to A on datum B (.004 in)

selection + ribbon 'Home › Annotation > Feature Control Frame'; dialog filled; MB2 = OK

differs

frame 'perpendicularity | 0.102 | A'; editable values ['0.102', 'A']; FreeCAD 1.1 has only fixed GD&T pictures, NXStyle adds NX’s Feature Control Frame dialog

H17

Position Ø0.254 (M) to A, B, C under the hole note (.010 in at MMC)

selection + ribbon 'Home › Annotation > Feature Control Frame'; dialog filled; MB2 = OK

differs

frame 'position | Ø0.254 (M) | A | B | C'; editable values ['0.254', 'A', 'B', 'C']; FreeCAD 1.1 has only fixed GD&T pictures, NXStyle adds NX’s Feature Control Frame dialog

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.

What differs from NX

FreeCAD 1.1 has only fixed GD&T pictures; NX-Style adds NX’s two dialogs, with values that stay editable.
TechDraw dimensions need vertices at hole centres; NX snaps to arc centres.
The hole limits show as Ø13.335 ±0.381; NX can also show them as limits.
TechDraw’s default standard (ISO Oriented) writes a hole note along its leader; ASME is a preference.