Sheet Metal

Ctrl+Shift+M opens the Sheet Metal application, as in NX. Its features come from FreeCAD’s SheetMetal add-on (LGPL), which NX-Style bundles in vendor/FreeCAD_SheetMetal and the launcher loads. NX-Style gives it NX’s ribbon and names, and adds what NX keeps per part: the Sheet Metal Preferences and a Flat Pattern that uses them.

The Home tab

NX	Add-on command	Does
Tab	Make Base Wall	A plate of the material thickness from a closed sketch (or a bent profile from an open one).
Flange	Make Wall	A flange on selected edges: length, angle, bend radius, Length Spec (Leg, Outer Sharp, Inner Sharp, Tangential) and Bend Type (Material Inside or Outside, Thickness Outside, Offset).
Bend	Fold a Wall	Bends a flat sheet along a sketched line.
Hem Flange	Make Hem	A hem on an edge.
Extend Face, Extend by Sketch, Base Shape	Extend Face, Extend by Sketch, Add base shape	Lengthen a wall; a ready-made bracket or channel.
Convert to Sheet Metal	Convert to Sheet Metal	Turns a shelled solid into sheet metal.
Rip, Bend on Edge	Make Junction, Make Bend	Splits a corner; adds a bend between two walls of a converted solid.
Bend Relief, Corner Relief	Make Relief, Add Corner Relief	Reliefs at bends and corners.
Normal Cutout	Extruded Cutout	A cutout through the sheet.
Wrapped Cutout, Form Feature	Wrap Cutout, Make Forming in Wall	A sketch’s cutout wrapped onto bent sheet; a formed (stamped) feature.
Flat Pattern	Unfold (NX-Style’s)	The flat pattern, with the preferred neutral factor.
Sheet Metal Preferences	NX-Style’s	Thickness, bend radius, neutral factor.

Add-on command

Does

Tab

Make Base Wall

A plate of the material thickness from a closed sketch (or a bent profile from an open one).

Flange

Make Wall

A flange on selected edges: length, angle, bend radius, Length Spec (Leg, Outer Sharp, Inner Sharp, Tangential) and Bend Type (Material Inside or Outside, Thickness Outside, Offset).

Bend

Fold a Wall

Bends a flat sheet along a sketched line.

Hem Flange

Make Hem

A hem on an edge.

Extend Face, Extend by Sketch, Base Shape

Extend Face, Extend by Sketch, Add base shape

Lengthen a wall; a ready-made bracket or channel.

Convert to Sheet Metal

Convert to Sheet Metal

Turns a shelled solid into sheet metal.

Rip, Bend on Edge

Make Junction, Make Bend

Splits a corner; adds a bend between two walls of a converted solid.

Bend Relief, Corner Relief

Make Relief, Add Corner Relief

Reliefs at bends and corners.

Normal Cutout

Extruded Cutout

A cutout through the sheet.

Wrapped Cutout, Form Feature

Wrap Cutout, Make Forming in Wall

A sketch’s cutout wrapped onto bent sheet; a formed (stamped) feature.

Flat Pattern

Unfold (NX-Style’s)

The flat pattern, with the preferred neutral factor.

Sheet Metal Preferences

NX-Style’s

Thickness, bend radius, neutral factor.

The Analysis, PMI, View, Tools, PLM and Application tabs are those of Modeling.

Sheet Metal Preferences

Material Thickness, Bend Radius and Neutral Factor for new features. They are the add-on’s own defaults, so Tab and Flange start from them, and Flat Pattern unfolds with the neutral factor (the add-on’s own Unfold starts at a fixed 0.4).

The dialog shows what the values give for a 90° bend, and checks the neutral factor:

the neutral factor K places the neutral layer, the one that keeps its length, at K × T from the inside of the bend. Shih gives 0.25 to 0.5 as the practical range, and his exercise uses 0.41, which is also NX-Style’s starting value; values outside 0.25 to 0.5 are flagged, values outside 0 to 0.5 refused. DIN 6935 quotes k = 2K, so a DIN value typed here is refused rather than silently doubling the bend allowance;
a bend radius smaller than the thickness is noted: check the material’s minimum bend radius.

Bend allowance and flat length

For a bend through the angle A (90° for a right-angle flange), inside radius R, thickness T (Shih, Parametric Modeling with Siemens NX, ch. 13):

bend allowance     BA   = A (R + K T)            A in radians
outside setback    OSSB = tan(A/2) (R + T)
bend deduction     BD   = 2 OSSB − BA

dimensioned between bend tangent lines: flat length = the straight lengths + BA per bend;
dimensioned to the outside (outer sharp to outer sharp): flat length = the outside lengths − BD per bend.

nxstyle/sheetmetal.py has both; its unit tests reproduce Shih’s hand calculation of the actuator bracket. Tutorial W builds that bracket and compares the add-on’s flat pattern with the book: 67.0523 mm against 2 × 1.31992 in = 67.0519 mm (the book rounds to five places).

Switching it off

python launch_nx.py --no-sheetmetal, or "sheet_metal": "none" in nxstyle.json, starts without the add-on; Ctrl+Shift+M then explains how to get it. An add-on already installed in the NX profile’s Mod folder is used instead of the bundled one, never both.

What differs from NX

NX keeps the sheet metal preferences per part; the add-on keeps them per user.
NX’s Flat Pattern is a feature with its own drawing view type; here the flat pattern is a solid (with sketches of its outline and bend lines) that a drawing views from above.
NX’s Contour Flange, Lofted Flange, Jog and Gusset have no add-on equivalent; a Tab from an open, bent profile covers the contour flange.