What differs from NX

Units are a preference, not a choice in the New dialog. NX-Style makes them metric (FreeCAD’s Standard schema: mm, kg) and switches an imperial schema back; "units": "freecad" leaves FreeCAD’s choice alone.

Typed values keep their precision (3.175 mm stays 3.175).

Files are .FCStd, not .prt. A new part is named at its first save.

FreeCAD asks for the sketch plane in the Dialog panel; clicking the plane in the graphics window also works.

No dynamic dimensions while you draw, and no "scale the whole sketch to the first dimension?" prompt.

Project Curve makes defining geometry; turn it into reference geometry before extruding a region across it.

A sketch fillet does not dimension its radius, and removes the constraints that held its corner.

Offset Curve takes side and distance from an MB1 click; type the exact distance afterwards.

FreeCAD names a dimension in its properties and takes a formula after =; NX numbers dimensions p0, p1 ….

Studio Spline Through Points is always cubic (NX takes a degree), and its points after the first are typed as length and angle from the point before, not as XC and YC. The first point takes X and Y, but Enter in either field places it. A typed point within FreeCAD’s pick radius of a curve (5 pixels at the current zoom) gets an automatic constraint to it, which moves the point.

Extrude and Revolve have command boxes with None, Unite and Subtract; Intersect is unavailable. Unite and Subtract target the sketch’s Body. NX’s full limit, draft and target-body options are not available.

Selected sections can use curves from one sketch; multiple sketches and solid edges are not supported.

Block, Cylinder, Cone and Sphere have NX-style dialogs and all four Booleans, including Intersect. Their supported creation methods and editing behavior are listed in the modeling guide.

Thread Detailed is a PartDesign Subtractive Helix of the basic thread profile, so it is real geometry and takes seconds to recompute. Symbolic is a feature that records the thread without NX’s dashed display. The thread starts at an end of the cylinder; the tables are ISO coarse and UNC only, single-start and straight.

Move Object offers Distance, Angle and Point to Point typed in its dialog; Dynamic is FreeCAD’s Transform dragger in its own dialog. Copies are not associative (NX’s default): a Body’s copy is a new Body on a static copy of the solid. There is no Associative option, no Move Object feature, and no vector from a picked face. A Body whose features refer to its origin (a Revolve about the Z axis) moves by its Placement, and FreeCAD 1.1’s Unite / Subtract into it then ignores the move; the dialog warns.

Hole drills at circle centres in a sketch; NX places hole points directly and adds their location dimensions.

At Angle datum planes turn about the face’s own axes; NX lets you pick the hinge axis.

Datum CSYS with nothing selected asks whether to continue; a Body already has its own origin.

Mirror Feature: select the feature first, then the command.

Patterns are separate buttons (Pattern Feature for linear, Circular Pattern, Multi-Transform); NX’s negative pitch is spacing with Reverse; Direction 2 is a tick box.

Design changes reopen the feature’s dialog (Edit Parameters) rather than editing a dimension shown on the model.

Parent/child links are properties (Attachment, Base Feature), not a Dependencies panel. Unsuppressing a child does not bring its parent back.

Expressions live in a spreadsheet (Ctrl+E); a dimension uses =Expressions.name. Names that are unit symbols (N, the newton) are refused.

Assign Material applies at once and closes with Close; FreeCAD 1.1 gives the body the material’s colour.

One FreeCAD joint can do the work of two NX constraints (Touch Align plus an axis).

No Show Degrees of Freedom; drag the part to see what moves.

New Explosion moves parts by dragging a 3D handle only.

The parts list is a spreadsheet (Bill of Materials), not a table on the drawing.

NX names a new assembly in the New dialog, FreeCAD at the first save.

Sheet size, projection and scale are the sheet’s template and properties, not a Sheet dialog. FreeCAD’s default sheet is A4.

Projected View is a projection group; a second Base View stands in for a view dragged off the base view.

A new section view lands on top of its base view and is moved afterwards.

Dimensions need vertices: add cosmetic vertices on hole centres first.

A basic dimension is the Theoretical Exact property; hole limits show as a value ± tolerance.

No Feature Parameters: reference dimensions measured from the view stand in.

View styles, smooth edges and arrowheads are view and dimension properties.

The sheet updates by itself; NX marks it out of date.

NX’s icons are Siemens' and are not copied; NX-Style uses FreeCAD’s icons and its own line icons.

Synchronous modelling goes no further than Delete Face (FreeCAD’s Defeaturing).

Feature dialogs are FreeCAD’s task panels, in the Dialog tab (or floating, with floating_task_panel).