Assemblies

The Assemblies application is FreeCAD 1.1’s Assembly workbench. It shows the Modeling ribbon with the Assemblies tab in front, so modelling commands stay at hand.

The Shaft Support assembly

A new assembly

  1. Application › Assemblies.

  2. Ctrl+N: in the Assemblies application, a new document starts with an empty Assembly, as NX’s Assembly template does.

  3. Save it (Ctrl+S) next to its parts; NX names the assembly in the New dialog, FreeCAD at the first save.

Adding components

Assembly › Add Component lists the open parts, and its dialog opens others from disk. Click one and press MB2.

  • The first component asks Ground Part?: the same as NX’s question about the Fixed constraint.

  • FreeCAD places a new component beside the last one; NX lets you drag it to a spot first.

  • Create New Component starts a new part inside the assembly.

Constraints

FreeCAD calls constraints joints. The Assembly Constraints group carries NX’s names:

NX constraint FreeCAD joint Use

Touch Align

Distance

Two faces against each other (offset 0), or at a distance.

Concentric

Revolute

A hole on a pin: on one axis, faces together, free to turn.

Align Axes

Cylindrical

Two cylinders or holes on one axis; free to slide and turn.

Align/Lock

Slider

On one axis, free to slide, not to turn.

Fix

Ground

Holds a component where it is.

Bond

Fixed

Two components move as one.

Parallel

Parallel

Two faces or edges parallel.

Perpendicular

Perpendicular

Two faces or edges at a right angle.

Angle

Angle

Two faces or edges at an angle.

Ball, Rack and Pinion, Screw and Gear are FreeCAD joints with no NX counterpart on that group.

Select the two faces or edges, click the constraint, and press MB2. One FreeCAD joint can do what two NX constraints do: a Revolute is NX’s Touch Align plus the axis.

Degrees of freedom

NX’s Show Degrees of Freedom has no FreeCAD equivalent. To see whether a part can still move, drag it with MB1 in the graphics window: a part with freedom left follows the drag the way its joints allow, a fully constrained one stays. Tutorial G checks the book’s degree-of-freedom results at each step this way.

FreeCAD 1.1.4 drops a Parallel joint whose faces start exactly perpendicular: the part does not turn although the solver reports success. Delete the joint, turn the part a little and apply Parallel again (Known issues).

Editing a part

Open the part, change it and save; the assembly follows when it recomputes. NX’s Open in Window is opening the part’s own document.

Exploded views and parts lists

  • Exploded Views › New Explosion moves parts by dragging a 3D handle; it has no distance field like NX’s.

  • Reports › Bill of Materials makes a spreadsheet with the parts and their quantities. NX puts the parts list on the drawing; a FreeCAD drawing can show the spreadsheet as a Tabular Note.

Clearance and space

Clearance Analysis and Simple Interference (NX’s Assembly Clearance) and Volume Claim and Check Volume Claims are on the Assemblies tab: see Assembly clearance and volume claims.

See also

  • Tutorial G — the Shaft Support, from Add Component to the parts list.

  • Tutorial U — volume claims and assembly clearance in a system layout.

  • Data management with Strata — Strata versions an assembly and its parts together.