Selecting
NX treats selection as part of every command: what you may pick, from where, and why a pick was not taken. NX-Style adds the parts of that FreeCAD lacks, on top of FreeCAD’s own selection. The reference is NX 2212: its Type Filter, Selection Scope and QuickPick (rest the pointer until it shows three dots, then click). That gesture and the scope names are taken from NX user material and course notes, not checked in a running NX 2212.
Type Filter and Selection Scope
The Top Border Bar holds two filters and the Curve Rule.
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The Type Filter (No Selection Filter, Curve, Datums, Edge, Face, Feature, Point, Sketch, Solid Body) restricts what you can pick, in the graphics window and in the Part Navigator.
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The Curve Rule (Inferred Curves, Single Curve, Tangent Curves, Connected Curves) says what one picked sketch curve adds to the section of Extrude and Revolve (modeling.adoc#sections); it does not restrict what you can pick.
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The Selection Scope says where a pick may come from:
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Entire Assembly: anywhere (the default);
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Within Work Part and Components: the work part and the components inside it;
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Within Work Part Only: the work part’s own objects, not those of its components.
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The work part is FreeCAD’s active part. Double-click a part, or a component in an assembly, in the Part Navigator to make it the work part; the Part Navigator names it at the top. A component is one occurrence of a part: two links to the same part look alike in the graphics window, but only the one you made the work part counts as inside it. With no work part set, the whole document is the work part.
Why a pick is refused
When the filter, the scope or the running command refuses what is under the cursor, the cue line says so in red, for example:
The reason stays for a few seconds after the cursor moves on.
Select-through and QuickPick
Select-through. If the nearest thing under the cursor is refused and something allowed lies behind it, an MB1 click selects that one. The status bar names what was selected and why the nearer one was refused.
QuickPick. Rest the pointer over overlapping geometry for half a second: when two or more things there can be selected, the cursor shows three dots, and the next MB1 click opens the QuickPick list instead of selecting.
Holding MB1 still for the same time opens it too.
The list shows everything under the cursor, nearest first, each row with the element and the occurrence it belongs to (Face6 of Asm › UnitA › Box).
Rows the filter or the command refuses are greyed; hover one for the reason.
Hovering an allowed row highlights it in the graphics window; clicking it selects it.
Move the pointer away and the dots go, and a click selects as usual.
Select-through and QuickPick are off in a sketch, while FreeCAD edits an object in the view (a dragger), and with Ctrl or Shift held: MB1 then reaches FreeCAD at once.
"quickpick_hold_ms" in the settings sets the rest and the hold; raise it if slow clicks open QuickPick too often, 0 switches QuickPick and select-through off.
Commands that collect: Edge Blend
Home › Feature › Edge Blend collects the edges to round with a selection collector:
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✱ Select Edge (0)until it has enough, then✔ Select Edge (3): the count and whether it is enough; -
the curve rule: Single Curve, Tangent Curves (the default: one pick takes the whole smooth chain, such as the two lines and the arc of a rounded corner) or Connected Curves (follows a wire end to end; on a solid three edges meet at every corner, so it stops there);
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the collected edges, and the latest refused pick with its reason.
The collector takes only what Edge Blend can use: edges, of one body, picked in the part itself rather than through a component. OK hands the edges to FreeCAD’s Fillet, where you set the radius.
Both orders work:
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Select, then Edge Blend. If every selected item is a usable edge, FreeCAD’s Fillet opens at once with them, as before. If something unusable is among them (a face, an edge of another body), the collector opens with the usable edges, lists the rest as refused with the reason, and deselects them.
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Edge Blend, then select. The collector opens empty; pick the edges, then OK.
While the collector is open, its own rules are in force. Changing the Type Filter meanwhile does not override them; the new filter applies when the command ends. Cancel brings back the selection and the filter you had before.
FreeCAD’s own dialogs put up selection rules of their own while you pick references in them, and remove whatever rules are up when they close. NX-Style leaves a dialog’s rules alone: a Type Filter you choose while it is open takes effect when it closes, and the Type Filter and Selection Scope are put back in force after every dialog.
Part Navigator status
Above the tree the Part Navigator shows:
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Work part — the occurrence path of the work part;
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Active body — the body new features go into;
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Suppressed and Errors — how many features are suppressed or failed to update, and which; click the count to select them;
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Selected — the element and the occurrence the selection is on.
In the tree a suppressed feature is struck through and a failed one is red, with the error as its tooltip. FreeCAD 1.1.4 itself marks a failed feature only with a small overlay and a suppressed one not at all.