Symbol Workbench

Id: symbol · Tenth entry in the workbench dropdown

Symbol edits a part's schematic symbol, which is stored in the part document itself. BREP does not use a KiCad library directly; a component placed in a Diagram or PCB document takes a copy of its part's symbol. A pin IS one of the part's connection points, bound by name: drawing a pin here declares the point of that number, and the Inspector says which one (Editing a pin). It runs eCAD's symbol editor in place of the 3D view.

What it offers

Symbol creates no features. It adds:

• the symbol editor, drawn in place of the 3D view (The eCAD editor);
• the Inspector pane, for the symbol and its selected item, brought to the front when you enter the workbench unless you left another tab in front of it;
• the Qualify pane — like every workbench, while the part declares connection points — where picking a pin selects its point and the Pads button takes you to the pad;
• the editor's drawing tools in the workbench row (below).

Toolbar buttons

Six, eCAD's own tools; Select, Line, Rectangle and Circle look like the sketch tools that do the same thing:

Undo and Redo are the main toolbar's own, so the row carries neither. With the pointer over the editor, the mouse wheel zooms without fixed limits; the Zoom buttons have the same range. F fits it (the main toolbar's Zoom to fit does not). Keys reach the editor wherever the pointer is, unless a text field has the keyboard. Pressing Select or Escape puts any tool down.

Choosing this workbench while a sketch is being edited finishes the sketch, as its Finish button does, so the drawing is kept.

Editing a pin

A pin runs from its tip — the electrical end, where a wire meets it on a sheet — to its body end, the end that meets the symbol's outline. That line is the pin's direction and its length, and both are editable.

On the canvas. Click a pin to select it and it wears two handles: a disc on the tip and a square on the body end. Drag either one and the pin turns to follow the pointer and reaches as far as it is taken; the end you did not take hold of stays exactly where it was. Dragging the pin anywhere between them moves the whole pin, as it always has. Each drag is one press of Undo.

Every gesture — a drag, Orientation, Length, R, [ and ] — leaves a pin pointing one of four ways (left, right, up or down) with a length of whole grid steps (1.27 mm): a schematic pin is drawn on the axes everywhere, and a tip off the grid is a tip no wire on a sheet can be drawn to. Typing Tip or Body end sets any value; a pin left off the axes says On neither axis. Pick a direction to straighten it.

In the Inspector, with a pin selected:

From the keyboard, wherever the pointer is (but not while typing in a field): R turns the selected pin a quarter turn clockwise about its body end, ] lengthens it by one grid step (1.27 mm) and [ shortens it by one, never below one step, U selects the next pin that binds nothing, and Delete removes the selected item.

Placing pins. Drag with the Pin tool from where the tip goes toward the body, and the drag says both the direction and the length. Or just click: that places a pin of the length you last worked in, leaving the body to the left.

At the foot of the Inspector, Connection points says how many of the symbol's pins are bound, names anything that does not pair, and says when an edit could not be carried across to the points. A pin that binds nothing is drawn with an orange tip on the canvas and listed in orange under Items, so you can see which pins need attention without selecting each one. On a long symbol the list scrolls, so the pins that bind nothing are also named above it — for example 6 pins bind nothing: 9, 17, 23, 31, 36, 39 — and Next unbound pin selects each in turn and scrolls the list to its row. Selecting a pin on the canvas scrolls the list to its row too. In a tall window the list is taller. To see more rows or fewer, drag the grip under the list; double-click the grip to go back to the height the window gives it.

Import from KiCad

A part's symbol, pads and 3D model can come from KiCad together. Press the toolbar's Import button and pick a .kicad_sym symbol library. The import writes into the open part as one edit, so one Undo takes all of it away.

1. The symbol. A library holding several symbols lists them, with a search field. Choose one and press Next; a double click does the same.
2. The footprint. The symbol's Footprint property names one, such as Package_SO:SOIC-8_3.9x4.9mm_P1.27mm. The import reads it from Package_SO.pretty in your KiCad footprint folder. A generic symbol, such as Device:R, names none and offers filter patterns instead (R_*). The footprints they match are listed, as KiCad lists them, and you choose one or No footprint.
3. The 3D model. The footprint names a .wrl in KiCad's 3D library. BREP imports STEP, not VRML, so the import reads the .step of the same name beside it.
4. The review shows what will be written: the symbol, the pads with the file they came from, the model with its offset, rotation and scale, and the connection points. It also lists each link that could not be followed, naming the file it looked for. The model's STEP file is read while the review is open; Import is greyed until it has been read.

The part gets:

• the symbol, which this workbench then edits;
• the pads, which the Pads workbench edits;
• the model, as one Import 3D Model feature, placed on the pads exactly where KiCad places it;
• one connection point per pin, in one port group Pins (purpose pcb), named with the pin's label, on that pin's pad, pointing up out of the board. A pin on several pads gets its point on the first, and a pin on no pad gets its point at the part origin. Both are reported.

A link that cannot be followed does not stop the import. With no footprint, the part imports with its symbol only. With no model, or no .step beside the .wrl, it imports without a model. KiCad's own libraries name some models that were never made, such as the Molex Micro-Fit 43650-0215's. Either way, the review says so first.

A part that already has a symbol is not imported into: undo the earlier import first.

Your KiCad library. The dialog shows the two folders it reads, and where each came from:

• Footprints holds the *.pretty libraries;
• 3D models holds the *.3dshapes folders.

Each comes from KiCad's KICAD9_FOOTPRINT_DIR and KICAD9_3DMODEL_DIR when they are set, else from KiCad's install folder. Type another folder and press Use these folders to keep it for next time. A kept folder that has since gone falls back to KiCad's, and the dialog says so. KiCad's own library tables are not read, so a footprint library is found only if it sits in the footprint folder. The web version cannot read a KiCad library: it imports the file you upload, and nothing that file points to.

From an AI client (MCP). The same library is reached without the dialog by two commands. kicad_library_search finds symbols (and, with kind: footprint or for_symbol, footprints) by words in their Library:Name id, reading the folders above or the ones passed as symbols, footprints and models, and says which folders it read. kicad_part_add then makes the part the dialog would make, saves it in the models folder and adds it to the open assembly as a component, the way Add part to assembly does; a generic symbol is refused until a footprint is chosen (kicad_library_search with for_symbol lists the ones its filters offer) or no_footprint is given. Neither downloads anything: the library must already be on this machine.