Symbol editor · SoftForge Electronics Designer

.kicad_sym libraries open in the symbol editor (or use Edit symbol in the Libraries tab of a schematic, or Electronics Designer: New symbol…). It shares undo/redo, save, revert and hot exit with the other editors, and writes the library back with a minimal diff: symbols you do not touch stay byte-identical.

Library tab (left): the library’s symbols with a search box, the unit (A, B, …) and body style (normal / De Morgan) selectors, New and Export (save the symbol to another library; a derived symbol is flattened when its parent is not there).
Symbol tab (right): fields (Reference, Value, Footprint, Datasheet, Description, keywords, footprint filters and user fields), unit count and interchangeable units, De Morgan, power symbol, in BOM / on board / exclude from simulation, pin name offset and pin name / number visibility. With a pin selected it shows the pin (number, name, electrical type, graphic style, length, orientation, unit, body style, hidden, alternates); with a body graphic selected its stroke, fill and points; with a text its text size, bold, italic and justification.
Text boxes are fully editable: the Symbol tab edits the text (several lines), position and size, orientation, font size, bold, italic, horizontal and vertical justification, the border (on / off, line width and style), the fill and the four margins. A selected text box shows eight resize handles on the canvas: drag a corner or an edge to resize it on the grid (the opposite side stays), drag the box itself to move it, Esc puts the handles away. The schematic text box tool draws new text boxes on the symbol.
Pin table (Symbol tab): every pin of every unit in an editable grid; sort by any column, edit several rows at once, paste CSV / TSV rows (number,name,type,shape,x,y,orientation,length,unit, header optional).
Tools: Add Pin (each click places the next pin, numbers and names increment), rectangle, circle, arc, polyline, line, Bézier, text and text box; the grid defaults to KiCad’s 50 mil (1.27 mm). Move (M), rotate (R), mirror (X/Y), duplicate (Ctrl+D) and delete work on pins, graphics and fields. Derived symbols (extends) show the parent’s body and pins locked; only their fields are edited, as in KiCad.