Most editing commands are available in the menu, but definitely key-bindings and Mouse actions are the most effective way to build and arrange schematics, so you should learn at least the most important ones.
The basic principle in XSCHEM is that first you select something in the circuit then you decide what to do with the selection. For example, if you need to change an object property you first select it (mouse click) and then you press the edit property ('q') key. It you need to move together multiple objects you select them (by area or using multiple mouse clicks with the Shift key), then you press the move ('m') key.
EDITOR COMMAND CHEATSHEET
This list is available in XSCHEM in the Help menu
XSCHEM MOUSE BINDINGS ---------------------------------------------------------------------- LeftButton Clear selection and select a graphic object (line, rectangle, symbol, wire) if clicking on blank area: clear selection shift + LeftButton Select without clearing previous selection ctrl + LeftButton if an 'url' or 'tclcommand' property is defined on selected instance open the url or execute the tclcommand LeftButton drag Select objects by area, clearing previous selection shift + LeftButton drag Select objects by area, without clearing previous selection Ctrl + LeftButton drag Select objects by area to perform a subsequent 'stretch' move operation Shift + Select objects by area without unselecting Ctrl + LeftButton drag to perform a subsequent 'stretch' move operation Mouse Wheel Zoom in / out MidButton drag Pan viewable area Alt + LeftButton Unselect selected object Alt + LeftButton drag Unselect objects by area RightButton Edit property of object under the mouse else edit global schematic / symbol property string Shift + RightButton Edit property of object under the mouse else edit global schematic / symbol property string using the specified (or default) text editor. LeftButton Double click Terminate Polygon placement XSCHEM KEY BINDINGS ---------------------------------------------------------------------- - BackSpace Back to parent schematic - Delete Delete selected objects - Insert Insert element from library - Down Move down ctrl Enter Confirm closing dialog boxes - Escape Abort, redraw, unselect - Left Move right - Right Move left - Up Move up - '!' Break selected wires at any wire or component pin connection - ' ' Pan schematic - ' ' When drawing lines or wires toggle between manhattan H-V, manhattan V-H or oblique path. - '#' Highlight components with duplicated name (refdes) ctrl '#' Rename components with duplicated name (refdes) - '5' View only probes - 'a' Make symbol from pin list of current schematic ctrl 'a' Select all shift 'A' Toggle show netlist - 'b' Merge file ctrl 'b' Toggle show text in symbol - 'c' Copy selected obj. ctrl 'c' Save to clipboard shift 'C' Start arc placement shift+ctrl 'C' Start circle placement alt 'C' Toggle dim/brite background with rest of layers ctrl 'e' Back to parent schematic - 'e' Descend to schematic alt 'e' Edit selected schematic in a new window shift+alt 'F' Toggle Full screen shift 'F' Flip alt 'f' Flip objects around their anchor points ctrl 'f' Find/select by substring or regexp - 'f' Full zoom shift 'G' Double snap factor - 'g' Half snap factor ctrl 'g' Set snap factor - 'h' Constrained horizontal move/copy of objects alt 'h' create symbol pins from schematic pins ctrl 'h' Follow http link or execute command (url, tclcommand properties) shift 'H' Attach net labels to selected instance - 'i' Descend to symbol alt 'i' Edit selected symbol in a new window shift 'J' Create symbol from pin list alt+shift 'J' Create labels with 'i' prefix from highlighted nets/pins alt 'j' Create labels without 'i' prefix from highlighted nets/pins ctrl 'j' Create ports from highlight nets alt+ctrl 'j' Print list of highlighted nets/pins with label expansion - 'j' Print list of highlighted nets/pins - 'k' Hilight selected nets ctrl+shift 'K' highlight net passing through elements with 'propagate_to' property set on pins shift 'K' Unhilight all nets ctrl 'k' Unhilight selected nets - 'l' Start line ctrl 'l' Make schematic view from selected symbol ctrl 'o' Load schematic - 'm' Move selected obj. shift 'N' Hierarchical netlist - 'n' Netlist Ctrl 'n' New schematic Ctrl+Shift 'N' New symbol shift 'O' Toggle Light / Dark colorscheme ctrl 'o' Load schematic - 'p' Pan shift 'P' Pan, other way to. alt 'q' Edit schematic file (dangerous!) - 'q' Edit prop shift 'Q' Edit prop with vim ctrl+shift 'Q' View prop ctrl 'q' Exit XSCHEM alt 'r' Rotate objects around their anchor points shift 'R' Rotate - 'r' Start rect shift 'S' Change element order ctrl+shift 'S' Save as schematic ctrl 's' Save schematic alt 's' Reload current schematic from disk ctrl+alt 's' Save-as symbol - 't' Place text alt 'u' Align to current grid selected objects shift 'U' Redo - 'u' Undo - 'v' Constrained vertical move/copy of objects ctrl 'v' Paste from clipboard shift 'V' Toggle spice/vhdl/verilog netlist - 'w' Place wire ctrl 'w' Place polygon. Operation ends by placing last point over first. shift 'W' Place wire, snapping to closest pin or net endpoint ctrl 'x' Cut into clipboard - 'x' New cad session shift 'X' Highlight discrepancies between object ports and attached nets - 'y' Toggle stretching wires - 'z' Zoom box shift 'Z' Zoom in ctrl 'z' Zoom out - '?' Help - '&' Join / break / collapse wires shift '*' Postscript/pdf print ctr+shift '*' Xpm/png print alt+shift '*' Svg print '-' dim colors ctrl '-' Test mode: change line width ctrl '+' Test mode: change line width '+' brite colors - '_' Toggle change line width - '%' Toggle draw grid - '=' Toggle fill rectangles - '$' Toggle pixmap saving ctrl '$' Toggle use XCopyArea vs drawing primitives for drawing the screen - ':' Toggle flat netlist
changes to default keybindings may be placed in the ~/.xschem file as in the following examples:
## replace Ctrl-d with Escape (so you won't kill the program :-)) set replace_key(Control-d) Escape ## swap w and W keybinds; Always specify Shift for capital letters set replace_key(Shift-W) w set replace_key(w) Shift-W
An important operation that deserves a special paragraph is the Stretch operation. There is frequently the need to move part of the circuit without breaking connections, for example to create more room for other circuitry or just to make it look better. The first thing to do is to drag a selection rectangle with the mouse holding down the Ctrl key, cutting wires we need to stretch:
After selection is done hit the move ('m') key. You will be able to move the selected part of the schematic keeping connected the wires crossing the selection rectangle:
In our example we needed to move up part of the circuit, the end result is shown in next picture. Multiple stretch rectangles can be set using the Shift key in addition to the Ctrl key after setting the first stretch area.
PLACE WIRES SNAPPING TO CLOSEST PIN OT NET ENDPOINT
The (uppercase) 'W' bindkey allows to place a wire putting start (and end point, later) to the closest pin or wire endpoint, this will make it easier to connect precisely without the need to zoom in all times.
while creating wires, lines, and moving, stretching, copying objects, pressing the 'h' or 'v' keys will constrain the movement to a horizontal or vertical direction, respectively.
Constrained horizontal move: regardless of the mouse pointer Y position movement occurs on the X direction only.
Unconstrained move: objects follow the mouse pointer in X and Y direction.