Skip to content

Latest commit

 

History

History
1040 lines (939 loc) · 71.9 KB

editor-guide.md

File metadata and controls

1040 lines (939 loc) · 71.9 KB

Editor guide

For a first session, start with the quickstart. This guide covers the desktop and browser controls in more detail; the capability table records current limits.

Home and recent projects

The app starts on Home, with compact New Schematic, New PCB and Open Project cards. New PCB opens an empty Untitled project in PCB layout; New Schematic opens its schematic. Both use the usual unsaved-changes prompt before replacing an open project. On desktop, Recent projects lists the last 12 successfully opened or saved projects, newest first, as cards with a rendering of the saved schematic, its name and path. Click a card to reopen it; unsaved work gets the usual Save/Don’t Save/Cancel question. Remove a card with ×, or choose Clear recent projects, without deleting any files. History is kept between launches in application settings. A missing or unreadable project reports an error and stays in the list until removed. Empty and unavailable previews have placeholders; previews load in the background without opening or changing a project. Browser uploads have no reusable local path, so recent projects are desktop-only. Home does not automatically reopen a project.

Net labels and power symbols

Capture → Ground starts an ordinary GND symbol placement. P opens the Parts Catalog at the Power library, including GND, VCC, VCC (bar), +3V3 and +5V. The two VCC choices have different drawings and the same initial Value. Edit Value before placement to name the global rail. Power uses the same component properties, independent fields and G/M/R tools as other symbols; G keeps connections while M leaves existing wiring in place.

Capture → Net label or L opens a local label form; Ctrl+L opens a global label form. Set its net name, scope and rotation, then choose its anchor. R rotates a placement preview and Esc cancels it. Power instances use ordinary component fields and terminal identities throughout the editor.

Names are case-sensitive. Local labels join matching names on the same sheet; global labels and power/ground symbols join project-wide. A marker anchored exactly on a pin or wire contacts it. The Browser, Net Inspector and PCB pad annotations show the resolved name. Named nets explains scope, aliases, shared commands and limits.

Overlapping symbols

Overlapping symbol drawing bounds show a Symbol overlap notice during placement and a compact amber count badge on the canvas, with affected references on hover. Placement remains allowed. The check excludes separate pin leads and instance fields, so it provides a visual bounds warning rather than an electrical rule or exact stroke-intersection test. Finish any active placement with Esc, then right-click over stacked bodies and use Select symbol to choose a reference before dragging that part away. Warnings update after edits, undo and reopen without changing saved files or document history.

Preferences and grid

Wheel zoom moves through intermediate scales over a short transition in schematic, PCB and library editor canvases. Pinch gestures and panning remain direct. A middle-button drag pans by default; Navigation → Middle-button drag can make it zoom up and down about the press point instead, with the wheel still following its own setting. Right-button drag can pan instead of starting a selection box; right-click menus and tool cancellation are unchanged. The chosen pointer or center anchor stays fixed during the transition, while the snap spacing stays unchanged. Clicking, leaving the canvas, losing focus, or using Fit or an explicit view command stops pending wheel movement. Fine grid marks fade near density changes while the coarser marks remain visible.

The app bar shows the project name and an unsaved marker beside Undo, Redo, and Save (Download in the browser). The gear (or Ctrl+,) opens Preferences, with pages for Appearance (theme, interface scale, panel style, PCB grid, grid opacity, schematic grid outside paper, units), Navigation (whether the wheel zooms or pans, zoom direction, speed and anchor, and how middle- and right-button drag behave), Views (selection following), a list of Shortcuts and, on the desktop, the AI page for the Assistant. The schematic keyboard shortcuts page inventories the schematic bindings with their focus and selection conditions; the board keyboard shortcuts page does the same for the PCB editor, whose keys deliberately reuse several letters differently. The library editor keyboard shortcuts page covers the Symbol Editor, Footprint Editor and Parts Library workspaces, which dispatch their own small set of chords rather than the project-workspace bindings. Every workspace, including Home, the Parts Library and the symbol and footprint editors, ends the app bar with the same utilities in the same places: the version and Report a bug on wide windows, Help (except on the narrowest bars), Preferences and, on the desktop, the Assistant (Ctrl+Shift+A). The PCB canvas starts with its grid hidden; Appearance → PCB grid chooses Off, Dots or Lines for all PCB views and windows. This choice is remembered between sessions and leaves snapping unchanged. Grid opacity fades visible grids from 100% down to hidden at 0%, with Reset to go back; parts still snap to the same points. The opacity applies across views and windows and is kept with your preferences, not in the project. Schematic sheets sit on paper, and parts can still be placed on the canvas around it. Show grid outside paper (on by default) continues the schematic grid there; turn it off for a clean surround. A new schematic starts with its whole sheet fitted into the editor viewport.

Under Appearance → Schematic canvas, Paper background defaults to Uniform, with the same canvas colour on both sides of the page outline and no paper shadow. Shaded uses the theme's paper fill; Custom enables the Sheet color picker. Canvas color changes the schematic editing surface. Both colours follow the active theme until overridden, with separate light/dark choices. Use theme clears an override. These preferences do not change page geometry, snapping, project files or Undo.

In PCB layout, wheel and pinch zoom go up to 64× for close inspection of copper and clearances. Fit board returns to the whole board.

The right end of the bottom status bar shows the grid point under the pointer (X, Y, with Y increasing down), the Grid button and the display unit. Click the unit, or press Ctrl+U (⌘U on macOS), to switch between mil and mm; the Appearance page chooses it too. Switching only changes how lengths read: geometry, grid spacing and the project stay exactly as they were, with no undo step. 100 mil is exactly 2.54 mm. The Grid button sets the focused pane's snap spacing: 100, 50 (the schematic default, where symbol pins sit), 25, 10 (the PCB default) or 5 mil, or any other spacing typed with or without a unit (20, 20 mil, 0.5 mm, from 0.01 mm to 1000 mil). A bare number is read in the display unit, and a typed unit overrides it. N steps the focused pane finer and Shift+N coarser. A new spacing never moves or rescales anything already drawn, and pins stay reachable at any spacing because wires attach to them by clicking. When zooming out thins the dots, the button says how far apart the drawn dots are (for example Grid 10 mil · dots 50 mil). Each pane keeps its own spacing through focus changes, splitting and reopening files; the last one chosen is kept with your preferences, not in the project. Schematic and PCB panes remember their spacing separately, so changing the board grid does not replace the schematic's startup choice (and the reverse). Schematic panes start at 50 mil and PCB panes at 10 mil until changed; a saved choice, including an explicit 50 mil board grid, is kept. Search finds any setting; changes show at once, and Cancel puts them back. The house button beside the brand opens Home, with New Project, Open, Save, Preferences and About in its rail. Press Esc or choose Back to the project to return to the schematic, which stays open with its history while Home is shown. See VISION.md for the project's direction.

Tools and parts

The schematic ribbon has Capture, Sheets, Analyze, Libraries and View tabs. Capture groups placement, connections, clipboard, selection edits and PCB synchronization. Sheets keeps independent sheet creation, subsheet placement and hierarchical labels together. Analyze contains checks, annotation and reports; Libraries contains editors and source management; View contains panels, navigation and editor layout. Unavailable tools are disabled and appear in caption menus on compact windows. Fit and Net Inspector also have quick actions beside the tabs.

Choose Capture → Symbol or press A to open the Parts Catalog and focus search. The large form has library navigation, searchable results and a selected-part preview. Basic components contains the resistor, LED, capacitor, two-pin connector, four-pin header and NPN transistor from libraries/basic-components; registered sources appear as additional libraries. Power contains the built-in power and ground drawings. Manage libraries… opens the existing source manager. See the native source guide for loading a library and symbol library format for native definitions.

Click a result to inspect its drawing, value and source, then choose Place. Double-clicking a result or pressing Enter also starts placement. In the large form, the catalog closes and leaves a preview on the canvas; click to place it, R to rotate or Esc to cancel. A result can also be dragged directly onto the sheet, including Power entries with their chosen net name. Cancel, Esc or the header's × closes the large form without changing the project. On narrower hosts, a Library selector replaces its navigation pane; the smallest forms have Parts and Preview tabs.

Repeat placement, enabled by default for new settings, keeps the chosen part or power symbol active after each placement, preserving its rotation until Esc. With it off, one placement finishes the tool. Each instance has its own undo step, and the choice is retained when switching catalog presentations or restoring an arrangement. The active placement's right-click menu also offers Repeat placement, Rotate and Cancel. Placement commits on the primary press, so motion before releasing cannot turn a quick placement into a discarded drag.

Right-click empty canvas in the default pointer mode for Draw wires, Place symbol…, Place ground, Select all, Unselect all, Fit schematic and a Grid submenu with the same spacing presets as the status bar. Opening this menu preserves the current selection; symbol and wire hits retain their object menus.

Dock in the large form switches to a compact catalog, initially docked beneath Browser. Its header's Expand control returns to the large form. Both presentations keep the same library, query, selection, result density and custom power name, and reopening uses the last presentation. The compact catalog stays open after Place or a drag onto the sheet. A focuses its search; Esc releases search focus before another Escape cancels a canvas tool.

Drag the compact header to float the catalog or release it near an edge to dock. Its … menu also offers Float, Dock left and Dock right. The chevron collapses it to its header, and × closes it. Returning from the large form preserves the compact catalog's position. Docking overlays the canvas without resizing it; Fit keeps the drawing clear of the visible cards. Compact mode and its placement/visibility are retained in saved arrangements; an open large form and unfinished input gestures are not restored.

New resistors, capacitors, LEDs and two-pin connectors use shorter leads from revision 2 of the starter symbols; saved revision 1 parts retain their original geometry.

Copy and paste

The schematic canvas uses the system clipboard across split panes, detached windows, projects and running instances. Ctrl+C, Ctrl+X and Ctrl+V (⌘ on macOS) also appear in the canvas context menu and Capture → Modify. Paste previews at the pointer, R rotates the group, a click places it and Esc cancels. Ctrl+D duplicates without replacing the clipboard, while Ctrl+Shift+V opens reference, named-net and original-position options. The clipboard guide describes preserved definitions and wiring, cut behavior, browser gestures, shared commands and supported limits.

Moving symbols

Hover a symbol and press G, or choose Grab (keep connected) from its context menu, to move it without holding a mouse button. Attached wires follow the symbol; press R to rotate the preview and click to finish, or use Esc or right-click to cancel. Ordinary symbol dragging keeps the same connected movement and supports R.

Press M with a symbol selected, or hover a symbol with no selection, to pick it up while leaving its wiring in place. Click to place it elsewhere, or press Esc or right-click to cancel the preview. Disconnect and Move in the symbol's context menu performs the same action. R also rotates this preview; movement and rotation commit together as one undo step, while cancellation changes neither. The move and disconnection share one undo step; placing a replacement at the vacated pins connects it to the preserved wire ends.

With multiple items selected, M moves the selection while disconnecting contacts to unselected objects. Selected symbols, wire routes and named-net labels move together; connections within the selection remain intact, and no-connect markers follow their selected owners. Unselected wires stay in place. G grabs the group while keeping external wires connected, as ordinary group dragging does. Click to place, or press Esc or right-click to cancel; placement is one undo step.

Drawing and editing wires

Intentionally unused pins and wire ends

Hover a pin lead or open wire endpoint and press Q, or choose Capture → No connect and click the targets to mark. A larger X replaces the arrow, snapping its center to the attachment. The placed X follows the pin or wire end as it moves. Esc or right-click cancels the placement tool; empty-space and wire-interior clicks cannot create detached marks. Right-click a marked target and choose Delete, or click the X and press Delete or Backspace. Marker selection takes precedence over starting a wire, and its outline identifies the selected X. Shift/Ctrl, window/crossing selection and Select All include markers; the No connects selection filter controls them independently. Deleting selected marks clears only their intent, preserving the pin or wire. Drag a wire-end X to stretch its attached wire; the X stays selected and follows the same endpoint. Esc cancels that drag, and dropping onto a connection is refused while the mark remains. Q/Capture clears the previous selection and highlights. These edits support Undo/Redo and travel with copied parts and wires. Normal marks use dedicated blue theme ink; conflicts remain red.

Analyze → Electrical menu → No-connect check lists intentional no-connects, unmarked unconnected pins and open wire ends, plus connected, missing or type-changed marker targets. Use Show to navigate to a target. Error ink identifies conflicting intent. A marker suppresses only its own unconnected-pin or dangling-end warning; it never removes wires, changes the netlist or clears physical DRC violations. New wires and endpoint attachments at an X are blocked, including with W; remove the mark first. Hovering or quickly clicking near an X does not start a wire. Older saved conflicts remain visible in the check. This focused check does not implement the remaining type-conflict and power-driver ERC rules. See the identity and storage contract.

Wires

Click an unconnected symbol pin or free wire end to start directly. Press W to start immediately at the pointer, including on a connected pin, junction, wire segment or empty grid point. Capture → Wire instead waits for the first canvas click. The green crosshair marks the drawing point; a ring marks an existing connection target. Hold Ctrl to bypass the placement grid while drawing; releasing it restores snapping. Pins and wire connections still use their exact positions. Ordinary clicks on connected nodes retain selection behavior. Click to add corners, Space to flip the current elbow, and Backspace to remove the last corner. Click a destination pin or endpoint to finish, or press Enter or double-click to finish on empty space. Esc or right-click → Cancel discards the draft and exits drawing. Completing a wire clears its corners and keeps the tool ready for a new start; Esc returns to selection. Click a completed wire segment in selection mode to select it; only that segment turns blue, and Delete removes it. Drag a segment perpendicular to its direction to adjust alignment, or hover it and press G, then click to finish. Attached pins and junctions stay fixed while the adjoining legs adjust. Esc cancels the preview. Free endpoints, shared junctions and interior corners can be dragged without selecting the wire first. Hover a handle and press G, or right-click the wire and choose Grab, to pick it up without holding a button, then click to place it. Moving a shared junction adjusts all its attached routes; terminal pins stay on their symbols. Right-click → Select Wire selects the whole route for dragging or deletion; box and modifier selections continue to select whole wires. With one wire or segment selected, M picks up its whole route, including its bends and free-end no-connect markers; click to place, or press Esc or right-click to cancel. Pins outside the selection stay fixed and disconnect from the moved wire. Crossings stay disconnected. Select a wire segment, then use Capture → Modify for Slice, Heal or Delete in the group caption menu. Right-click a wire for these edits and whole-wire selection/deletion: Slice splits it at the grid point under the pointer and keeps it connected, so a new wire can start from the slice point. Break, available in this context menu, detaches the leg under the pointer from neighboring legs, pins and shared junctions at either end. It works with one or both ends attached; an already-free end stays free. The detached straight piece moves in both directions when dragged, carrying its ends with it. Its old contacts stay disconnected during departure. Once pulled clear, dropping it back onto those contacts reconnects them, including within the same drag. Ordinary drags of connected segments still anchor pins and shared junctions. Delete Segment removes just that leg, and Delete Wire the whole route. Hovering a row previews what it changes. An unconnected wire end shows a small square, a point where three or more wires meet shows a dot, and two wires meeting end to end read as one line. Agents use schematic.slice_wire, schematic.break_wire and schematic.delete_wire_segment with a point on the wire. schematic.move_wire_segment takes wire, at, to and expected_revision; to moves the point at at in both axes for a detached straight wire, or perpendicular to the segment when its ends are anchored. It uses the same geometry as the canvas preview and commits one undo step. Optional connect_ends names up to two of that wire’s degree-one junction IDs to join to exact stationary pin or wire contacts; ordinary geometry-only commands omit it. These commands are available in headless MCP and through the live desktop connection.

Selecting a segment also shows square handles on its wire’s corners and free ends. Drag a handle to reshape it in place: a straight segment slides across its direction, a corner drags the two legs that meet there, and a free end or junction drags the end leg of every wire attached to it. The wire's other ends stay put, gaining an orthogonal leg where needed; pins never leave their parts. Dropping a free end or junction on a highlighted pin, endpoint or wire segment connects every wire at that junction to the target, using its exact position even on a different grid. A segment target creates a branch automatically. Ambiguous contacts are refused. Moving or placing a part onto a wire connects its touching pins; placing a two-pin part across one straight run removes the span between its pins, inserting it without a short. Moving a whole wire onto a part also connects an exactly touching endpoint to its pin. Drags move by the grid's snapped travel, so an off-grid wire retains its offset until attached. Release to commit one undoable edit; Esc, releasing outside the sheet, or an edit made meanwhile cancels it. Multi-item selections and explicit Select Wire selections still move whole routes. Agents use schematic.move_wire_segment, schematic.move_wire_corner and schematic.move_junction. For an explicit connection, use schematic.attach_junction with junction, a pin/junction reference or {"wire":"wire-N","at":{"x_nm":0,"y_nm":0}} as to, and expected_revision. The same wire/point target works with schematic.draw_wire.

Completed draws and moves heal positive-length collinear overlaps, doubled-back legs, duplicate strokes and redundant straight-through junctions in the affected routes. When dragging folds a stepped route back over itself, obsolete split corners disappear instead of becoming dangling stubs; original free ends, pins and branches stay connected. When a route returns to an already connected straight wire through a U-shaped detour, healing slides the junction to the nearer intersection without passing another branch or moving a pin. Self-crossing returns also shorten. When a new route reconnects to its existing net, cleanup keeps the new drawing gesture and removes the older alternative only when it has no intermediate pin or branch. Manual cleanup and geometry-only moves retain the shorter-route policy. While drawing, retracing the draft shortens its preview immediately, including a reversal that runs past an earlier corner. Backspace restores the previous clicked corner, and finishing keeps the shortened route in one undo step. Preferences → Schematic → Auto-heal wires defaults on and is remembered as a user preference; the Modify menu offers the same toggle. Turn it off to keep detours and loops during editing, then use Heal on selected wires when you want cleanup. Commands that draw, place, move or attach support the optional auto_heal boolean with the same default; schematic.heal_wires always performs cleanup. Crossings and nearby geometry remain disconnected. Heal applies the same cleanup to selected wires and connects old endpoints that exactly touch a pin; agents use schematic.heal_wires with items and expected_revision. Healing is part of the initiating edit's undo step, and opening a file never performs cleanup. Ambiguous pin contacts, unsupported connections and overly complex edits are rejected as a whole. This local cleanup does not route around obstacles or resolve conflicting net names (named nets are separate work).

Symbol properties and selection

The Selection filters card sits below Properties in schematic and PCB views. Pins and Pads enable individual inspection selection and start off to preserve existing picking defaults. Its checkboxes also control symbols (including power/ground), wires, no-connect markers, local/global and hierarchical labels, and sheets in the schematic, and footprints and board graphics in PCB layout. All items toggles the supported categories together; Reset enables them all. Categories without individual selection support are disabled. Filtering does not hide geometry or change connectivity. Turning a category off clears its edit selection and cancels unfinished gestures; explicit placement and drawing tools remain available. Each view retains its filters through workspace changes, splitting and detach/dock, and saved arrangements keep them in local application settings. The card's chevron collapses it to its header; View → Selection filters hides or shows the card while retaining its settings.

Selection filters, Layers and Properties have draggable titles and a … position menu with Float, Dock left and Dock right. Drag a title away from its edge to float the card, or release near either edge to dock it; Esc restores the position from before the drag. Cards docked on the same edge stack beneath one another, with Browser above left-docked cards. Positions belong to the view, survive split and detached layouts, and are kept in local project arrangements. Preferences → Appearance → Panel style chooses whether the ribbon, Browser and docked cards float as separate rounded cards or join the window edge and each other; cards dragged over the canvas stay floating. The Symbol and Footprint editors use the same docking controls and panel style for Properties.

The schematic Properties card shows the focused selection's reference, value, orientation, X/Y position and footprint. Coordinates accept mm, mil or inch suffixes; bare numbers use the current display unit. Changing display units reformats valid drafts without applying or rounding away their stored coordinates. Apply changes commits all fields in one undo step. More properties, E over the body or away from text with one symbol selected, or a double-click on the body opens the expanded form. General combines reference, value, field visibility, datasheet, description, manufacturer, manufacturer part number and named custom fields; these belong to the selected component without changing its library definition. HTTP(S) values have an open-link control beside the input, including custom fields. Add link creates an additional named field for documentation, supplier pages or other web URLs. Each link opens independently, while D opens the saved datasheet for the hovered component (including its text), or the single selected component when the pointer is elsewhere. Opening a link changes neither the project nor undo history; text entry, dialogs and active tools retain their keyboard input. Local document paths remain plain field values.

Double-click visible reference, value or custom-field text, or hover it and press E, to edit it in place on the canvas. Enter applies the string as one undoable edit; Escape, an outside click, focus loss or a changed view/project cancels it. Invalid input stays in the text box for correction without changing the document. The editor stays in its originating split pane or native window and holds live mutation commands until accepted or cancelled.

The Text appearance disclosure selects a field and controls its name display, size, alignment, rotation and local offsets. Drag the reference, value or another visible field on the canvas to move only its text. Its outline appears on hover; the preview commits on release, while Escape, focus loss or release outside the canvas cancels. Moving the body carries its text, and rotating the body rotates manual offsets while retaining the chosen text orientation. Hover visible field text and press R to rotate that field about its anchor. R also rotates a field while dragging; release commits its position and angle together, and Escape discards both. Reset appearance restores automatic placement and default appearance for that field.

The attributes beside placement record population and output/simulation exclusions. Board exclusion prevents new placement. With reviewed board updates enabled, excluding an existing placement stages its removal for Apply; otherwise remove its footprint before excluding its component. BOM and simulation flags are retained intent for their future consumers. Exclude from pick-and-place files records omission from assembly position exports (reference, coordinates, orientation and board side); PCBcraft retains the flag, but does not yet generate those files.

Reset changes discards the compact draft, and Cancel discards the expanded draft. Attached wires follow coordinate changes through the same contact and healing rules as symbol movement. Invalid input or ambiguous contacts reject the entire draft. View → Properties shows or hides the inspector for that window. Footprint choice opens a responsive package browser focused on that component. From PCB layout, a searchable, scrolling component list lets you work through the project. The browser includes a library list, token-based name/package search, pin-count and mounting filters, and a larger physical 2D preview. Drag the preview to pan, use the wheel or +/− to zoom, and Fit to restore its framing. On narrow windows the library, results and preview stack in the scrolling body while Assign and Close remain visible. Browsing does not change the component; choose each terminal-to-pad connection or use Match numbers when their identifiers agree, then Assign. Source/license details remain available beneath the preview. The Library tab shows the pinned source/revision and opens Manage libraries or Edit symbol copy. Copy editing opens an independent definition document; it does not update the placed symbol. Updating a placed symbol from a library revision or replacing it with another symbol is not implemented. Apply or cancel pending field changes before using these actions.

Power symbols use these same properties and independent fields. Value supplies the global net name, while drawing and terminal behavior belong to the pinned definition. There is no separate power-marker form or glyph-style selector.

Press R over a symbol to rotate it, or select it first. Press X or Y to mirror the hovered or selected symbol about its center: X flips it left to right and Y flips it top to bottom. The same actions are in the symbol's right-click menu and in Capture → Mirror X/Mirror Y. Mirroring composes with the current rotation, rotating afterwards turns the mirrored drawing, and applying the same axis twice restores the original pose. Attached wires stay on their terminals, and reference/value text remains upright and editable. With a symbol selected, E opens its expanded properties and Delete removes it with its wires. Right-click a symbol for the same actions, and press Esc to clear the selection. New generic resistor and capacitor placements show neutral R and C values. Set their actual ratings in Properties; existing projects and pinned library revisions keep their original values.

Reference and value belong to the component; position, rotation and field appearance belong to its placed unit. Text sizes scale with the drawing when zooming. Native formats 2 and 3 record these separately, and opening a format 1 project migrates it on the next save. Authored wire routes use format 3. Footprints link to the component.

With no placement or wiring tool active, left-drag empty canvas or right-drag to select a group. Left-to-right draws a solid Window box and selects fully enclosed symbol bodies, wire paths and named-net anchors (including power and ground); right-to-left draws a dashed Crossing box and selects touched objects. The box shows the hit count. Shift adds to selection and Ctrl toggles items, with either boxes or individual clicks. Drag a selected member to move the group, or press Delete to remove it; each operation is one undo step. Connected pins on unselected components stay attached. Esc cancels a drag or clears selection, and a stationary right-click still opens the context menu. Selection alone does not modify the project.

Scroll to zoom or drag with the middle mouse button to pan. Use Fit to bring the circuit into view and Nets to open the Net Inspector.

Project Browser and sheets

The Browser floats over the left of the canvas and shows the project as Sheets → Main → Symbols / Nets and Boards → Board → Footprints under the project, using the same tree in schematic and PCB workspaces. Ordinary clicks never change workspaces: document rows navigate within the current workspace, or fold a branch belonging to the other workspace. Disclosure arrows only fold. Right-click a document for Open in Schematic or Open in PCB layout. Unfold Symbols, Nets or Footprints to inspect objects. An object click selects and centers within its workspace; Show in… in its context menu opens it explicitly in another workspace. A net row selects one of its wires. With one view open, the document path and count sit directly on the canvas beside the Browser, without a tab strip. Split views have one closable header above each canvas showing its document path, such as Power controller › Main. Click the Browser's title to fold it. Browsing never changes the project, and the canvas keeps its full size; Fit keeps the drawing clear of the Browser. The ribbon's View tab shows or hides the Browser and Net Inspector, opens the Parts Catalog, and fits the view. The Net Inspector uses the same collapsible card and tree rows as the Browser, with expandable named nets, their individual pins and a separate unconnected-pin section. Search filters nets or pins; inspecting them does not change the project. Each ribbon group's caption, such as Place ⌄, opens a menu of the same actions.

A project supports up to 64 sheets, either at the project root or nested under a parent. Right-click Sheets or a sheet row to create a sheet, or use Sheets → New sheet; a sheet row also offers Rename Sheet… and Delete Sheet…. Deleting a sheet removes its symbols, wires and associated board footprints in one undo step, and the project always retains at least one sheet. Each pane keeps its sheet target, camera and selection independently.

Use S or Sheets → Subsheet to place a hierarchical sheet symbol, then choose a new child or an existing unparented sheet. Double-click inside the symbol to enter its child; Alt+Backspace returns to the parent. The sheet name sits above the outline; drag either to move it, or select it and drag a corner handle to resize. Attached wires follow, and each gesture is one undo step. H or Sheets → Hierarchical label places a hierarchical label inside a child. Its matching pin appears on the parent symbol automatically, with the same name and direction; W connects wires to either end. The Browser nests child sheets beneath their parent. Each child has one parent, and repeated names on different sheets do not connect them. See hierarchical sheets for editing and deletion behavior.

Views and windows

View → Split opens another view of the current schematic in that window. Each pane keeps its camera, grid and edit selection while sharing the project's commands, undo history and saving. Click a pane or its header to activate it; the header underline marks that window's focused view. Browser and Net Inspector stay in place and target that view. The large Parts Catalog captures its opening view/revision; compact placement captures the current view when the gesture starts. A stale drag or modal choice cannot edit a different view or newer project state. Selecting a sheet in Browser or switching workspace changes that pane without adding document tabs.

On the desktop, View → New window opens another view without moving an existing one. Multiple native windows and splits can coexist, and each detached window can have its own split. Detach moves the active pane to a new window; when moving the only primary pane, another view remains at the same zoom and position. Dock in a detached window moves its focused pane beside the main window's focused pane, preserving the other panes and windows. Closing a native window while another remains dismisses only its views, without a save prompt or an implicit split elsewhere. Each window uses the same title-bar style and has its own panels. Every window's operating-system title, which the taskbar and window switcher show, names its focused document, such as Dual LED · transistor flasher › Main — PCBCraft; Home shows PCBCraft alone.

Right-click a pane's header for Split up or Split down to open another view above or below that pane. The same menu offers Open beside, Open in new window, Detach view, Dock in main window and Close view, as applicable. These actions target that pane, including its remembered document navigation. Dividers resize panes, with narrow areas stacking vertically.

On desktop, drag a pane header over a destination pane and choose Split up or Split down beneath that pane's header. Between different panes this moves the existing view and its cached documents, then collapses the old slot. Neighbouring panes expand into the vacated space; with only two panes, the resulting split can span the window. Its top, bottom, left and right edges offer the same placement. Dropping onto the source pane itself, or choosing Split up/down in its context menu, opens another view there.

The drag list also offers Split window up and Split window down. These move the existing pane above or below the window's entire remaining layout, closing its old slot. The preview is labelled Split window above/below and spans the window. Explicit pane and window splits keep their direction when resized or restored from a saved layout.

On desktop, dragging a header shades its source pane and displays window destinations. Drop over the centre of another pane in the same window to move into that slot; intervening panes shift, so a two-pane layout exchanges its positions. The full slot highlights Move pane here, retaining divider ratios and cached documents. Release outside the window or over Open in new window to detach, retaining its remembered documents and camera. Detached panes retain a draggable header with a leading Dock button that returns the pane to the main window in one click. Window destinations remain available beside the initial header press when the pointer leaves the source window. Drag onto Dock in main window or another window target; its row and destination split region highlight before release. Direct drops over exposed panes in another window are also available where the compositor exposes window positions. Moving outside the client highlights Open in new window; the new OS window is created on release. There is no window preview outside the client. Esc cancels. Every target belongs to the same running instance and project session. Live MCP can address the same destination with view.dock, passing the source view and destination beside view IDs from inspect_editor. An optional side of top, bottom, left or right selects an explicit split in the same window or another one. The window destination list also offers Above and Below, including on compositors that do not expose window positions. view.open_beside accepts side and an optional destination beside, opening a copy of source view inside that pane. view.dock adds scope: "window" with beside and side for a full-window move; its default scope retains ordinary docking. view.reorder takes source view and destination target IDs for in-window movement. Opening another view copies the source camera and grid without copying its edit selection. Turning Split off keeps the focused pane; turning it back on restores the window's remembered split arrangement, seeding restored cameras from the focused view. Layout and focus changes cancel unfinished gestures.

Selecting symbols or wires highlights their counterparts in every other visible view in amber; blue remains each view's own edit selection. Highlights follow the latest selection without taking focus. View → Settings → Follow selection offers highlight only (the default), all views, other views following primary, or primary following other views. Following reveals out-of-view items once while preserving zoom. When you select a PCB footprint, a following schematic pane can switch to the sheet containing its linked symbol. The pane does not take focus or select that symbol for editing. Primary is the original view even if detached, and its pane keeps the role whichever sheet it shows; closing it transfers that role to the main window's focused view. Delete acts only on the focused view's own selection, and clearing the source selection clears its highlights.

Closing any editor window leaves the others open. If the original window closes, a surviving window takes over project dialogs and the Assistant without moving its panes or resetting its camera. Closing the last editor window, or choosing File → Quit from any window, uses one Save / Don’t Save / Cancel decision for the project. Canceling or failing a save leaves the project open.

Saved arrangements of the project's panes and windows are available under File → Layouts. Use New arrangement to add one; each layout's submenu offers Activate, Rename…, Duplicate… and Delete…. Arrangements restore when a saved project is reopened on the same computer; they live in user-local app settings and do not change or travel with project files. Unsaved projects keep arrangements only for the session until their first successful save. See the arrangement persistence details.

PCB layout

The PCB ribbon separates Layout, Draw, Analyze, Manufacture, Libraries and View. Layout contains footprint placement, Route, clipboard, Modify and board setup/synchronization. Alignment and distribution are available in the Modify menu. Draw contains Line and Rectangle, which use the active layer. Analyze contains checks, measurement and cross-probing; Manufacture contains fabrication outputs; Libraries contains library editors and sources; View contains panels, navigation, Flip view and window layout.

Active layer, Track / line width and Via pad / drill stay visible as you switch PCB tabs. They sit at the right of a wide ribbon and wrap below the commands on narrow windows, while each tab's commands scroll independently. Choose a width or paired via size from its dropdown, or choose Custom… to enter a value in the display units (explicit units such as 20 mil also work). Save as preset remembers a custom choice in local application settings. These choices are separate from Board Setup profiles; shareable or project-pinned routing profiles are not implemented yet.

Left-drag empty canvas or right-drag to select footprints with the same Window/Crossing box used in the schematic. Only visible footprint geometry contributes to selection; Shift adds and Ctrl/Command toggles. Escape cancels the box, and Delete removes the selected footprints in one undo step. Footprint moves, rotation and flips operate on one placement at a time. With nothing selected, Properties summarizes the board: the Board Outline's overall Size in the display units (or No outline), copper layers, footprints, tracks, vias and, once connections are accepted, the number still Unrouted.

With two or more footprints selected, the Modify menu aligns them by their physical bounds (pads, courtyard and fabrication outlines, not silkscreen): Align to Left, Right, Top or Bottom, or Align to Vertical Center and Horizontal Center (the middle of the selection). With three or more, Distribute Horizontally or Vertically keeps the physical outermost parts fixed and makes the gaps between them equal to nanometer precision. Overlapping selections are refused if distribution would move an outermost part or change the selection's span. Each is one undo step. With one footprint selected, Properties edits its X, Y and Rotation exactly (in the display units and whole degrees) and switches its Side between Top and Bottom; each change is one undo step through the same transform command as M, R and F, keeping the other values. F (or Layout → Modify → Flip) moves the hovered or selected footprint to the other side of the board in one undo step, and F during an M move flips the part being moved. A bottom-side footprint is mirrored as seen from the top, its surface pads use the back copper, mask and paste, and its silkscreen, courtyard and fabrication graphics use the back technical layers; through-hole pads stay on every copper layer. Properties shows its Side, DRC compares courtyards only on the same side, and Outputs adds a bottom silkscreen file.

Browser builds support panes within one tab; native window actions are desktop only. The workspace tile can switch to PCB layout, open it beside the schematic or create a board window directly. Physical SMD placements render rounded rectangular copper pads, body outlines, courtyards and silkscreen, with component counterpart highlights, grouped Layers and Properties. Legacy placements retain pad-center markers. The editor supports up to 64 flat or hierarchical schematic sheets sharing one board. Existing footprints can be moved by left-dragging or by hovering/selecting one and pressing M, then clicking to place it. R rotates 90° counterclockwise and Shift+R clockwise, including during a move. Esc or a right-click cancels a move; releasing a drag over a panel also cancels it. The Layout ribbon offers Move and Rotate for a single selection, and Properties shows the saved position, rotation and side as editable fields. Moves snap the footprint origin to the view's grid, independently of grid visibility; each completed move and its preview rotations form one undo step. Routed tracks come along: each track end on one of the footprint's pads stays on that pad while the rest of the track stretches, in the preview and in the same undo step. A flip leaves an end behind when its SMD pad moves to the other side, and its airwire returns. A move, rotation, flip or alignment that would put a pad or a carried track onto another net's copper is refused, leaving the board unchanged. A conflicting edit, focus/workspace change or project reopen cancels the draft. The starter footprints include 0402/0603 resistors and capacitors, 0402 LEDs, SOT-23 and a two-pin plated header, pinned into projects with explicit terminal mappings. New views hide fabrication and courtyard graphics by default; Layers can show them. Board setup → Silkscreen stages physical text height, stroke width and pad clearance alongside the layer and stackup settings. Apply commits them in one undoable board change; Cancel discards the draft. Defaults are 1 mm, 0.15 mm and 0.25 mm respectively; lengths accept mil/mm input and save with the project. Assign Footprint… in a schematic symbol's context menu, or Layout → Place → Footprint in PCB layout, opens package selection and explicit terminal-to-pad mapping. Assigning pins the package without placing it. In PCB layout, Place on board places an assigned component at unit-aware X/Y coordinates, as a separate undo step; it then uses the ordinary M/R tools. Changing an already placed package awaits reviewed board updates. Native-folder registration, arcs and slots remain planned.

Drag a reference designator or hover over it and press M, then click to place it. The reference position is stored on that footprint and follows its rotation and side. The board view and silkscreen export use the moved position. Clicking the lettering selects the text, highlights its owning footprint and shows remaining airwires and text Properties. A dashed leader connects selected or moving lettering to its footprint even when the board is fully routed. Pad, silkscreen and reference highlights lighten their existing layer colors. R rotates the selected text; Delete hides it. Local printed words, font, paired height/stroke, rotation, alignment, visibility and offsets are undoable placement edits. Clear Use component reference to enter literal printed words; Rename… explicitly renames the shared component in the schematic and outputs. Reset silkscreen removes local appearance and position overrides. A footprint body's Edit silkscreen text button opens these controls even when its text is hidden. To author the default for future placements, edit the definition's reference offset in the Footprint Editor.

Layout → Board → Board setup and Layers → Board setup… share a revision-bound Craft settings form, including on a board with no saved stackup. The first opening shows a complete editable two-layer 1.6 mm FR-4/1 oz draft; nothing changes until Apply. Existing setups retain their own dimensions and materials. Board editor layers provides names and optional membership; Physical stackup provides every even copper count from 2 through 64, finished thicknesses/tolerances, a laminate total and cross-section, locked-gap fitting, and core/prepreg construction. Materials offers generic family presets and custom definitions, with sourced Tg/Dk/Df specifications and explicit pinned revisions behind technical details. The laminate preview uses copper and dielectric appearances independently of canvas layer colors. Profiles imports/exports a self-contained .pcsetup.json snapshot of stackup, materials and silkscreen; imported settings remain staged until Apply. Empty values stay unknown and typed units override the display unit. Apply is one undoable transaction; Cancel and invalid/stale drafts leave the board unchanged. Existing material pins cannot be rewritten; create a new revision and explicitly choose it in construction. Populated copper changes retain physical surface identities and resolve existing front/all-copper bindings; occupied drawings and authored stratum data are protected against removal.

Left-click footprints to select them, then press Delete to remove only their board placements. Layout → Modify menu → Delete provides the same action. Components, schematic wiring and physical package assignments are retained for re-placement, and undo restores the original placements. Active drawing tools and movement previews keep keyboard ownership.

Layers → Net names shows readable pad, via and track names when they fit the copper. Each view keeps its own overlay choice; document history is unchanged. Accepted PCB names wait for reviewed Update PCB when the schematic has changed.

The Layout ribbon's Active layer selector and status bar identify the drawing layer. Click a row in Layers to activate it, with an arrow and color swatch beside its name. The eye at the right toggles visibility independently: a pupil means visible, a slash means hidden, and its outline is always shown. Hidden active layers carry a (hidden) suffix. Show all and Isolate active change only visibility in the focused view, leaving saved board data and document undo unchanged. Click a layer color swatch to open the themed color form. Choose a color or enter #RRGGBB, then Apply color; Cancel discards the draft, and Reset to default removes that layer's override. Colors are local settings shared by every view of this board, including copper, Board Outline, silkscreen, mask and other technical layers. They survive renames without changing layer ownership or entering project files and undo. The ribbon's selected layer and every dropdown row include the same effective color patch. + and − cycle through the picker order, wrapping through technical and hidden layers without changing visibility. PgUp selects front copper and PgDn selects back copper when that side exists. Text fields, menus and dialogs keep their normal keys; switching layers cancels an unfinished Board Outline gesture or route, except that PgUp and PgDn during a route place a via and keep routing on that side. The keys are also listed in Keyboard Shortcuts.

Use Draw → Line or Rectangle on the active, visible layer. Line accepts successive vertices, closes when you click the first vertex, and finishes an open path with Enter. Rectangle uses two opposite corners. Both use the grid and nearby graphic vertices, with the current Track / line width as the physical stroke. Esc cancels unfinished geometry before exiting the tool.

On copper, these tools create conductive linework: a rectangle outline becomes four connected segments. It participates in connectivity, short checks, DRC and fabrication and uses the ordinary copper selection/editing tools. Filled copper zones use Layout → Route → Zone to draw editable zone outlines, with fill and refill remaining separate follow-ups. Non-copper shapes remain independent editable graphics: select a line, drag a vertex or segment, use M to move it, or Delete to remove it. Silkscreen, mask and paste artwork reaches its matching fabrication surface. Mechanical, fabrication, courtyard and user-layer graphics remain documentation in the native board.

Select Board Outline when drawing the physical boundary. Its centerline continues to define the board edge; a closed boundary is required for fabrication. Board Outline is also available without a copper setup. Fit and layer visibility include these graphics, while DRC reports a missing closed outline and copper outside it or too close to the edge.

To route copper, select a copper layer such as Top and press X or use Layout → Route → Track. Set Track / line width in the persistent controls in the display units (0.25 mm by default). The crosshair follows the pointer, while a dot marks where a click will land in free space or a ring marks a nearby copper connection. Free points snap when the grid point is close to the cursor. Hold Ctrl to bypass the grid while pads, track ends and vias still snap to their exact positions. Click to start a route or fix the current target. The preview uses clearance-aware 45° walkaround around fixed copper, with a wider release radius for magnetic contacts. Clicked targets wait for full-path validation; blocked or incomplete searches fix no new vertex. Use / to flip whether the diagonal comes first. Click a copper connection, double-click or press Enter to finish.

The route preview uses a lighter shade of each segment's copper layer color. A halo shows the default copper clearance (0.2 mm) around the draft tracks and vias. Press V while routing to drop a through via at the pointer and continue on the other side: front copper leads to back, any other layer to front, and the view's active layer follows once the proposed path and via validate. While routing, PgUp and PgDn switch to front or back copper, adding a via only when the layer changes. Hold Ctrl with either page key to place the via off-grid in free space. The Via pad / drill field beside the width field sets the pad diameter and drill (0.6 mm and 0.3 mm by default). Backspace removes the last via, returning to the previous layer, or else the last vertex. Right-click opens the route menu with Finish track, Remove last vertex, Place through via, Flip track posture, and Cancel. Esc or Cancel drops the unfinished route, and a second Esc exits the tool. The whole route is one Undo step. When copper joins two terminals of a net, their airwire disappears. A route that would connect pads on two different nets is refused with a message, leaving the board unchanged. Analyze → Checks → DRC starts a read-only snapshot check and opens a DRC card listing up to 1,000 findings. It reports a short when one copper island joins pads from different intended nets, copper of different nets closer than the clearance (0.2 mm), tracks narrower than 0.15 mm, via annular rings under 0.1 mm, each unrouted connection, a missing closed Board Outline, copper outside the outline or within 0.3 mm of its edge, and overlapping footprint courtyards. Courtyards on the same side are compared by their actual rectangle and closed-polyline shapes after rotation and flip, so empty space between separate courtyard elements or inside a concave outline is free. Courtyards that only touch at an edge or corner pass; overlap and containment are reported. Circles, arcs, open lines and self-intersecting outlines are still compared by their bounds, and those findings say they are conservative. Short checks include direct pad contact and via-mediated connections, even with a zero clearance rule. A board with reviewed connectivity uses its accepted terminal membership; pending schematic edits do not change that intent until accepted. Clearance remains a separate check, so direct pad contact can produce both a short and a clearance finding. Click a finding to center the view on its marker; the status bar shows the result, and an edit marks it out of date until Run again. The card shows stage progress and Cancel check while work is pending. Pan and zoom remain usable. Esc cancels unfinished work when the canvas owns keyboard input; closing the card or leaving its view also cancels it. Run again keeps only the latest queued request. An edit, rule change or project reopening discards obsolete completions, and stale findings stop drawing canvas markers. Desktop checks run on bounded workers; the browser advances the same engine checker in cooperative batches. Live MCP pcb.check_design waits for its report without blocking editor input, and fails if its source changes or its request expires. A headless command still returns its report directly. Both the card and headless report list at most 1,000 violations, while counts and total cover every finding. These rule values are fixed defaults until net classes and board rules arrive (#77); zones, hole spacing, silkscreen and solder mask are not checked, so a clean result is not a manufacturing sign-off.

Manufacture → Fabrication → Outputs generates a ZIP to save or download (suggested name <project>-fabrication.zip), with Gerber X2 files for each copper layer, the top and bottom solder mask, paste and silkscreen, and the Board Outline, plus an Excellon drill file for every plated hole (vias and through-hole pads). Coordinates are in millimeters with Y up, as seen from the top, measured from the board's placement origin: board zero unless an origin has been set with pcb.set_placement_origin (see MCP). Gerber coordinates are exact nanometres; Excellon coordinates are rounded to 0.001 mm with halves going up, so both shift exactly when the origin moves by a whole micrometre. Mask openings use pads on the corresponding outer copper layer; paste includes only surface-mount pads, not through-hole pads. Neither adds process expansion. Vias receive no automatic mask opening, but authored mask artwork can open them. The shape approximations below also apply to these openings. Generation needs a board setup, a closed Board Outline and a resolvable placement origin, and reports missing prerequisites. It does not edit the project. Repeated generation from the same captured inputs and exporter build produces the same archive; project names affect filenames and exporter versions appear in the Gerber header. Saving can be cancelled, busy or fail at the destination; generation alone is not a successful save. Run DRC first: outputs do not check the design.

Gerber X2 .AperFunction distinguishes copper-defined surface-mount pad flashes, through-hole pad flashes, via pads and tracks, even when their apertures have the same shape and size. Pad regions carry a descriptive aperture attribute but are not pad flashes. Copper obrounds emitted as strokes are not tagged as pads. Mask, paste and silkscreen artwork use Material. Closed Board Outline drawings are tagged Profile; open outline artwork is still plotted but untagged. Remove stray open artwork before sending the profile to fabrication. The aperture attributes do not change plotted geometry.

On copper, X2 .N identifies the intended net of pads, tracks and vias. Component pads carry .C (reference designator) and, on outer copper, .P (reference and physical pin number). A footprint land explicitly unmapped to a pin has an empty pin number. A short between intended nets or an unresolved via assignment leaves the affected tracks and vias without .N; individually assigned pads keep their intended net. Pads, tracks and vias use the same Gerber name for a given intended net. Distinct nets with the same display name get distinct Gerber names. Separate unwired terminals that each join several pads get distinct names even before the board has an accepted update baseline. Copper with no net has an empty .N. To avoid the reserved N/C marker, net names that equal N/C or begin with N/C: gain one N/C: prefix in Gerber only. These attributes change neither the plotted geometry nor the saved board. They describe intent, not verification of connectivity. Layer exports include the actual net and pin names; review what you are sharing before sending files to a fabricator.

For pads exported on a layer, round pads use standard circular (C) flashes. Rectangular (R) and obround (O) flashes require library-pad and placement rotations to each be multiples of 90° and the resolved corners to form a nondegenerate axis-aligned rectangle. Sizes follow the final X/Y axes, not either rotation in isolation. Rectangles also require their resolved midpoint to equal the integer pad center; odd-sized or otherwise uncentered rectangles retain their resolved polygon regions. Obrounds require width and height to have the same parity, so their capsule endpoints are integral and match the engine land contour. Mixed-parity or other rotated obrounds retain the existing approximate round-ended stroke (a C flash when both resolved sides are equal). Other rectangles remain regions, including net-cardinal poses reached through non-cardinal intermediate rotations. Very small collapsed rectangular pads can emit a retraced path with zero area. Rounded rectangles flash a Gerber aperture macro with circular corners when the inner shape is a convex quadrilateral, a line or a point and the emitted radius is within 1 nm of the authored radius. The diameter is rounded to the nearest nanometre after projection. The macro uses the placed pad's geometry, including rotation and side. Export stops without a file set if a convex macro core is not covered by its edge strips under Gerber coordinate and size tolerances and its outline could cross under coordinate perturbation. Rounded pads that do not qualify for the macro retain resolved polygon regions. This changes only generated pad artwork, not saved pad geometry, track or Board Outline output.

Copper filenames receive numeric suffixes when sanitized names collide with another output, including names that differ only in case. Fixed mask, paste, silkscreen and outline filenames retain their names. On Unix, replacement saves preserve the existing file's permission bits and new archives follow the process umask. The archive is flushed before replacement and its directory is flushed afterward on Unix. If that last flush fails, the error states that the complete archive was published but its directory sync failed.

The ZIP contains manifest.json alongside the Gerber and drill members. Its generator_version and ordered files list describe the same capture. Each record contains the member name, size_bytes and lowercase hexadecimal sha256 of its uncompressed UTF-8 bytes, including line endings. To check a member, compare its extracted byte length and SHA-256 with that record. The manifest lists neither itself nor the outer ZIP and does not depend on the save name. It checks file integrity, not source identity, configuration or DRC/ERC freshness, and cannot authorize a synchronized release.

Desktop re-export can replace the same ZIP without moving any old companion file. Cancelling the save dialog writes nothing. One editor limits its own active export requests, not other writers to the destination. The browser requests one ZIP download and cannot confirm completion or cancellation; check your browser for the saved ZIP.

Press Backtick over a visible pad, track or via to highlight its net. Visible pads, tracks and vias on that net brighten in their own colors while the rest of the board dims. The status bar names the net. Each copper island takes the net of its first netted pad, and each pad keeps its own net. Press Backtick over empty space to clear the highlight. Starting a route on existing copper temporarily emphasizes its net or, for an unassigned trace or via, the connected copper. The previous view returns when the draft ends.

Analyze → Measure (Ctrl+Shift+M) is a ruler that never edits the board. Click a start point, then an end point; both snap to a nearby pad center, track end or via, otherwise to the grid. The ruler shows the length and its horizontal and vertical parts (Y up) in the display units, follows the pointer until the second click, and a third click starts again. Esc clears the ruler, a second Esc or right-click leaves the tool. Measurements are not saved.

View → Navigate → Flip view shows the board from below in this view: model X runs right to left around the centered point, at the same zoom, and the status bar says Bottom view. Selection, routing and moves work as usual, mapped through the mirror; the board, its layers and its files are unchanged, and the button toggles back. Fit includes tracks and vias. Rotation follows the screen: R and the Rotate button turn counterclockwise, and Shift+R turns clockwise, whether the view is flipped or not. This also applies to move, footprint placement and PCB paste previews.

To stitch layers or start a route from a via, choose Layout → Place → Via or press Ctrl+Shift+X (macOS: Command+Shift+X). Each click places one through via with the current pad and drill, snapping to a nearby pad center or track end on any copper layer, otherwise to the grid; the tool stays armed until Esc or right-click, and each via is its own undo step. A via that would join pads on two different nets is refused, as is a second via on the same spot. The tool needs a board setup with at least two copper layers.

Without a tool, click a track or via to select it (Shift adds, Ctrl or ⌘ toggles) and press Delete to remove it; deleting a via keeps its tracks. Selected copper brightens in its layer color, like footprint pads, without adding an outline or changing its displayed width. A selection box also picks tracks and vias, with the same Window/Crossing rules as footprints. U selects every track and via joined by copper to the one under the pointer, or to the current copper selection. With copper selected and no footprint selected, M (or Layout → Modify → Move) moves the selection with the pointer until the next click, and dragging a track or via moves it directly; both snap to the grid, Esc or right-click cancels, and each completed move is one undo step. Properties shows the selected tracks and vias, with editable Width, Via pad and Via drill fields in the display units; a value applies to every selected item when you release a drag or press Enter. Copper Properties stays read-only while an accepted edit prepares, then becomes editable against its published values. A move or resize whose copper would reach another net's pad is refused, leaving the board unchanged. The Lock choice in copper Properties locks or unlocks the selected tracks and vias together; it shows Mixed when their states differ. Locked objects remain selectable, with size fields read-only. Moving, resizing, reshaping, segment-dragging or deleting protected copper is refused for the whole edit, including changes carried by a footprint move or alignment. Unlock it first. Copy/duplicate/paste retain locks on the new objects; Cut refuses protected objects. Undo/redo and native saves preserve lock state.

The Tracks and Vias selection filters turn picking of each off, by click, drag, U or box, and drop that kind from the current selection. Tracks stay on their layer, so a back-side track does not reach front-only SMD pads, while a via joins copper on every layer. With the pointer over a segment and no tool armed, D drags that segment with the pointer while segments touching it on the same layer stretch to stay attached. An end that meets the middle of another track holds there, so the segment pivots on that junction. A click commits them all as one undo step, and Esc or right-click cancels. Vias at its ends stay put. Blind or buried vias are not implemented yet. Routing does not check clearance; run Analyze → Checks → DRC for that. Live MCP reaches the transform command and these view, workspace and window controls too (see the MCP guide). See the board inspection walkthrough.

The same picker includes Symbol Editor and Footprint Editor as independent authoring workspaces with Draw, Library and View ribbons. Switching retains each definition's history, camera, selection and pending Properties fields, and returns to the last document of the selected kind. Their picker rows and View ribbons support the same split, detach/dock and native-window placements as project views. A definition can share a split with a schematic or PCB view; multiple views of one definition share its history while retaining independent navigation and selection. Closing a pane retains the definition and any unapplied fields. Definition placements currently last for the session, with the last saved project arrangement retained while definition panes are open.

Opening and saving projects

Open project.json, its project folder, or a .pc archive from File → Open…. On desktop, pcbcraft <path> opens one such target as the app starts, including through a symlink to a project folder or archive; a failed open reports in the status bar and leaves Home usable. pcbcraft takes no options and at most one path, and a usage error exits before the window opens. Quote paths containing spaces, for example pcbcraft "C:\boards\my board\project.json" on Windows. Startup errors also go to stderr when a handle is available. Windows release builds use the GUI subsystem and do not attach to the launching console; redirect stderr with 2>startup-error.txt to capture diagnostics. A failed open still appears in the status bar. Opening from PCB layout binds the incoming project's board before restoring its saved views, including split panes and detached windows. Desktop projects default to a folder containing separate project, schematic, board and saved symbol documents. Save keeps the opened form, and File → Save As… offers Project folder… and Packed project (.pc)…. Commit the folder to Git; use the archive to share the complete project. Ordinary hand-zipped project folders open too, including those without a manifest. The browser uploads and downloads current .pc archives. Version 0.1.0 breaks older project layouts; see the release notes. The native storage notes describe the formats, file safety and performance checks.

Bundled Power instances

New Power catalog and Ground ribbon placements use the same component fields, properties, inline text and G/M/R tools as Default or registered library symbols. Value names the global rail; the definition declares which terminal names it. The catalog's Value input is available for every symbol, in both presentations. The former power-marker annotation styles are unsupported; there is no automatic migration of those old records.

Board rules

Analyze → Rules edits the board's dimensional limits and preferred routing sizes through the same revision-checked command as MCP. Preferences must fit the hard bounds. Apply creates one undo step; Cancel leaves the board untouched, and Use built-in defaults removes the saved record. DRC reports the effective rules and any violations in existing copper. Rule edits make previous checks and route drafts out of date. See board-rules.md for units, local size choices, provenance and file compatibility.