Placement and Routing

Embedr takes a board from a generated layout to routed copper with the agent: you choose who will make the board, place or lock the parts that matter, and the agent routes the board automatically and fixes small manufacturing issues. Everything is written to the KiCad board in your project, where you can review it in the Board tab or in KiCad.

Before you start

Placement and routing need:

• a pcb/ workspace with a board .zen file that builds (see Schematics and PCB),
• a generated KiCad layout (ask "Generate the PCB layout"),
• a closed board outline on Edge.Cuts. Draw one with the Board outline tool, use Generate Outline, or ask the agent for exact dimensions,
• real footprints for every part, ideally from the component library.

Choose your board maker first

The board is designed and checked against one fabricator's limits from the start, so routing never produces copper the maker cannot build.

• In Plan Mode the agent asks who will fabricate the board and with which process. PCBWay's standard 2-layer and 4-layer processes are built in.
• On the first layout of a new board (no routed copper yet, no process recorded), Embedr records PCBWay's standard process for the board's layer count unless you said otherwise. The agent reports "Recorded the … manufacturing limits on this new board".
• Another fabricator: tell the agent, for example "We're making this at JLCPCB, 2 layers, standard process." It skips the PCBWay process and records the limits it researched for your maker instead.
• Change later: ask the agent to set the board's design rules to another process. The row reads PCB design rules. You can make limits stricter than the process, never looser.

PCBWay standard processes (1 oz copper):

Limit	2-layer and 4-layer
Minimum track width	0.127 mm
Minimum clearance	0.127 mm
Minimum via drill	0.3 mm
Minimum annular ring	0.15 mm
Hole to hole	0.5 mm
Minimum slot width	0.8 mm
Copper to board edge	0.3 mm

When a process is recorded, every net class on the board is raised to these minimums, and KiCad's design-rule check uses them, so a board that passes DRC should also pass the maker's manufacturing check. The process name appears in the Manufacturing tab heading ("Manufacturing checks · PCBWay").

If the board's layer count does not match the recorded process (for example a 4-layer board with a 2-layer process), the agent says the minimums were not checked and offers to record the matching process. For layer counts without a built-in process, it records researched limits or suggests a supported layer count.

The process is stored next to the board as <board>.embedr-rules.json.

Place the parts

Most boards need a person to decide where the mechanical and user-facing parts go. Do this before routing:

• By hand in the Board tab: drag parts in Select / move mode, rotate with R, or set exact X, Y, rotation and side in Properties.
• With the agent: "Put J1 on the left edge facing out, the two mounting holes 3 mm from the corners, and the LEDs along the top edge." The row reads Manual PCB placement.
• Lock what must not move: "Lock J1, H1 to H4 and the LEDs." Locked parts (also parts locked in KiCad) stay put during Auto Place.

Mounting holes and other non-plated holes are passed to Auto Place and Auto Layout as keepouts automatically; you do not need to draw keepouts for them.

Route automatically

Ask the agent to route ("Route the board"). Routing is one step: the row Route PCB with Freerouting runs in the cloud and, in the same call:

1. restores the board's design rules to the recorded process if they had dropped below it (for example after a layout sync),
2. routes every unrouted connection, keeping existing valid copper,
3. widens or resizes any vias and tracks below the process minimums,
4. runs KiCad's checks on the result and applies it only if it adds no new DRC errors.

You need to be signed in. A screenshot of the routed board is attached to the result.

What the result tells you

Row result	Meaning
PCB has no unrouted connections	Nothing to route; no run was used.
Freerouting candidate ready for review	Routing applied. Check the open-connection count in the details and in the Board tab footer (Unrouted).
Freerouting could not apply a route	The result added DRC errors or dangling copper. The original board is kept untouched.
Freerouting canceled	You stopped the agent run while routing.

When connections are still open, the agent explains why routing stopped:

• It stopped improving. Running it again on the same placement will not finish it. Move or rotate the parts around the open nets, then route again, or use Auto Layout.
• It reached its time limit. The best result so far was applied.

Routing does not tune differential pairs, impedance or trace lengths.

Small manufacturing issues fixed for you

After routing, vias and tracks below the process minimums are resized in place, or a via is moved a short distance with the tracks that meet it. Anything that cannot be fixed without rerouting is reported. The agent can run the same fix on its own with Repair manufacturing findings; it never adds or deletes copper, and a fix KiCad then rejects is undone.

Plans and limits

• Free accounts include two started routing runs. After that, the row shows "PCB automation is not included in your current plan." with View plans.
• When the routing queue is busy, runs wait in line. A run that never starts is not counted.
• If the board's rules are below the recorded process, routing is refused before it starts ("Net classes are below the … manufacturing minimums") and no run is used. The agent raises the rules and routes again.

Auto Place and Auto Layout

For boards automatic routing cannot finish, or when you want a first placement proposal, the agent can use Advanced PCB Automation:

Tool	What it does
Auto-place PCB	Proposes positions for unlocked parts. Locked parts are kept. Refused if the board already has tracks, vias or zones, because placement does not keep copper.
Auto-layout PCB	Routes copper with parts kept where they are. Existing copper is kept by default.

Both require a paid Embedr plan and available automation credit.

Approval

Each run asks you first. Before asking, the agent checks the board: a missing or open outline stops it ("Create the intended Edge.Cuts board outline before automation."), as do rules below the recorded process.

• Free plan: a card titled PCB Auto Place or PCB Auto Layout says "Automated component placement and board routing require an Embedr subscription." with View plans and Not now.
• Paid plan: a Permission required card names the action, says it "can modify the KiCad board file and may consume automation credits", and lists any constraints the agent set (locked parts, side preferences, copper policy). Choose Allow once or Decline, then Confirm. There is no "Always allow" for these runs, and the card waits until you answer.
• Out of credit: "PCB automation requires available bundled or prepaid credit." with Add overage credit.

If you decline, the agent stops and reports what is still unrouted; it does not start routing by hand.

Progress

While a run is active, the Board tab shows its progress at the bottom of the canvas, for example:

• "Route queued", "Place starting"
• "Route running • rev 3 • 41/52 routed • 11 open • 0.123 cr"
• "Route complete • 52/52 routed" or "Route partial • 3 open • 120 tracks"
• "Auto placement applied"

Board editing tools are disabled until the run ends. Decline the approval if you do not want a run to start; once it has started, the app has no control to stop it.

Result and recovery files

The result is written to the .kicad_pcb file, and the agent reviews a screenshot of it. Next to the board you will find:

• <board>.kicad_pcb.pre_pcb_auto_<placement|routing>_<time>.bak: the board before the run,
• <board>.kicad_pcb.post_pcb_auto_<placement|routing>_<id>.bak: the board as the run left it (also written after automatic routing).

To go back, ask the agent to restore one of them.

Routing by hand

The agent does not route a whole board by hand. When automatic routing leaves connections open, it moves parts, retries, or suggests Auto Layout. It hand-routes a few nets only when a requirement calls for it, such as an RF feed or a datasheet's layout guidance.

If you want manual routing, say so: "Route this board by hand, no autorouter." The agent will mention the trade-off once and then follow your choice. You can also draw tracks yourself with the Route tool in the Board tab.

A typical session

You:   Generate the PCB layout. We're using PCBWay, 2 layers.
Agent: Generated the layout and recorded pcbway-standard-2layer-1oz.
You:   Board is 50 x 30 mm. USB-C on the left edge, mounting holes in the
       corners 3 mm in, LEDs along the top. Lock those, then place the rest.
Agent: Placed and locked J1, H1–H4, D1–D3; placed the rest. Screenshot attached.
You:   Route it.
Agent: Routed 52/52 connections, resized 2 vias to 0.3 mm drill. DRC: 0 errors.

Review checklist

Before you treat a routed board as ready:

• Run DRC in the Board tab and resolve every error; read every warning.
• Check that Unrouted in the footer is 0.
• Connector positions, orientation and pin 1.
• Regulator layout and the power path; decoupling capacitors close to their pins.
• Track width on power and high-current nets.
• Clearance around mounting holes and the board edge.
• Antenna keepouts and RF feeds.
• Silkscreen readable and not on pads.
• Look at each copper layer on its own, and at the board in 3D.
• Run the manufacturing check in the Manufacturing tab. See Manufacturing and ordering.

You own the electrical sign-off.