+91 8866188126 [email protected]

PCB design guide

PCB design rules and DFM checklist

Design for manufacturing (DFM) means drawing your board so it can be made reliably, without guesswork. This guide covers the rules that matter most — tracks, holes, solder mask, silkscreen and the board outline — plus a checklist to run before you upload your Gerber.

Get an instant quote

Why design rules matter

Every order is checked by our engineers before production. A board that follows good design rules goes straight to the factory floor; one that does not may be held while we ask you a question.

What the engineering check looks for

That the Gerber matches the options you chose (layers, size, thickness), that tracks, gaps and holes can be produced, that the outline is complete, and that nothing on the files looks accidental — for example text on a pad or copper touching the board edge.

If something must change

We contact you before anything is made and explain what we found. Nothing in your design is changed without your agreement. If your design needs a different option, we tell you the new price.

If the price changes

You decide: accept the change and pay the difference, or cancel the order and get a refund. We never build a changed board without your agreement.

Design rules from your CAD tool are only half the story

Your CAD software checks the rules you entered into it. If those numbers are tighter than what the board can be made with, the DRC will still pass. Set your rules from the guidance below and from our PCB capabilities page before you start routing — not after.

Tracks and spacing

Thin tracks and narrow gaps are possible, but every step towards the limit makes etching harder and raises the chance of shorts or opens. Use generous values wherever the board has room.

RuleGeneral guidanceWhy
Track widthUse the widest track the layout allows. Many designers keep signal tracks at about 0.2 mm (8 mil) or wider when there is space, and go thinner only where a fine-pitch part forces it.Wider tracks etch more consistently and survive small defects.
Track-to-track gapA common rule of thumb is to keep the gap at least equal to the track width. Leave more space between high-voltage nets — follow the creepage and clearance rules of your product standard.Narrow gaps are the most common source of shorts.
Copper poursKeep a clear gap between a pour and nearby tracks and pads (often wider than your track gap), and remove small isolated copper islands.Islands can flake off; tight pour gaps cause shorts.
Thermal reliefsConnect pads to large pours with thermal spokes unless the pad needs maximum current or heat transfer.Solid connections make hand soldering and rework difficult.

Current and copper weight

1 oz (35 µm) copper is standard and suits most signal and low-power boards. For higher current, either widen the track or choose 2 oz or more copper in our calculator. Use an IPC-2152 based track-width calculator to size power tracks for your current and allowed temperature rise. Heavier copper also needs wider gaps, because thick copper is harder to etch finely.

Keep copper away from the edge

Routing and V-cut scoring cut through the board, so copper drawn right up to the outline can be exposed or damaged. As a common rule of thumb, keep tracks and pours a few tenths of a millimetre back from a routed edge, and further back along V-cut lines, where the scoring blade removes material on both sides. If you need copper on the edge on purpose, choose edge plating in the calculator instead.

Holes, vias and annular ring

The annular ring is the ring of copper left around a hole after drilling. If it is too small, a slightly off-centre drill can break out of the pad and cut the connection.

TermWhat it meansDesign tip
Drill sizeThe diameter of the drill bit that makes the hole.For plated holes, the drill is slightly larger than the finished hole because plating adds copper inside the barrel.
Finished hole sizeThe hole size after plating — the size that matters for component leads.For through-hole parts, a common rule is lead diameter plus about 0.2–0.3 mm. Check the datasheet’s recommended hole.
Annular ring(Pad diameter − hole diameter) ÷ 2.Keep a ring of roughly 0.15 mm or more on vias as general guidance, and more on component pads that will be soldered.
Via padThe copper pad around a via on each layer.Make it at least hole + 2 × annular ring. Larger pads are more forgiving.

The “Min via hole size” option in our calculator

On boards with 4 or more layers our online calculator offers a Min via hole size / diameter choice. The standard option is a 0.3 mm via hole with a 0.4 mm pad (4 layers) or 0.45 mm pad (6+ layers). Smaller vias — down to 0.1 mm — are available as options and may add to the price. Pick the option that matches the smallest via in your drill file; we read it from your Gerber when we can.

Small vias come with extra rules

Vias smaller than 0.3 mm add a 4-wire Kelvin resistance test, and on 4–6 layer boards the 0.25 mm and smaller classes also need TG155 material — the calculator adds these for you. 0.1 mm vias need a board 1.0 mm thick or less and an ENIG or OSP finish (not HASL). On 1–2 layer boards the standard via size applies, so keep your vias at 0.3 mm or larger.

Solder mask

Solder mask is the coloured coating over the copper. It is opened over pads so they can be soldered, and the thin strip of mask left between two pads is called a mask dam.

Opening expansion

Mask openings are usually drawn slightly larger than the pad (a small expansion on each side) so that a little misalignment never covers the pad. Most CAD tools set this globally — use their default unless you have a reason not to.

Mask dams on fine pitch

Between closely spaced pads (QFN, TSSOP, fine-pitch connectors), a dam of mask stops solder from flowing from one pad to the next. If the gap is too small for a dam to form reliably, the openings are usually merged into one shared window (a gang opening), which leaves the pads without a mask barrier between them.

Why thin dams cause bridges

A dam that is too narrow can break off or not form at all. Without it, molten solder can join two pads during reflow — a solder bridge. If you assemble fine-pitch parts, check that your pad gap leaves room for a real dam.
SituationGood practice
Vias near padsKeep vias tented (covered by mask — the standard option) so solder does not wick into them during assembly.
Via-in-pad under BGAChoose plugged or epoxy filled vias in the calculator. Boards with BGA parts are reviewed by our engineers before assembly pricing — see how PCB assembly works.
Mask colourGreen is the standard and fastest. Other colours work the same electrically; the colour only changes the look.

Silkscreen

The silkscreen (legend) is the printed text: designators, polarity marks, logos and labels. It helps assembly and repair, but it must never get in the way of soldering.

Text size

As general guidance, keep text at about 1 mm high or taller with a line width of roughly 0.15 mm or more. Smaller text may be printed blurred or with letters filled in.

Keep the legend off pads

Ink on a pad stops solder from wetting it. Check that no text, outline or logo overlaps a pad or a mask opening — many CAD tools can clip the silkscreen to the mask for you.

Legend colour

The legend colour follows the mask: white legend on every mask colour except white, and black legend on a white board.

Mark polarity and pin 1

Diode cathodes, electrolytic capacitor polarity and pin 1 of ICs and connectors should be marked clearly next to the part, not under it, so they stay visible after assembly.

Board outline and mechanical features

The outline tells the router where to cut. An incomplete or doubled outline is one of the most common reasons a board is held for review.

  1. 1

    Draw one closed outline

    The outline must be a single, continuous closed shape on its own layer (the board outline / edge-cuts / mechanical layer). Gaps, overlapping segments or two different outlines on different layers make the board shape uncertain.

    Tip: Zoom in on every corner and arc join — tiny gaps are easy to miss.

  2. 2

    Put slots and cut-outs on the outline layer

    Internal cut-outs and milled slots should be drawn as closed shapes on the same outline layer. Plated slots should also appear in the drill file. If a slot appears only on a copper or silkscreen layer, it may not be cut.
  3. 3

    Choose the outline tolerance you need

    Our calculator offers a board outline tolerance option. ±0.2 mm is standard; choose ±0.1 mm when the board must fit a tight enclosure or line up precisely with a connector.
  4. 4

    Allow for edge connectors and panels

    Gold fingers and castellated holes are options in the calculator. If you deliver your own panel, keep V-cut lines and break-away tabs clear of parts — see the panel guide.

Pre-upload DFM checklist

Run through this list before you upload. For how to export each file from your CAD tool, see Preparing your files.

CheckWhat to confirm
Layer count matchesThe number of copper layers in your Gerber is the same as the layers you choose in the calculator.
Outline is closedOne continuous board outline; cut-outs and slots on the same layer.
Drill file includedThe Excellon drill file (plated and non-plated holes) is in the zip, not just the copper layers.
Mask and silkscreen layers presentTop and bottom solder mask and legend layers are included for every side that has them.
Paste layer for assemblyIf we are assembling your boards, the top/bottom paste layers are included — the stencil is made from them.
DRC clean with realistic rulesYour CAD design-rule check passes with rules no tighter than the guidance above and our capabilities page.
Smallest via knownOn 4+ layer boards, you know the smallest via hole and have picked the matching “Min via hole size” option.
Units and scaleThe board size shown after upload matches your design (a wrong unit setting can make a board 25× too big or small).

Tip: view your Gerber before you upload

Open the exported files in a free Gerber viewer. If something looks wrong in the viewer, it will look wrong to the factory too. This one step catches most missing layers and outline problems.

Common reasons orders are held for review

Missing or open outline

The board shape cannot be read, or slots appear on the wrong layer.

Layer count mismatch

For example, a 4-layer Gerber ordered as a 2-layer board.

Holes smaller than ordered

The drill file contains vias smaller than the min via option you selected.

Spacing too tight

Tracks, gaps or rings below what can be produced. Compare against our PCB capabilities.

Silkscreen on pads

Legend ink overlapping solderable pads, which needs to be clipped back before production.

Unclear notes

Special requests that conflict with the chosen options. See the manufacturing FAQ for how we handle them.

Frequently asked questions

If our engineers find an issue such as legend text over a pad, we contact you and explain what needs to change. We never change your design without your agreement, so the safest route is to fix problems in your CAD files before you upload.

We contact you with the reason and the new price. You can accept the change and pay the difference, or cancel the order and receive a refund. Production only starts once you have agreed.

1 oz is standard and right for most designs. If your tracks carry high current and you cannot make them wider, choose 2 oz or more in the calculator. Remember that heavier copper also needs wider gaps between tracks.

In our online calculator the Min via hole size choice is offered for 4+ layer boards only. On 1–2 layer boards the standard via size applies, so design your vias at 0.3 mm or larger.

No. The paste layer is used to make the assembly stencil. Include it whenever you might order assembly, so the files are ready — see Preparing your files.

Yes. Every bare board gets a 100% flying-probe electrical test, free of charge. It catches opens and shorts in manufacturing, but it cannot catch a mistake in your design — that is what the checklist above is for.

Related guides

Still have a question?

Send us your files or call us — our engineers will help you choose the right options for your boards and assembly.

Streamline your innovation with seamless PCB ordering.

For More Details Contact Us