Knowledge Hub
How printed circuit boards are made, and how each process works.
General industry knowledge. The Knowledge Hub explains how PCBs are made across the industry and what the standards say. It is not a list of what Wrekin Circuits builds, and figures here are typical values, not our limits. Only the notes marked "At Wrekin" describe our own process. For our capabilities and design rules, use the Engineers Hub.
Go deeper into each process
Technical guides to individual processes, materials and standards. Pick a subject to read the full guide.
Aspect ratio and small holes
Aspect ratio is the board thickness divided by the drilled hole diameter. It is the single number that best predicts whether a hole can be drilled accurately and plated reliably.
Why it matters
A plated hole is only as good as the copper in the middle of its barrel. Plating solution has to be pulled through the hole, and the deeper and narrower the hole, the harder it is to exchange fresh solution at the centre. Copper builds faster at the two ends than in the middle, so a high aspect ratio hole ends up with thin plating exactly where the barrel is under most stress in thermal cycling.
Drilling is affected too. A long, thin drill flexes. It wanders off position as it goes deeper, it breaks more easily, and it has to be withdrawn several times (pecking) to clear the chips, which slows the job down.
Drilled size and finished size
The size on your drawing is normally the finished hole size, after plating. The factory drills larger, commonly by 0.10 to 0.15 mm, to leave room for the copper and the surface finish. Aspect ratio is worked out on the drilled size, not the finished size, so a 0.20 mm finished via is usually a 0.30 mm drill.
Typical figures
| Hole type | Typical aspect ratio limit |
|---|---|
| Mechanically drilled through hole, standard production | About 6:1 to 8:1 |
| Mechanically drilled through hole, advanced production | 10:1 and above |
| Mechanically drilled blind via | About 1:1 |
| Laser drilled microvia | 0.75:1 to 1:1 |
These are industry ranges, not promises. Every factory publishes its own limit, set by its plating lines.
Design checklist
- Work out board thickness divided by your smallest drill before you start routing.
- Use the largest via that fits. A larger hole plates better, costs less and is more reliable.
- If a thick board needs small vias, consider blind vias for the fine pitch areas instead of forcing the ratio.
- Keep the number of different drill sizes down. Sizes that differ by less than 0.05 mm can usually be merged.
Barrel plating and IPC classes
The copper cylinder inside a plated hole is called the barrel. Its thickness and quality decide how many thermal cycles a board survives, which is why it is the most closely controlled feature in PCB manufacture.
How the barrel fails
Laminate expands much more through its thickness than copper does, particularly above its glass transition temperature. Every soldering operation and every hot and cold cycle in service stretches the barrel. Thin or brittle copper cracks, usually near the middle of the hole or at the knee where the barrel meets the surface pad. A cracked barrel can be an intermittent open circuit that only appears when the board is hot.
How it is built
After drilling and desmear, the hole wall is made conductive with a very thin electroless copper deposit. Electrolytic copper is then plated on top to build the working thickness. The plating must be continuous, free of voids and well bonded to the edge of every inner layer it meets.
What the classes ask for
IPC-6012 sets performance classes. Class 1 covers general electronics, Class 2 covers dedicated service electronics where long life is wanted, and Class 3 covers high reliability products where downtime is not acceptable. For ordinary plated through holes the copper requirement rises with class:
| Class | Average barrel copper | Thinnest point allowed |
|---|---|---|
| Class 2 | 20 µm | 18 µm |
| Class 3 | 25 µm | 20 µm |
Always check the current revision of IPC-6012 and your own drawing. Blind vias, buried vias and microvias have their own figures.
How it is checked
Plating cannot be seen from outside. A coupon from the panel is cut through the holes, mounted, polished and measured under a microscope (a microsection). The same section shows voids, cracks, resin smear and the quality of the bond to the inner layers.
Design checklist
- State the IPC class on the drawing. Do not ask for Class 3 unless the product needs it, because it also tightens annular ring and inspection rules.
- Keep the aspect ratio moderate so the middle of the barrel plates well.
- Avoid lots of isolated holes on one side of the board and dense holes on the other. Even hole distribution plates more evenly.
Via protection to IPC-4761
A via can be left open, covered, plugged or completely filled. IPC-4761 gives each option a type number so that designer and manufacturer mean the same thing.
The seven types
Five of the seven types come in two forms. The letter a means the protection is applied to one side of the board only, and b means it is applied to both sides. Types V and VII fill the whole hole, so they have one form.
| Type | What it is | Forms | Typical use |
|---|---|---|---|
| I. Tented | Dry film mask bridges over the via with nothing inside it | I-a, I-b | Simple cover |
| II. Tented and covered | Dry film tent with liquid solder resist over the top | II-a, II-b | Extra seal over a tent |
| III. Plugged | Resin or resist partly enters the hole | III-a, III-b | Stops solder and flux wicking through |
| IV. Plugged and covered | A plug with solder resist over it | IV-a, IV-b | Vias under BGAs away from the pads |
| V. Filled | The hole is completely filled with resin | V | Sealing vias fully, base for further layers |
| VI. Filled and covered | Completely filled, then covered with solder resist | VI-a, VI-b | Flat, sealed vias that are not soldered |
| VII. Filled and capped | Completely filled, then plated over with copper | VII | Via-in-pad, stacked vias |
Open vias
Leaving a via open, with the solder resist pulled back from the hole, is the simplest option and is perfectly sound for most boards. The surface finish protects the copper in the barrel.
Why the a forms are a risk
If a via is closed on one side only, as in the a forms, process chemistry and flux can be trapped inside it with no way to be washed out. Over time this can corrode the barrel. If vias are to be covered, cover both sides or fill them.
Via-in-pad
A via inside a solder pad must be Type VII. The resin fill stops solder draining into the hole and the copper cap gives a flat, solderable surface. It adds filling, curing, planarising and a second plating stage, so it costs more and adds time.
Design checklist
- State the IPC-4761 type and form on the drawing, for example Type IV-b, and whether it applies to all vias or only some.
- Put vias that need filling on their own drill file or tool number.
- Keep filled vias to one drill size where you can. A single size fills more consistently.
- Do not tent vias that are used as test points.
Blind, buried and microvias
A through via takes up space on every layer, even the layers it does not connect to. Blind and buried vias only occupy the layers they join, which frees routing space on the rest.
The three kinds
- Blind via: starts on an outer layer and stops on an inner layer.
- Buried via: joins inner layers only and cannot be seen from outside.
- Microvia: a very small blind via, normally laser drilled, that usually spans one layer pair.
Sequential lamination
Buried vias are made by building part of the board first. A core or a sub-assembly of layers is drilled and plated as if it were a finished board, then imaged and laminated into the full stack. Each extra sub-assembly is another complete cycle of pressing, drilling and plating, so cost and lead time rise with every stage.
Mechanically drilled blind vias can be made the same way, by drilling and plating a sub-assembly that includes the outer layer, or by drilling to a controlled depth after the final press. Depth drilling is limited to an aspect ratio of about 1:1 because plating solution cannot flow through a hole that is closed at the bottom.
Microvias
A laser removes the dielectric down to a copper target pad on the layer below. The hole is shallow and tapered, with an aspect ratio of 0.75:1 to 1:1, and is then plated. Microvias can be staggered from layer to layer, or stacked on top of each other if each one is copper filled. This is the basis of HDI (high density interconnect) boards.
Design checklist
- Talk to your manufacturer before fixing the via structure. The choice of which layers are joined decides the whole build sequence.
- Keep blind and buried spans to as few different layer pairs as possible. Every new span can mean another lamination.
- Give each via span its own drill file, named with its start and end layer.
- Keep the stack-up symmetrical so the sub-assemblies stay flat.
Stack-up design
The stack-up is the list of every copper layer and every piece of insulating material in the board, in order, with thicknesses. It sets the finished thickness, the impedance of the tracks and how flat the board stays.
The building blocks
- Core: fully cured laminate with copper on both sides. Its thickness is fixed and accurate.
- Prepreg: glass cloth with part cured resin. It bonds the cores and foils, and its finished thickness depends on how much resin flows into the copper pattern next to it.
- Copper foil: forms the outer layers in a foil build.
Prepreg is named after its glass style. The common styles, from thinnest to thickest, are 106, 1080, 2116 and 7628. Thin, resin rich styles fill around heavy copper well. Thick styles build thickness cheaply.
Rules that keep a board flat
- Make the stack-up symmetrical about its centre: the same materials, thicknesses and copper weights above and below.
- Use an even number of layers. An odd count is harder to balance and rarely cheaper.
- Balance the copper on each layer. A solid plane opposite a nearly empty signal layer pulls the board into a bow.
Rules that help signals
- Give every signal layer a solid reference plane next to it.
- Keep power and ground planes close together. A thin dielectric between them adds useful capacitance.
- Route high speed signals on layers between planes where you can, to contain their fields.
Finished thickness
The finished thickness is the sum of the cores, the pressed prepreg, all the copper, the plating and the solder resist. A tolerance of plus or minus 10% is the usual expectation. State whether your thickness is measured over the laminate, over the copper or over the solder resist.
Design checklist
- Ask for a stack-up from the manufacturer before routing controlled impedance tracks.
- Specify what matters (overall thickness, impedance, copper weights) and let the factory choose the exact prepregs where it does not.
- Put the stack-up on the fabrication drawing, including the layer order and which file belongs to each layer.
Controlled impedance
At high speeds a track behaves as a transmission line. If its impedance does not match the driver and the load, part of the signal reflects back and corrupts the data. Controlled impedance means building the track to a target value and proving it.
What sets the impedance
- Track width: wider tracks have lower impedance.
- Dielectric height: the distance to the reference plane. A thinner dielectric lowers impedance.
- Dielectric constant (Dk): a higher Dk lowers impedance.
- Copper thickness: thicker copper lowers impedance slightly.
- Spacing: for differential pairs, a smaller gap lowers the differential impedance.
Common structures
- Microstrip: a track on an outer layer over a plane. Solder resist over it lowers the impedance by a few ohms.
- Stripline: a track on an inner layer between two planes. Better shielded and more consistent.
- Coplanar: ground copper runs alongside the track on the same layer.
Typical targets
| Interface | Typical target |
|---|---|
| Single ended RF and general high speed | 50 Ω |
| USB differential pair | 90 Ω |
| Ethernet, LVDS, HDMI, PCIe differential pairs | 100 Ω |
A tolerance of plus or minus 10% is standard. Tighter tolerances are possible but need more process control and cost more.
How it is made and tested
The manufacturer models the structure with a field solver, using the real pressed thicknesses and the Dk of the chosen material, then adjusts the track width to hit the target. A test coupon with the same structures is built on the panel border and measured by time domain reflectometry (TDR). The coupon result is the evidence that the board meets its target.
Design checklist
- List each impedance on the drawing: value, tolerance, layer, track width and reference layers.
- Give impedance tracks a width that is used for nothing else on that layer, so CAM can find and adjust them.
- Allow the factory to adjust track widths slightly to meet the target.
- Do not route impedance tracks over a split in the reference plane.
Track width and current
A track carrying current heats up. The job of the designer is to make it wide enough that the temperature rise stays within what the board and the parts around it can stand.
What decides the temperature rise
- Cross section: width multiplied by copper thickness. Doubling either one roughly halves the resistance.
- Where the track is: an outer track loses heat to the air. An inner track is surrounded by laminate, although nearby copper planes spread heat very effectively.
- The board around it: thickness, material and the amount of copper nearby all change how well heat escapes.
The standards
The older method, from IPC-2221, uses charts and a formula based on tests from the 1950s. It is simple and conservative for inner layers. IPC-2152 replaced it with modern test data and takes account of board thickness, copper planes and material. If you use an online calculator, check which of the two it is based on.
Rules of thumb
- Decide the temperature rise you can accept first. 10°C is cautious, 20°C is common.
- 1 oz copper is about 35 µm thick. 2 oz copper carries the same current in about half the width.
- Voltage drop often matters before heat does on long, low voltage tracks. Check both.
- Remember the vias. Several vias in parallel are needed to carry the current of a wide track between layers.
What the factory does to your track
Etching makes a track slightly narrower at the top than at the bottom, and plating adds copper to outer layers. Finished copper thickness is specified by the standards as a minimum, not as the nominal weight. If a track is running at its limit, say so on the drawing so it is treated as a controlled feature.
Design checklist
- Size power tracks for the worst case current, not the typical one.
- Use planes or copper pours for high currents instead of very wide tracks.
- Keep narrow necks short. A neck heats up far more than the wide track on either side of it.
- Heavier copper needs wider gaps. Check the spacing rules before choosing it.
Heavy copper
Boards with 3 oz copper (about 105 µm) or more are usually called heavy copper. They carry high currents and spread heat well, but every stage of manufacture has to be adjusted for the extra metal.
Etching
Etchant attacks sideways as well as downwards. The thicker the copper, the longer it is in the etcher and the more the track is undercut, leaving a trapezoid shape instead of a rectangle. CAM compensates by drawing the tracks wider on the phototool, and that compensation needs room. This is why the minimum track and gap grow with copper weight.
Lamination
On inner layers, the spaces between thick tracks are deep. The prepreg has to supply enough resin to fill them completely, so heavy copper builds use more sheets of resin rich prepreg. Too little resin leaves voids, which show up later as delamination.
Solder resist
A tall track has a sharp shoulder that resist tends to thin on. Heavy copper boards often need more than one coat to cover the track edges properly.
Soldering
Thick copper pulls heat away from a joint. Pads connected straight into a heavy plane are hard to solder, so use thermal relief spokes on through hole pads and give the assembler notice that more preheat will be needed.
Design checklist
- Ask for the track and gap rules for your copper weight before you route.
- Keep copper evenly spread on each layer so plating and etching stay even.
- Avoid mixing fine pitch parts and very heavy copper on the same layer. The two need opposite things.
- Allow for the extra board thickness the copper adds.
- If only a few nets carry high current, consider a wider track in standard copper instead.
Surface finishes compared
The surface finish protects the exposed copper until the board is assembled and forms the surface the solder joint is made to. No finish is best at everything, so the choice depends on the parts, the assembly process and how long the boards will be stored.
| Finish | Strengths | Watch for |
|---|---|---|
| Lead-free HASL | Very solderable, robust, long shelf life, low cost | Not flat, so less suited to fine pitch and small BGAs. Extra thermal shock for the board |
| Tin-lead HASL | As above, with a lower process temperature | Not RoHS compliant. Only for exempt products |
| ENIG | Flat, long shelf life, good for fine pitch, BGAs and contact areas | Higher cost. Needs good process control to avoid nickel corrosion |
| ENEPIG | As ENIG, and suitable for gold and aluminium wire bonding | The most expensive common finish |
| Immersion silver | Flat, low loss at high frequency, good solderability | Tarnishes if handled or stored badly. Keep it sealed |
| Immersion tin | Flat, suits press-fit connectors | Shorter shelf life. Sensitive to handling |
| OSP | Flat, low cost, simple | Shortest shelf life. Limited number of heat cycles. Hard to inspect |
| Hard gold | Wear resistant, for edge connectors and keypads | Not for soldering. Plated only where needed |
How the main ones are applied
HASL: the board is fluxed, dipped in molten solder and drawn out between hot air knives that blow the excess off the surface and out of the holes.
ENIG: a chemical process with no current. Nickel deposits onto the copper, typically 3 to 6 µm, followed by a very thin layer of gold that protects the nickel. The solder joint forms to the nickel.
Immersion silver and tin: the metal replaces a little of the copper at the surface in a chemical exchange. The coating is very thin.
OSP: an organic compound bonds to the clean copper and is displaced by flux during soldering.
Choosing
- Fine pitch parts and BGAs want a flat finish.
- Through hole and larger surface mount boards do well with HASL.
- Boards that will be stored for a long time before assembly suit ENIG or HASL.
- Wire bonding needs ENEPIG or a soft gold made for bonding.
- Edge connectors that are plugged in repeatedly need hard gold on the fingers.
Whatever the finish, keep boards sealed in their packing until assembly and handle them by the edges.
Solder resist and legend
Solder resist keeps solder where it belongs and protects the copper for the life of the board. Legend tells people what goes where. Both are printed onto a surface that is not flat, which sets limits on how fine they can be.
Openings and expansion
The resist opening is made slightly larger than the pad so that normal misregistration does not leave resist on the pad. This expansion is typically 50 to 75 µm on each side. Many designers send the resist layer at pad size and let the manufacturer apply its own expansion.
Dams
The strip of resist left between two neighbouring pads is called a dam, and it stops solder bridging between them. A dam needs a minimum width to stay stuck to the board, typically around 100 µm for green resist. If the pads are too close for a dam after expansion, the pads are opened as one block (gang relief) and the bridging risk moves to the assembly process.
Solder mask defined pads
Normally the copper pad sets the solderable area and the resist stands clear of it. On some fine pitch BGAs the resist overlaps the pad edge instead and defines the area itself. Follow the part maker recommendation, and tell the manufacturer, because CAM would otherwise open the resist up.
Colour
Green is the standard: it images most accurately, holds the narrowest dams and is easiest to inspect. Other colours are widely available, but dark and heavily pigmented resists, especially black and white, block UV light and usually need wider dams.
Legend
- Text height of 1.0 mm or more with a line width of 0.15 mm or more stays readable.
- Legend is always clipped back from pads and holes. Ink on a pad stops it soldering.
- Inkjet printing straight from data gives finer text than screen printing and needs no screen.
- White is standard. Use black on white resist.
Design checklist
- Check that a dam survives between your finest pitch pads after expansion.
- Decide whether vias are open, tented or filled, and make the resist layer agree with it.
- Keep legend off pads and away from fiducials.
- Mark pin 1, polarity and the board revision.
Laminate materials
The laminate is the structure, the insulation and part of the electrical circuit all at once. A datasheet has a lot of numbers on it, but a handful of them decide whether a material suits a design.
The numbers that matter
| Property | What it means | Typical for FR4 |
|---|---|---|
| Tg, glass transition temperature | Above this the resin softens and expands much faster through its thickness | 130 to 140°C standard, 150°C mid, 170°C and above high Tg |
| Td, decomposition temperature | Where the resin starts to break down and lose weight | Above 300°C for lead-free capable grades |
| Dk, dielectric constant | Sets impedance and signal speed. Varies with frequency and resin content | About 4.2 to 4.6 |
| Df, loss tangent | How much signal energy the material absorbs | About 0.015 to 0.020 |
| CTE, z axis | Expansion through the thickness, which stresses the hole barrels | About 40 to 70 ppm/°C below Tg, several times higher above |
| CTI, comparative tracking index | Resistance to surface tracking at high voltage | 175 V and above. 600 V grades exist |
Material families
- Standard FR4: glass and epoxy. The right answer for most boards.
- High Tg FR4: for lead-free assembly of thick or high layer count boards, and for hot environments.
- Halogen free FR4: uses flame retardants without bromine.
- Low loss and very low loss: modified resin systems with Df from about 0.010 down to 0.002, for high speed digital and RF.
- PTFE and ceramic filled: the lowest loss and most stable Dk, for microwave work. Softer and harder to process.
- Polyimide: very high temperature resistance. Also the base film for flexible circuits.
- Metal backed (IMS): an aluminium or copper base for heat spreading.
Specifying a material
IPC-4101 groups laminates into numbered slash sheets by resin type and performance. Calling up a slash sheet, or giving minimum values for Tg, Td and CTE, lets the manufacturer use an equivalent grade that is in stock. Naming one brand and grade with no alternative can add weeks if that sheet is not on the shelf.
Design checklist
- Choose on the properties you need, and add "or equivalent" unless the exact grade matters.
- For impedance work, use the Dk of the actual construction at your frequency, not the headline figure.
- For lead-free assembly of thick boards, look at Td and z axis CTE as well as Tg.
- Mixed builds, with low loss material only on the layers that need it, can save cost. Ask before you design one.
Castellations and edge plating
Both features put plated copper on the edge of the board. Castellations are a row of half holes used to solder a module onto another board. Edge plating is a continuous band of copper round the edge, used for shielding and grounding.
How castellations are made
The holes are drilled on the board outline and plated with every other hole. Once the board is finished, the router cuts along the outline through the centre of each hole. The risk is at that cut: the router bit can drag a burr of copper across the opening or lift the plating from the wall. Factories manage it with cutter direction, extra drilling or routing passes and a deburr step, which is why castellations are a chargeable extra.
Designing castellations
- Use a generous hole. Around 0.5 to 0.6 mm is a common minimum, and larger is more robust.
- Give each hole a pad on the top and bottom layer, and on inner layers too where possible, to anchor the barrel.
- Place the hole centres on the board outline, or slightly inside it so more than half the barrel remains.
- Keep an even pitch and leave enough laminate between holes for strength.
- A flat finish such as ENIG suits modules that will be reflowed onto a host board.
How edge plating is made
The edges to be plated are routed as slots before the panel goes through metallisation, so the edge is plated at the same time as the holes. The board has to stay attached to the panel, so the plating is interrupted wherever a holding tab is left.
Designing edge plating
- Show clearly on a mechanical layer which edges are plated and where tabs may go.
- Run copper on the outer layers right up to the plated edge and overlap it, so the edge plating has something to join to.
- Pull back from the edge any inner layer copper that must not connect, such as power planes.
- V-scoring cannot be used on a plated edge.
Panels and arrays
Small boards are usually assembled several at a time in an array, sometimes called a delivery panel. A well designed array runs cleanly through the pick and place line and breaks apart without damaging the boards.
Two ways to hold boards in an array
| V-scoring | Tab routing | |
|---|---|---|
| How | A V groove is cut into both faces, leaving a thin web | Boards are routed round, held by small tabs with breakaway holes |
| Shape | Straight lines right across the panel. Rectangular boards | Any outline |
| Space between boards | None needed | The width of the router bit, commonly 2.0 to 2.4 mm |
| Edge after breaking | Slightly rough along the whole edge | Smooth, with small nibs at the tabs |
| Watch for | Copper and parts need clearance from the score line. Thin boards can sag | Place tabs away from sensitive parts and connectors that overhang |
Rails, fiducials and tooling
- Rails: waste strips on two or four sides give the conveyor something to grip. They are needed when parts sit close to the board edge.
- Fiducials: small bare copper dots, typically 1 mm across with a clear area round them, that the placement machine uses to find the panel. Three on the rails, plus local ones for fine pitch parts.
- Tooling holes: non-plated holes in the rails for fixtures.
Breaking out
Separating boards puts stress into them. Ceramic capacitors close to a score line or a tab can crack. Keep them a few millimetres away, and turn them so their long side runs parallel to the break.
Design checklist
- Ask your assembler for their preferred panel size, rail width and fiducial pattern before fixing the array.
- Keep copper back from scored edges on every layer, inner layers included.
- Do not put tabs where a connector overhangs the edge.
- If you have no preference, let the manufacturer propose the array. They will fit it to their production panel for the best yield.
Flex and flex-rigid
A flexible circuit replaces cables and connectors with a thin circuit that bends. A flex-rigid board goes further and builds the flexible layers into rigid sections, so the whole assembly is one part.
Materials
- Base film: polyimide, commonly 25 or 50 µm thick, with copper bonded to one or both sides.
- Copper: rolled annealed copper has a grain that survives repeated bending better than standard electrodeposited foil.
- Coverlay: a polyimide film with adhesive that is pressed over the tracks instead of solder resist. Its openings are drilled, routed or laser cut before bonding, so they are less fine than resist openings.
- Stiffeners: pieces of FR4, polyimide or metal bonded on to support connectors and components.
How flex-rigid is built
The flexible layers are imaged, etched and covered first. Rigid material is then laminated to them using no flow prepreg, which has been cut back so that resin does not creep onto the area that must bend. The assembly is drilled, plated and finished like a rigid multilayer. The rigid material over the bend area is removed at the end.
Bending
The tighter the bend and the thicker the flex, the more the copper is strained. As a starting point, allow a bend radius of around 10 times the flex thickness for a one or two layer flex that is bent once on installation, about 20 times for multilayer flex, and 100 times or more for a flex that moves in service. IPC-2223 gives the full method.
Design checklist
- Run tracks straight across the bend, at right angles to it. No vias, pads or corners in the bend area.
- Use curved tracks and teardrops on pads. Sharp corners start cracks.
- Stagger tracks on opposite sides of the flex so they do not sit directly over each other.
- Use hatched copper instead of solid planes where the flex has to bend.
- Keep plated holes back from the join between rigid and flex.
- Flex materials absorb moisture. Expect to bake them before assembly.
IMS and thermal boards
An insulated metal substrate (IMS) is a circuit on a metal plate. A thin dielectric bonds the copper to the metal and carries heat away from the parts far better than FR4 can. It is the standard solution for power LEDs and compact power electronics.
The three layers
- Circuit copper: usually one layer, from 1 oz upwards.
- Dielectric: a thin, ceramic filled layer, typically 75 to 150 µm. It has to insulate electrically and conduct heat, and these two pull in opposite directions.
- Metal base: usually aluminium around 1.0 to 1.6 mm thick. Copper bases conduct better but cost and weigh more.
Thermal conductivity
Standard FR4 conducts about 0.3 W/mK. IMS dielectrics commonly range from 1 to 3 W/mK, with premium grades higher. What matters to the part is thermal resistance, which depends on thickness as well: a thinner dielectric of the same grade moves more heat but withstands less voltage.
How manufacture differs
Most IMS boards are single sided with non-plated holes. The circuit is imaged and etched in the normal way with the metal base protected. Drilling, routing and scoring cut through metal, so tooling and feeds are different. Plated holes through the metal base are possible but need the base to be drilled oversize and filled with insulating resin first.
Other ways to move heat
- Thermal vias: an array of plated vias under a part carries heat through an FR4 board to copper on the other side.
- Heavy copper and planes: spread heat sideways.
- Bonded heatsinks: a metal plate bonded to a finished multilayer.
Design checklist
- Start from the heat you have to remove and the isolation voltage you need, then choose the dielectric.
- Keep copper back from the board edge and from mounting holes to preserve isolation to the base.
- Use large copper areas round hot parts to spread heat before it crosses the dielectric.
- White solder resist is common for LED boards because it reflects light.
Standards and testing
Standards give designer, manufacturer and customer a shared definition of a good board. Most of the industry works to the IPC family, and a short list of documents covers nearly every bare board.
The documents you will meet
| Standard | Covers |
|---|---|
| IPC-2221 and IPC-2222 | Design rules for printed boards in general and rigid boards in particular |
| IPC-2152 | Current carrying capacity of tracks |
| IPC-4101 | Laminate and prepreg materials |
| IPC-4761 | Via protection types |
| IPC-6012 | Qualification and performance of rigid boards: what must be achieved |
| IPC-6013 | The same for flexible and flex-rigid boards |
| IPC-A-600 | Acceptability of printed boards: what good and bad look like, with pictures |
| IPC-9252 | Electrical test of bare boards |
| IPC-TM-650 | The test methods the other standards refer to |
| UL 94 and UL 796 | Flammability and safety recognition |
Classes
- Class 1: general electronic products, where function is all that matters.
- Class 2: dedicated service products, where long life and reliable operation are wanted. Most industrial and commercial boards.
- Class 3: high reliability products, where the equipment must work on demand. Tighter limits on plating, annular ring and defects, and more inspection.
How a board is proved
- AOI: optical comparison of each copper layer with the design data.
- Electrical test: every net is checked for continuity and for isolation from its neighbours, against a netlist.
- Microsection: a coupon is cut and polished to measure plating, dielectric thickness and registration inside the board.
- Solderability and thermal stress: samples are floated on solder to show the finish wets and the holes survive.
- Impedance: coupons are measured by TDR where impedance is controlled.
- Dimensional and visual inspection: against the drawing and IPC-A-600.
Paperwork
A certificate of conformance states that the boards meet the drawing and the stated standard. Test reports, microsection reports and first article inspection reports can be supplied when they are ordered.
Design checklist
- State the performance standard and class on the drawing.
- Supply an IPC-D-356 netlist so the test is made against your design intent and not only the Gerber data.
- Only call up the tests and reports you need. Each one adds time and cost.
This hub is general guidance on PCB manufacture and industry standards. It does not describe Wrekin Circuits capabilities. Check your design against what we build in the Engineers Hub.
Designing a board for us to build?
The Knowledge Hub covers how PCBs are made across the industry. To check a design against what Wrekin Circuits builds, use the Engineers Hub, or send your Gerbers and stack-up to our Technical Department.