Engineers Hub
Check your design against what we build, and compare your options.
Check your design against what we build in our UK factory, compare your options, and get it right before you send your data.
Design Checker: can we build your board?
Enter your board once. We check every line against what we build in our UK factory, tell you what to change, and show your options. Then open any tool below to go deeper.
Paste the report into your quote request or fabrication notes so our engineers see your intent. This check covers the main limits. Our CAM engineers still review every job.
Which laminate material do I need?
The laminate is the glass and resin the copper sits on. It decides how hot the board can get, how fast signals travel and how much they lose. Pick a material family to compare.
Choosing a material
- Start with standard FR4. It suits most products and is the quickest and lowest cost to build.
- Go high-Tg for heat. Lead-free reflow and thick multilayers put more stress on the board. A higher Tg resin copes better.
- Go low-loss for speed and RF. Fast signals and RF lose less energy in low-loss and PTFE materials, and the Dk stays stable.
- We work with leading brands including Arlon, Isola, DuPont, Taconic, Rogers and Ventec. Contact us to confirm material availability or the lead time from the supplier.
Solder resist and legend colours
Choose a resist colour and a legend colour to see how your board will look, and whether the markings will be easy to read.
Specialist boards
Beyond standard rigid boards, we build specialist technologies in the UK. Pick one to see how it works.
PCB glossary
Plain-English meanings for the words you will meet in PCB design and manufacturing.
IPC standards explained
IPC standards set how boards are designed, made and accepted. The class you choose sets how strict the acceptance criteria are.
| Standard | What it covers |
|---|---|
| IPC-2221 | Generic design rules for printed boards, including current capacity and spacing |
| IPC-2141 | Design guide for controlled impedance |
| IPC-4101 | Specification for base materials (laminate and prepreg) |
| IPC-4761 | Via protection types, from tented to filled and capped |
| IPC-6012 | Qualification and performance of rigid boards |
| IPC-A-600 | Visual acceptance of printed boards |
| IPC-D-356 | Netlist format used for electrical test |
What drives the cost of a PCB?
Tick the features your board needs to see which ones add process steps, material or machine time.
A guide to what affects price, not a quote. For a price, send your data to our team.
Can I use this drill size in this board thickness?
Plated through-holes are limited by aspect ratio: board thickness divided by drill diameter. Our limit is 6.4:1, so a 1.6 mm board needs a 0.25 mm drill or larger.
Why the aspect ratio limit exists
- Plating has to reach the middle of the hole. Copper is electroplated from solution that must flow through the barrel. In a long, narrow hole the solution exchange slows down, so the centre of the barrel plates thinner than the ends. Press Run plating to watch it happen.
- Thin barrel copper cracks. FR4 expands far more in Z than copper does. During reflow and thermal cycling the board stretches the barrel, and a thin spot in the middle is where it fractures, often as an intermittent open that passes test and fails in the field. Press Run reflow to see where it gives way.
- Small drills wander in thick boards. On our machines, holes within 6.4:1 stay inside our ±0.038 mm position tolerance. Smaller drills in thicker boards deflect more and are more likely to break, which is why we set the limit there. Press Run drill to see it.
- It is a hard limit. Above 6.4:1 we cannot guarantee copper thickness in the middle of the barrel, so we will not build it. Designing to the limit from the start avoids a re-layout after you have asked for a quote.
Is my pad big enough for this hole?
Annular ring is the copper left around the hole: (pad diameter minus drill diameter) divided by 2. Too little and the drill can break out of the pad.
Why you need more than the minimum ring
- Every hole lands slightly off-centre. Drill position tolerance is ±0.038 mm, and on multilayers each layer pair can register up to ±0.2 mm. The ring is your margin for that movement.
- Breakout weakens the joint. If the hole breaks out of the pad, the connection between the track and the barrel narrows. That is a reliability risk and may fail IPC acceptance.
- Inner layers move more. Layers shrink and shift slightly in lamination, so inner pads need a little more ring than outer pads.
- Bigger rings cost nothing. If the routing allows a larger pad, use it. It improves yield.
What finished hole size will I actually get?
Plated holes are drilled oversize so the finished hole comes out right after copper and finish are added. Enter the finished hole you need.
| Hole size | Plated | Non-plated |
|---|---|---|
| Up to 1.0 mm | ±0.050 mm | ±0.025 mm |
| 1.0 to 2.0 mm | ±0.076 mm | ±0.038 mm |
| Over 2.0 mm | ±0.087 mm | ±0.050 mm |
Why plated holes have wider tolerance
- Plating closes the hole down. Barrel copper and surface finish build up on the hole wall, so we drill larger than the finished size. HASL and tin-lead add more than ENIG or gold, so they need a bigger allowance.
- Plating thickness varies slightly. That variation adds to drill tolerance, which is why plated holes are ±0.05 mm and up, while non-plated holes are drilled straight to size.
- Specify finished size, not drill size. Put finished hole sizes in your drill table and drawing. We work out the tool size.
- Holes over 6.0 mm are routed. Our largest drill is 6.0 mm. Larger holes are cut with the router at ±0.1 mm.
Via covering and filling: which option is right?
IPC-4761 sets out seven ways to protect a via, from a simple tent of solder mask to resin filled and copper capped. Pick a type to see how it is built, what it is good for and what to watch out for.
How to choose
- Under BGAs and fine-pitch parts, close the via. An open via next to a pad can wick solder away from the joint. Filling or covering it stops that and gives assembly a flat surface for vacuum pick-up.
- Avoid trapping anything inside. Tenting and double-sided plugging can trap air, moisture or process chemistry in the hole, which expands in reflow. A fully filled via (Types V to VII) has nothing left inside to trap.
- Via-in-pad needs Type VII. If a via sits inside a component pad, it must be filled and plated over so the pad is flat and solderable. Otherwise solder drains down the hole and starves the joint.
- Mark it in your data. Put the vias to be filled, plugged or capped on their own layer and name the IPC-4761 type in your fabrication notes.
Through, blind and buried vias
A via does not have to go all the way through the board. Pick the layers you want to connect to see what kind of via that is, and how it is built.
What each type means for your board
- Through vias are the simplest. They are drilled and plated once, after the whole board is pressed together. Lowest cost and quickest to build.
- Blind vias connect an outer layer to an inner one. They free up routing space on the layers they do not pass through, which helps under dense BGAs.
- Buried vias connect inner layers only. They are drilled and plated inside the board before the outer layers are added, so they cannot be seen from the outside.
- Each extra structure adds a stage. Blind and buried vias mean building the board in stages (sequential lamination). That adds cost and lead time, so use them where they earn their place, and talk to us early about the stack-up.
Is my track width and spacing OK for this copper weight?
Heavier copper takes longer to etch, and the etchant undercuts sideways as it goes down. So the thicker the copper, the wider the minimum track and gap.
Hole to track clearance
Why heavier copper needs wider tracks and gaps
- Etching works sideways as well as down. To clear 105 µm of copper (3 oz) the etchant also eats into the track edges. Start too narrow and the track ends up thinner than drawn, or gone.
- Narrow gaps in thick copper may not clear. Etchant cannot circulate into a tight slot between two tall copper walls, which leaves copper slivers and shorts.
- Heavy inner layers need more room. The gaps between thick inner copper must be filled with resin during lamination. Wider gaps help the prepreg flow in without voids.
- Outer layers are plated up to the finished weight. Tell us the finished copper weight you need. We start the outer layers on the next weight down and plate up to it, so the track and gap rules for the lighter starting copper apply. For 1 oz finished outers, that means the 0.5 oz rules.
- Fine line is available by arrangement. We can go down to 50 µm (2 thou) on thin copper. Talk to us early so we can plan the stack-up.
How wide should my track be for this current?
Uses the IPC-2221 relationship between current, copper cross-section and temperature rise, then checks the answer against our minimum track for that copper weight.
What drives track width
- Heat, not current, is the limit. A track heats up as current flows through its resistance. The width you need depends on how hot you allow it to get above ambient.
- Inner layers need about 2.6 times the width. Outer tracks lose heat to the air. Inner tracks are buried in FR4, which insulates them, so IPC-2221 halves the allowed current for the same cross-section.
- Heavier copper saves board space. Doubling copper weight roughly halves the width you need. We build from 0.25 oz up to 24 oz, so power tracks do not have to take over your layout.
- Treat it as a starting point. IPC-2221 is conservative and does not account for nearby planes, vias or airflow. Its charts cover up to 35 A and 10 to 100 °C rise.
Thou, mm, inches and copper ounces
Type in any box and the others update. Handy when your CAD tool, datasheet and drawing all use different units.
Can you build this layer count at this thickness?
Pick your board type, layer count and finished thickness. We check it against our published ranges, from 2-layer flex at 0.05 mm to 40-layer multilayer at 8.5 mm.
| Board type | Layers | Thickness |
|---|---|---|
| Single / double-sided | 1 to 2 | 0.05 to 4.8 mm |
| Multilayer | up to 40 | 0.3 to 8.5 mm |
| Flex | 1 to 2 | 0.05 to 0.4 mm |
| Flex-rigid | 2 plus rigid | 0.2 to 4.8 mm |
| Multilayer flex-rigid | up to 16 | 0.2 to 3.2 mm |
Things to know about layer count and thickness
- Each layer needs dielectric. A high layer count in a thin board means very thin cores and prepregs. That is possible, but it limits material choice and affects impedance.
- Even layer counts stay flat. A balanced, symmetrical stack-up resists bow and twist through reflow. Odd counts can be built but usually cost the same as the next even count.
- Thickness drives your drill size. The thicker the board, the larger the smallest plated hole. Check the drill tool once you have picked a thickness.
What stack-up gets me to my target thickness?
Builds a balanced foil-lamination stack-up from the FR4 cores and prepregs we stock, and picks the closest matches to your target. Click a suggestion or pick your own.
How this estimate works
- Foil lamination. Outer layers are copper foil pressed onto prepreg. Inner layers sit on double-sided cores. A 6-layer board uses 2 cores and 3 prepreg gaps.
- Cores from stock. Standard FR4 cores we hold: 0.1 to 1.57 mm. Prepregs: 106, 1080, 2125, 2113, 2116 and 7628.
- It is an estimate. Prepreg flows to fill inner copper when pressed, so the real board comes out slightly thinner. Outer layers include about 25 µm of plating. Our CAM team confirms the final build with your quote.
- Impedance needs a fixed stack-up. If you have controlled impedance lines, agree the stack-up with us first, then lock your track widths.
What track width gives me 50 Ω or 100 Ω?
A quick estimate using the IPC-2141 closed-form equations for microstrip and stripline, single-ended and differential. It also solves the width you need for your target.
Using this estimate
- Good for early layout. Closed-form equations get you close enough to plan routing channels and pick a stack-up.
- Not the final word. Real Er varies with resin content and frequency, and etched tracks are trapezoidal. We confirm the final widths against the agreed stack-up and can adjust them in CAM.
- Tell us which nets. Mark impedance lines in your fab notes with layer, target, tolerance and reference plane. We build single and differential impedance control. TDR test coupons are available on request as a chargeable extra.
- Stay in range. The microstrip equation is most accurate for width-to-height ratios between 0.1 and 2.0.
Which surface finish should I choose?
Tick what matters for your board. The finishes we offer are ranked against your needs, with the thickness range we apply.
Are my solder mask and legend settings OK?
Enter the values from your CAD design rules. Each line is checked against our solder resist and ident capabilities. Hole to track clearance is in the Track and gap tool.
Why these clearances matter
- Mask registers to within a small tolerance. Without at least 0.05 mm clearance, mask can creep onto the pad and stop solder wetting.
- Legend is printed by inkjet. Our minimum ident line is 0.1 mm.
- Legend on a pad gets clipped. Ink on a pad stops it soldering, so our CAM team clips ident back to 0.127 mm (0.005") from the pad: 0.05 mm of resist relief plus 0.076 mm.
Will my board outline and cut-outs work?
Checks board size against our maximum, internal corners and slots against our router cutters, and your tolerances against what we hold.
Why routing has limits
- Router cutters are round. Our standard cutters are 0.6 to 2.4 mm, so the tightest inside corner we can cut has a 0.3 mm radius. Sharp inside corners need a radius on the drawing.
- Slots narrower than the smallest cutter cannot be routed. Use a slot of 0.6 mm or wider.
- Standard tolerance is ±0.1 mm. We can hold ±0.05 mm on request. Only call it up where it is needed, such as enclosure fit or connectors.
Is my data pack ready to quote?
Tick what you have. A complete pack means a faster, more accurate quote and no engineering queries holding up your order.
Every board we build is 100% electrically tested to your data, with AOI on inner layers before lamination.
Figures are Wrekin Circuits standard capabilities for IPC Class 2 build and are a guide only. The drill aspect ratio limit is fixed. Fine-line tracks below the listed minimums may be possible by arrangement. Calculators use published industry equations and are estimates. Your CAM review is the final word.
Need a second opinion on your design?
Everything in this hub is based on what we build in our UK factory. If your design goes beyond it, or you would like it checked before you order, send your Gerbers and stack-up to our Technical Department. We recommend a design review at prototype stage.