Skip to content
S.B. Electronics Printed circuit boards · since 2000, home page

Engineering guide · Fabrication & materials

What is a PTH PCB? Plated through-holes explained

How a drilled hole in an insulator becomes a copper barrel, how it differs from a non-plated hole, and the design rules that keep plated holes reliable through reflow.
ESP-12E breadboard adapter: two rows of plated through-hole header pads beside the surface pads for the module
FIG. 01ESP-12E breadboard adapter: two rows of plated through-hole header pads beside the surface pads for the module. Board design: ESP-12E breadboard adapter by sigma-prj, CC0-1.0; rendered from its Gerber files.
Written by
S.B. Electronics Engineering Team
Published
Topic
Fabrication & materials
Reading time
8 min · 1,771 words
On this page · 10 sections
  1. 01What is a PTH PCB?
  2. 02What is the difference between PTH and NPTH holes?
  3. 03How are through-holes plated?
  4. 04How thick is the copper in a plated hole?
  5. 05What is annular ring and how big should the pad be?
  6. 06How do you size a hole for a component lead?
  7. 07What types of plated holes are there?
  8. 08When should you choose PTH, and when NON-PTH?
  9. 09How do plated holes affect assembly?
  10. 10What should your drill file say about plating?

Building this board?

Drill a hole through FR-4 and you have a hole through an insulator. Plate its wall with copper and it becomes a conductor that joins every layer it passes through. That plated barrel — the plated through-hole, or PTH — is what turns two copper sides into one circuit, and it is the reason double-sided and multilayer boards exist. This guide explains how a hole is plated, how it differs from a non-plated hole, and the design rules that keep it reliable.

What is a PTH PCB?

A PTH PCB is a printed circuit board whose holes are lined with electroplated copper, so each hole connects the copper on every layer it passes through. PTH stands for plated through-hole. In India the term usually means a double-sided board with plated holes — a double-sided PTH PCB — as distinct from a double-sided NON-PTH board, whose holes are bare. Every multilayer board is a PTH board too: its vias are plated holes that link the inner layers to the outer ones.

A plated hole does two jobs. It is an electrical connection between layers, and it is a mechanical socket for a component lead: solder flows up the barrel and wets the lead along its length, which makes a through-hole joint far stronger than a joint on a single surface.

What is the difference between PTH and NPTH holes?

A non-plated through-hole (NPTH) is a drilled hole with a bare laminate wall. It carries no current and is used for screws, locating pins, connector pegs and tooling. Most PTH boards have both kinds; which hole is which is settled in CAM, so it must be unambiguous in your drill data.

Table 1 · PTH and NPTH holes compared

PropertyPTH — platedNPTH — non-plated
Hole wallElectroplated copper barrelBare laminate
Electrical roleConnects every layer it passes throughNone
Used forComponent leads, vias, press-fit pinsScrews, locating pins, connector pegs, tooling
PadsAnnular ring on each connected layerUsually none, or copper pulled back from the hole
Finished-size tolerance (typical)±0.075 mm±0.05 mm
When drilledBefore platingAfter plating, or masked during plating so no copper builds up
In your dataPlated drill fileSeparate non-plated drill file

Typical industry tolerances. Plating thickness varies slightly, which makes plated hole sizes less exact than bare ones.

A double-sided NON-PTH board has copper on both sides but no plated holes. Its sides connect only through component leads soldered on both sides, or through wire links. It skips the plating stages, so it costs less, and it still suits simple, cost-driven consumer boards. We build both — see double-sided PTH and NON-PTH PCBs.

How are through-holes plated?

Plating a hole means putting metal onto an insulator, which takes several chemical steps. The order below is the order of our own production stages; the chemistry named in each step is the industry's usual route.

  1. CNC drilling. Holes are drilled from your Excellon data; on multilayer boards the drill is registered to targets on the inner layers.
  2. Desmear. Drilling smears resin over the copper edges inside the hole. A permanganate or plasma treatment removes it, so the inner layers make clean contact with the barrel.
  3. Hole metallisation. The bare hole wall is made conductive — typically with a palladium catalyst and a thin film of electroless copper, well under 1 µm thick.
  4. Imaging. Dry-film photoresist is laminated and exposed, leaving the tracks, pads and holes uncovered.
  5. Copper plating. Electrolytic copper builds the barrel to its specified thickness, and a tin layer is commonly plated over it as an etch resist.
  6. Etching. Unwanted copper is etched away while the resist protects the tracks and hole walls; the resist is then stripped.

From there the board moves on to optical inspection, solder mask, surface finish, legend and routing, and then to the electrical test, which proves every plated connection on every net.

How thick is the copper in a plated hole?

Thick enough to survive heat. During reflow the laminate expands far more through its thickness than copper does: standard FR-4 grows roughly 50–70 ppm/°C below its glass transition temperature (Tg) and around 250–300 ppm/°C above it, against about 17 ppm/°C for copper. Every heat cycle stretches the barrel. If it is too thin it cracks, usually at the knee where it meets the pad or at an inner-layer connection.

Fig. 02Plated through-hole · cross-section

AThe plated hole

Hole-wall copper averages 20 µm at Class 2 and 25 µm at Class 3. In reflow the laminate expands far more than copper, so cracks start at the knee.

BWith a soldered lead

Solder rises from the solder side up the barrel; IPC-A-610 Class 2 and 3 look for at least 75% vertical fill.

Hole and ring in proportion · copper and plating drawn thicker than true scale

A plated through-hole in section on a 1.6 mm double-sided board: the barrel, the knee where it turns onto the pad, the annular ring, and the 75% fill line that through-hole joints are judged against at assembly.

Table 2 · Hole-wall copper under IPC-6012

RequirementClass 2Class 3
Average hole-wall copper20 µm25 µm
Minimum in thin spots18 µm20 µm
Typical productsIndustrial, commercial, most consumerProducts that must not fail in service

Values as commonly published for IPC-6012; confirm them against the revision named on your drawing.

Two more choices protect the barrel. A high-Tg laminate stays below its glass transition for more of the reflow profile, so it expands less. And a sensible aspect ratio — board thickness divided by drilled hole diameter — keeps plating even, because deep, narrow holes plate thinner in the middle. As a rule of thumb, keep through-holes under about 8:1; a 1.6 mm board with 0.3 mm holes sits comfortably at about 5:1. IPC Class 2 vs Class 3 covers the rest of the class differences.

What is annular ring and how big should the pad be?

Annular ring is the ring of copper left around a hole after drilling: pad diameter minus hole diameter, divided by two. It absorbs the small errors in drill position and layer registration that every process has. If the ring is too small, the drill can break out of the pad's edge, weakening the joint and, on inner layers, the connection to the track. Our design guideline is 0.15 mm minimum for drilled holes, so every pad should be at least 0.3 mm larger than its finished hole.

Fig. 03Annular ring · breakout by class

01Class 1

Up to 180° breakout: the hole may sit on the pad edge.

02Class 2

Up to 90° breakout permitted on plated holes.

03Class 3

No breakout; at least 50 µm of ring all round.

What a wandering drill does to the ring: IPC Class 1 accepts 180° breakout, Class 2 up to 90° on plated holes, Class 3 none. A 0.15 mm design ring leaves room for drill and registration error before any of these limits is reached.

Table 3 · Minimum pad for a 0.15 mm annular ring

Finished holeMinimum padTypical use
0.3 mm0.6 mmSignal via
0.8 mm1.1 mmAxial resistors and small diodes
1.0 mm1.3 mm2.54 mm-pitch header pins (0.64 mm square)
1.3 mm1.6 mmTerminal blocks and larger connector pins

Minimums. Larger pads solder more easily and survive rework better; use them wherever the layout has room.

How do you size a hole for a component lead?

Specify the finished hole size — the diameter after plating — and leave the drill size to CAM. Fabricators drill plated holes oversize, typically by about 0.1 mm, so the finished hole comes out at your figure once the barrel is plated. For a round lead, a finished hole about 0.2 mm larger than the maximum lead diameter is a common starting point; for a square pin, size from its diagonal. Check the datasheet, which often gives a recommended hole.

Too tight a hole and the lead will not insert, or solder cannot flow past it; too loose and the joint fills poorly and the part sits crooked. Press-fit pins are the exception to every rule of thumb: they need exactly the hole size and tolerance the connector maker specifies, and a flat finish such as ENIG, because HASL changes the hole size.

What types of plated holes are there?

Table 4 · Plated holes and where they are used

TypeWhat it isTypical use
Component holePlated hole with pads, sized for a leadThrough-hole parts, connectors, terminals
Through viaSmall plated hole with no leadCarrying signals and power between layers
Tented viaVia covered by solder maskStopping solder wicking and accidental shorts
Thermal via arrayGrid of vias under a hot componentConducting heat to planes or the opposite side
Castellated holePlated hole cut in half by the board edgeModules soldered flat onto a carrier board
Blind or buried viaVia that stops at an inner layer, or never reaches the surfaceVery dense multilayer designs

Blind and buried vias need sequential lamination, which adds press cycles, cost and time. Most designs up to 12 layers route without them; if yours might need them, raise it before layout, not after — together with any via-in-pad that will need filling.

When should you choose PTH, and when NON-PTH?

  • Choose PTH when routing has to change layers, when there are surface-mount parts on both sides, when the board carries fine-pitch ICs, or when through-hole joints must withstand vibration and thermal cycling. That covers most industrial, instrument and control boards.
  • Choose NON-PTH for simple, cost-driven double-sided boards where every top-to-bottom connection can be made through a soldered lead or a wire link, soldered on both sides.
  • Choose single-sided when one copper layer is enough — power supplies, LED drivers and appliance boards. There is nothing to plate, and it is the lowest-cost construction: see single-sided PCBs.

How do plated holes affect assembly?

Through-hole parts are soldered by wave, selective or hand soldering, and the plated barrel is what lets solder rise from one side to the other. IPC-A-610 asks for at least 75% vertical fill in plated holes for Class 2 and Class 3 work. Two design details decide whether you get it. Pads joined to a copper plane need thermal-relief spokes, or the plane draws the heat away and the solder freezes before it climbs. And vias beside SMT pads should be tented or kept clear, so paste does not wick down the barrel in reflow. SMT vs through-hole assembly covers the processes in detail.

What should your drill file say about plating?

The drill data is the only place a fabricator learns which holes are plated, so make it unambiguous:

  1. Plated and non-plated holes in separate Excellon files, or clearly attributed in one.
  2. Finished hole sizes in the tool table, in the same units as the Gerbers.
  3. No copper pad on a hole that must stay non-plated, unless the fab note says why.
  4. At least the guideline annular ring on every plated hole, on every layer.
  5. Press-fit and tight-tolerance holes listed in the fab note with their tolerance.
  6. Castellated holes and slots drawn on the outline layer and called out in the note.

The Gerber preparation guide covers the rest of the data pack. Rigid one- and two-layer boards, PTH or NON-PTH, can be priced in the instant quote, and our capabilities page lists the drill limits: 0.3 mm mechanical; 0.2 mm for fine-pitch designs.

Written by

S.B. Electronics Engineering Team

The CAM, production and quality engineers at our factory in the Gandhinagar G.I.D.C. Electronics Estate — the people who review incoming data and build the boards. Published .

Ask the engineering team a question

Questions

Questions about PTH PCBs

Short answers to what engineers ask us most often about this subject.

What does PTH stand for on a PCB?

PTH stands for plated through-hole: a hole drilled through the board whose wall is copper-plated, so it connects the copper on every layer it passes through. A PTH PCB is a board built with such holes — usually a double-sided board, as opposed to a NON-PTH board, whose holes are bare.

Is a via a plated through-hole?

Yes. A via is a plated hole used only to connect layers, with no component lead in it. It is usually smaller than a component hole and is often tented with solder mask. Blind and buried vias are variants that stop at, or start from, an inner layer of a multilayer board.

Can a single-sided PCB have plated holes?

Not in a useful sense. Plating connects copper on two or more layers, and a single-sided board has copper on one side only. A design that needs plated holes needs at least a double-sided PTH board; single-sided boards use plain drilled holes, with leads soldered on the copper side.

Why do plated holes come out smaller than the drill?

Because the plated copper, and any HASL coating, line the wall and reduce its diameter. Fabricators drill plated holes oversize to compensate. Specify the finished hole size you need, never the drill size, and let CAM choose the drill that delivers it.

Does S.B. Electronics make both PTH and NON-PTH boards?

Yes, both in-house, alongside single-sided and multilayer boards. Our drill range is 0.3 mm mechanical; 0.2 mm for fine-pitch designs, and every board is electrically tested before dispatch. Rigid one- and two-layer boards can be priced in the instant quote; send anything else through the contact page for an engineer's quote.

Start a project

Send the data. We will check it before we build it.

Price one- and two-layer boards online in seconds, or send the full data pack — Gerbers, drill, fab note, BOM and centroid — and an engineer replies with a reviewed quote.