PCB thickness is the distance between the two outer faces of a manufactured printed circuit board.
A rigid FR-4 PCB often starts at a nominal 1.60 mm, but that value is an industry convention rather than a universal rule. The correct thickness depends on the enclosure, connectors, stackup, copper, holes, mechanical loads, and inspection requirements.
A useful thickness specification must define more than one nominal number. It should also state the allowed tolerance, measurement locations, surface condition, and any connector-edge requirements.
This guide explains how engineers and buyers can turn a common starting value into a manufacturable and inspectable requirement.
Table of Contents
1. What Is PCB Thickness?
PCB thickness is a specified distance through the board’s complete cross-section at an agreed measurement location. It is different from core thickness, dielectric spacing, copper thickness, or the calculated stackup total.
Because suppliers may measure different surface conditions, a drawing should define what “finished” includes and where inspection occurs.
A rigid multilayer board may contain cured cores, prepreg, copper foil, plated copper, solder mask, and surface finish. A flexible circuit can add polyimide film, adhesive, coverlay, and local stiffeners. A metal-core board has another set of thickness components.
Three thickness values often appear during one project:
- Nominal thickness is the target value stated in the drawing or purchase order.
- Calculated stackup thickness is the expected sum of specified dielectric and conductive layers.
- Measured finished thickness is the inspection result obtained under an agreed method.
Those values are related, but they are not automatically identical. Prepreg flow, copper distribution, lamination pressure, plating, and local coatings can change the measured result.
Measurement boundaries also vary. Eurocircuits provides one supplier-specific example. Its finished-thickness method excludes plating, solder mask, and legend from the build calculation. The supplier measures selected laminate areas free of those features. This is an industry practice, not a universal rule.
2. What Is the Standard PCB Thickness?
The most common nominal thickness for a general-purpose rigid FR-4 PCB is about 1.60 mm, often associated with the historical 1/16-inch format. However, IPC does not require every PCB to be 1.60 mm. Product drawings, connector specifications, material availability, and agreed procurement requirements control the final value.
IPC’s board design standards describe IPC-2221 as a generic design standard and IPC-2222 as the sectional design standard for rigid organic printed boards. Their scopes do not establish 1.60 mm as a mandatory thickness for every rigid board.
IPC-6012F addresses qualification and performance requirements for rigid printed boards. It also recognizes procurement selections and requirement deviations. Exact contractual clauses should be checked in the purchased standard and invoked through the customer drawing or purchase order.
2.1. Why Are 1.57 mm and 1.60 mm Both Common?
The historical 1/16-inch value equals exactly 1.5875 mm. The conversion follows the NIST definition of one inch as 25.4 mm.
Modern drawings and catalogs often use 1.57 mm, 1.60 mm, 0.062 inch, or 62 mil as nearby nominal descriptions. They should not be treated as mathematically identical:
Nominal Description | Exact or Converted Value | Typical Engineering Use |
1/16 inch | 1.5875 mm | Exact imperial-to-metric unit conversion |
0.062 inch | 1.5748 mm | Common nominal thickness for inch-based PCB and card specifications |
1.57 mm | 0.06181 inch | Metric nominal thickness used in connector and PCB design documentation |
1.60 mm | 0.06299 inch | Industry-standard nominal PCB thickness for most rigid FR-4 circuit boards |
Manufacturing tolerances may overlap, but overlapping ranges do not make separate nominal dimensions interchangeable. A connector, rail, or card guide can still require one defined nominal value and tolerance.
2.2. Why Are 1.57 mm and 1.60 mm Both Common?
Connector manufacturers frequently distinguish between card thickness and recommended host-board thickness. The exact part drawing should therefore control the mating edge.
Connector Example | Manufacturer-Specified Card Thickness | Design Consideration |
Accepts a 1.57 mm card; recommended PCB range is 1.57–2.36 mm | Check both accepted card size and the wider product range | |
Edge card thickness is 1.57 mm; recommended PCB thickness is 1.60 mm | Do not assume the two catalog fields mean the same thing | |
Specified for a 1.57 mm, or 0.062-inch, card | Control the gold-finger edge to the applicable part specification |
These examples demonstrate the decision process. They do not replace the data sheet for the exact connector installed in your product.
Do You Need Any Help?
3. Which Common PCB Thickness Should You Choose?
Common rigid PCB thicknesses include 0.60, 0.80, 1.00, 1.20, 1.60, 2.00, and 2.40 mm. Use them as planning options, not automatic standards.
The following PCB thickness chart supports early comparison. Availability depends on material, copper weight, layer count, and panel format.
Planning Thickness | Suitable Starting Applications | Main Advantage | Main Risk to Review |
0.20–0.40 mm | Miniature sensors, compact modules, thin rigid circuits | Low profile and light weight | Handling, panel support, bow, twist, and assembly |
0.60 mm | Wearables, compact controls, space-limited modules | Thin construction with greater rigidity than ultra-thin boards | Connector and enclosure fit |
0.80 mm | Keyboards, small communication products, plug-in modules | Good balance between low profile and material availability | Local flexing and unsupported spans |
1.00–1.20 mm | Compact multilayer products and consumer electronics | Moderate rigidity with a reduced board profile | Prepreg availability and impedance geometry |
1.57–1.60 mm | General rigid FR-4 electronics | Widely supported by materials, manufacturing processes, and connectors | May be unnecessary for highly space-constrained designs |
2.00 mm | Industrial controls and larger PCBs | Higher bending stiffness and mechanical strength | Increased weight, drilling depth, and material consumption |
2.40–3.20 mm | Heavy assemblies, backplanes, and specialized mechanical structures | Excellent mechanical support and structural rigidity | Via aspect ratio, connector compatibility, and fabrication process limitations |
Choose PCB thickness through seven connected checks covering mechanical fit, electrical behavior, and realistic fabrication limits.
4. How Should You Choose PCB Thickness?
Choose PCB thickness by resolving the tightest mechanical requirement first, then building a stackup that meets electrical and manufacturing needs.
4.1. Start With the Enclosure and Mating Hardware
Review guide rails, card slots, standoffs, mounting bosses, heat sinks, and neighboring assemblies. Include coating, tolerance, and assembly variation in the mechanical stack. A board that fits the computer-aided design model at nominal dimensions can still interfere at the tolerance limit.
Card-edge connectors deserve a separate controlled dimension. The mating zone may need a local thickness callout, bevel, hard-gold requirement, and inspection location. Press-fit connectors can add another group of hole and board-support requirements.
4.2. Build the Electrical Stackup
Count the required signal, power, ground, and shielding layers. Then select available cores and prepregs with the fabricator. Controlled impedance depends on dielectric spacing, dielectric constant, trace width, copper thickness, and reference-plane geometry.
Do not route critical impedance structures against an assumed generic stackup. Approve the production stackup first, or define which trace dimensions the fabricator may adjust.
4.3. Check Mechanical Loading
Thickness increases bending stiffness when material, board dimensions, and support conditions remain similar. It is not the only way to control deflection. Additional standoffs, shorter unsupported spans, component relocation, or a metal support can be more effective.
Evaluate connector insertion, heavy transformers, vibration, shock, product drop, and manual handling. A thinner board may work safely when the product provides continuous support. A thick board can still flex near large cutouts or poorly placed mounting points.
4.4. Check Holes, Vias, and Assembly Handling
For a through-hole, the aspect ratio is commonly expressed as board thickness divided by drilled-hole diameter. Increasing thickness without increasing the hole diameter makes desmear, activation, and copper plating more difficult.
Thin boards create a different problem. They may need stronger panel frames, carriers, temporary tooling, or adjusted depaneling methods. Review the bare-board and assembly processes, not only the finished product.
4.5. Use a Decision Matrix
Dominant Requirement | Likely Thickness Direction | Required Verification |
Card-Edge Connector | Follow the exact connector nominal | Mating drawing, tolerance, bevel, and gold-finger area |
Low-Profile Enclosure | Consider a thinner PCB | Panel handling, assembly support, and bow/twist |
Heavy Components Or Long Unsupported Spans | Consider more thickness or structural support | Deflection, mounting locations, shock, and vibration |
Controlled Impedance | Let the approved stackup determine geometry | Material Dk, dielectric spacing, copper, trace dimensions, and coupon plan |
Small Drilled Holes In A Thick PCB | Reduce the aspect ratio or change via strategy | Drill diameter, plating capability, reliability class, and microsection plan |
High-Current | Increase copper cross-section before total FR-4 thickness | Trace width, copper thickness, temperature rise, airflow, and heat sinking |
Repeated flexing | Use a purpose-designed flex construction | Bend radius, copper type, coverlay, neutral axis, and stiffener location |
Do You Need Any Help?
5. How Does a Stackup Create Finished PCB Thickness?
Finished PCB thickness develops through material selection, lamination, drilling, plating, imaging, coating, and final inspection. Core and prepreg values provide the main dielectric build, but copper distribution and resin flow influence the pressed result. Local mask or finish can also affect a physical reading when the measurement contacts those features.
A simplified planning equation is:
- Expected stackup thickness = dielectric build + copper build + applicable local coatings
The equation is useful for design planning, but it is not an acceptance method. The drawing must define the actual measurement boundary.
Stackup Element | Contribution To Thickness | What The Engineer Should Confirm |
Core | Cured dielectric, often supplied with copper cladding | Whether the stated core value includes copper |
Prepreg | Resin-coated reinforcement that bonds the stack during lamination | Pressed thickness, resin content, glass style, and copper distribution |
Copper Foil | Starting conductor material | Weight or specified foil thickness |
Plated Copper | Added to hole walls and outer surfaces | Finished copper requirement and its effect on features |
Solder Mask | Local polymer coating over outer circuitry | Whether inspection contacts mask or an uncoated reference area |
Surface Finish | Local finish on exposed copper | Whether the selected finish affects a critical mating surface |
Coverlay Or Stiffener | Flex-circuit insulation or local reinforcement | Region-specific thickness and transition geometry |
Metal Base | Thermal and structural layer in metal-core boards | Base thickness, dielectric thickness, and total finished build |
IPC-4101E separates nominal laminate thickness, metal cladding, and laminate thickness-tolerance classes. IPC-4562B separately addresses metal foil, including copper foil area weights and calculated thicknesses. This separation is why “one-ounce copper” should never be used as a synonym for total board thickness.
The main manufacturing sequence is:
- Select laminate, core, prepreg, and copper constructions.
- Image and etch inner layers when the board is multilayer.
- Stack and laminate the layers under a controlled press cycle.
- Drill holes, desmear the walls, and deposit conductive material.
- Plate and image the outer layers, then etch the conductor pattern.
- Apply solder mask, surface finish, and identifying marks as specified.
- Profile the board and inspect agreed dimensional characteristics.
Each step can interact with thickness. A balanced copper design and an approved press construction help control local variation.
6. How Does Layer Count Affect PCB Thickness?
Layer count influences the available stackup, but it does not determine one mandatory finished thickness. A two-layer board can be thick for mechanical reasons, while an eight-layer board can use thin dielectrics to fit a compact product.
Layer count, dielectric spacing, copper, vias, and material availability must be reviewed together.
Layer Structure | Common Planning Options | Main Engineering Question |
One Or Two Copper Layers | 0.60, 0.80, 1.00, 1.20, or 1.60 mm | How much rigidity and assembly support does the product need? |
Four Copper Layers | 0.80, 1.00, 1.20, 1.60, or 2.00 mm | Can the power/ground spacing and impedance targets fit available materials? |
Six To Eight Copper Layers | Often 1.00–2.40 mm | Do via ratios, registration, and dielectric choices remain manufacturable? |
Higher-Density Multilayer | Project-specific | Does the design require blind, buried, or microvia structures and sequential lamination? |
These are concept-stage planning values, not acceptance ranges. The same nominal thickness can contain several legitimate stackups.
7. What PCB Thickness Tolerance Should You Specify?
Specify the widest PCB thickness tolerance that still protects connector fit, enclosure clearance, assembly, and reliability.
A universal tolerance is unsafe because material type, board thickness, copper distribution, panel size, and measurement method all matter. The approved drawing and purchase order should state both the permitted variation and its inspection basis.
IPC-6012F is the relevant performance specification for rigid boards, but public summaries should not be used to invent a universal total-thickness tolerance.
Use the purchased standard, customer drawing, and agreed supplier capability together.
For laminate measurement, IPC-TM-650 Method 2.2.18 describes mechanical measurement with a micrometer accurate to 0.0025 mm.
It distinguishes base laminate from overall metallic-clad laminate and requires individual readings plus minimum, maximum, and average results unless otherwise specified.
The method concerns laminate measurement; a finished-board inspection plan must still define its own applicable surface and locations.
7.1. Define the Measurement Basis
A complete thickness callout should answer these questions:
- Is the value measured after lamination or after complete fabrication?
- Does the measurement contact solder mask, exposed laminate, copper, or a connector edge?
- Are surface finish, conformal coating, adhesive, or stiffeners included?
- Which drawing zones or coupon locations must be measured?
- Which instrument, contact geometry, and measurement force apply?
- How many readings are required per board or lot?
- Are minimum, maximum, and individual readings reported?
- What happens if the drawing and supplier’s default method conflict?
7.2. Treat UL Thickness as Construction-Specific
UL 796 covers printed-wiring-board safety evaluation. A recognized material or board construction can have a minimum build-up thickness, temperature rating, soldering limit, or other conditions recorded in its UL file.
Do not write “UL requires a 1.6 mm PCB.” Instead, verify the exact recognized construction in UL Product iQ when product safety requirements apply.
Do You Need Any Help?
8. How Does PCB Thickness Affect Electrical and Mechanical Performance?
PCB thickness affects stiffness, connector fit, stackup geometry, drill depth, weight, handling, and cost. It does not independently determine current capacity, controlled impedance, or heat dissipation.
Engineers should separate total board thickness from the conductive and dielectric dimensions that directly control electrical and thermal behavior.
8.1. Mechanical Stiffness
A thicker board generally resists bending better when the material and supported area stay unchanged. Yet stiffness also depends on board length, width, cutouts, mounting points, and component mass.
Do not solve every deflection problem by adding FR-4. A support near a heavy component can reduce bending without increasing the thickness of the complete board.
8.2. Controlled Impedance
Controlled impedance depends primarily on trace width, copper thickness, dielectric spacing, material permittivity, and reference-plane geometry. Solder mask may also affect some surface structures. Total finished thickness matters only through the stackup dimensions that define those transmission lines.
Approve the stackup before releasing critical routing. If the fabricator may adjust trace width, define the allowed change process and the required impedance coupon.
8.3. Current Capacity
A thicker FR-4 base does not automatically let a trace carry more current. IPC-2152 addresses the relationship among current, conductor size, and allowable temperature rise. Its scope centers on copper conductors rather than total board thickness.
For power designs, evaluate copper thickness, trace width, planes, vias, ambient temperature, airflow, heat sinks, and allowed temperature rise.
Heavy-copper PCB design and fabrication may be relevant when conductor cross-section, not board rigidity, is the limiting factor.
8.4. Thermal Performance
More FR-4 does not automatically improve heat transfer. Isola’s 370HR data sheet lists a typical thermal conductivity of 0.4 W/m·K.
That value illustrates why copper planes, thermal vias, interface materials, airflow, and heat sinks often dominate the thermal path.
A metal-core structure can be appropriate when heat must move through a dedicated dielectric into a metal base.
8.5. Via Manufacturability
More thickness increases drill depth. With the same drilled diameter, that raises the through-hole aspect ratio and makes hole-wall preparation and plating more demanding.
Potential responses include increasing hole diameter, reducing board thickness, using blind or buried vias, or changing the layer architecture. The appropriate option depends on routing density, reliability class, cost, and the fabricator’s verified process.
8.6. Cost and Lead Time
Stocked cores, prepregs, and established stackups usually reduce sourcing risk. Ultra-thin boards may require carriers or special panel handling. Thick boards can increase material, drilling time, routing time, and plating difficulty.
Ask for a stackup review before layout freeze. A small early change is usually less disruptive than rerouting controlled-impedance nets after quotation.
9. What Problems Can Incorrect PCB Thickness Cause?
An incorrect or poorly defined PCB thickness can cause connector damage, enclosure interference, warpage, impedance changes, plating risk, and inspection disputes.
The defect is often not the nominal number alone. Missing tolerances, unclear measurement surfaces, or an unapproved stackup frequently create the actual failure.
Problem | Likely Cause | Detection Method | Prevention Or Corrective Action |
Card Will Not Enter A Connector | Mating edge is too thick, coated unexpectedly, or outside tolerance | Measure the controlled edge and compare it with the connector drawing | Add a local edge callout, surface condition, bevel, and inspection location |
Loose Or Intermittent Card Contact | Card edge is too thin or the wrong nominal was used | Inspect edge thickness and perform mating validation | Use the exact connector specification and validate worst-case tolerance |
Board Interferes With Enclosure | Mechanical stack omitted finish or tolerance accumulation | Dimensional inspection and first-article assembly | Complete the enclosure tolerance stack before PCB release |
Thin Board Bows During Assembly | Weak panel support, unbalanced copper, or unsuitable depaneling | Flatness inspection and assembly trial | Improve panel rails, copper balance, carriers, and support tooling |
Finished Thickness Varies Locally | Resin flow and copper distribution differ across the panel | Map readings at defined locations | Balance copper, approve the press build, and define inspection points |
Controlled Impedance Misses Target | Production dielectric or copper differs from the design assumption | Coupon test and stackup review | Approve materials and stackup before routing; control permitted trace adjustments |
Thick-Board Hole Plating Is Unreliable | Aspect ratio exceeds a stable process window | Microsection and electrical test | Increase drill size, reduce thickness, or use another via structure |
Supplier And Customer Disagree At Inspection | “Finished thickness” was never defined | Compare drawings, inspection method, and measurement surface | Add a contractual measurement basis and conflict-resolution rule |
Do You Need Any Help?
11. How Should You Handle Special PCB Types?
Rigid FR-4 thickness rules cannot be copied directly into flex, rigid-flex, metal-core, RF, or High-Density Interconnect (HDI) designs. Each construction has different functional layers, manufacturing constraints, and inspection zones.
Define thickness by region when the board does not have one uniform cross-section.
11.1. Flex PCB
A flex circuit combines polyimide, copper, adhesive or adhesiveless constructions, coverlay, and optional stiffeners.
DuPont’s Pyralux FR data sheet lists copper, adhesive, and Kapton polyimide thicknesses separately. This separation prevents one total-thickness value from hiding the flexible construction.
Select the flex region through bend radius, copper type, layer count, bend cycles, and coverlay. Define local connector stiffeners independently.
Review flex PCB manufacturing when bend zones and reinforced zones need different thickness requirements.
11.2. Rigid-Flex PCB
A rigid-flex drawing should show rigid-island thickness, flex-region thickness, transition geometry, coverlay, adhesives, and stiffeners. One overall number cannot describe every region.
Pay special attention to copper routing across transitions and to the neutral bend axis. Thickness changes near the transition can concentrate strain.
11.3. RF and Microwave PCB
RF stackups depend on material-specific dielectric thickness, design dielectric constant, copper profile, and surface roughness.
Rogers RO4000 material data lists material thickness options and copper claddings as separate product choices.
Use the exact material grade and construction in the field solver. A generic 1.60 mm FR-4 stackup is not a reliable substitute.
11.4. Metal-Core PCB
Specify copper, thermally conductive dielectric, metal base, and total thickness separately. Thermal performance depends strongly on the dielectric layer and interface to the heat sink.
A thick aluminum base cannot compensate for an unsuitable dielectric or poor mechanical contact.
12. What Should You Put in a PCB Fabrication Note?
A PCB fabrication note should state nominal finished thickness, approved tolerance, measurement basis, controlled locations, material, copper, and stackup approval requirements.
The bracketed fields below are intentional template variables; replace each one before releasing a production drawing.
Do not rely on a quotation form’s default value when thickness affects fit or reliability.
The following template is intentionally conservative:
FINISHED BOARD THICKNESS: 1.60 mm ± [APPROVED TOLERANCE]
MEASUREMENT STAGE: AFTER COMPLETE PCB FABRICATION
MEASUREMENT SURFACE: [DEFINE MASKED / UNMASKED / CONNECTOR-EDGE CONDITION]
MEASUREMENT LOCATIONS: [REFERENCE DRAWING ZONES OR COUPON]
LAYER COUNT: [APPROVED VALUE]
BASE MATERIAL: [APPROVED MATERIAL AND GRADE]
OUTER / INNER COPPER: [STARTING AND/OR FINISHED REQUIREMENTS]
CONTROLLED IMPEDANCE: [YES / NO; INCLUDE TARGETS IF YES]
FABRICATOR STACKUP APPROVAL BEFORE PRODUCTION: REQUIRED
FIRST-ARTICLE THICKNESS REPORT: [REQUIRED / NOT REQUIRED]
DEVIATIONS: REQUIRE WRITTEN CUSTOMER APPROVAL BEFORE PRODUCTION
If the connector edge needs a different condition, add a local note. For example, define whether gold, nickel, mask clearance, or bevel geometry is part of the controlled measurement.
13. What Should Engineers and Buyers Confirm Before Ordering?
Engineers and buyers should confirm the same technical baseline before requesting a quote. That baseline includes files, material, layers, copper, finished thickness, tolerance, measurement method, impedance, holes, finish, quantity, and inspection records.
A supplier should explain which values are routine, which require engineering review, and which depend on an approved stackup.
Use this checklist before release:
- Gerber or ODB++ data, NC drill files, board outline, and fabrication drawing
- Nominal thickness and tolerance
- Defined measurement surface and locations
- Exact connector and press-fit part numbers
- Material family, grade, glass-transition requirement, and UL condition when applicable
- Layer count and approved stackup
- Starting and finished copper requirements
- Controlled-impedance targets and coupon requirements
- Minimum drilled holes, via structures, and acceptable aspect ratio
- Surface finish, solder mask, coverlay, stiffeners, and local edge co
- First-article, microsection, dimensional, electrical, or other reporting needs
- Written approval process for material or stackup changes
The following supplier-evaluation table is useful when comparing quotations:
Supplier Question | Evidence To Request | Why It Matters |
Is This Thickness A Routine Construction? | Proposed stackup and material list | Routine builds usually carry less sourcing and process risk |
How Is Finished Thickness Measured? | Written inspection method and measurement drawing | Prevents disputes about mask, copper, and location |
Can The Connector Edge Be Controlled Separately? | Local capability confirmation and first-article plan | Protects insertion force and contact reliability |
Is The Via Aspect Ratio Within A Stable Process? | Drill review and, when needed, microsection plan | Reduces hole-wall preparation and plating risk |
How Are Impedance Changes Controlled? | Coupon plan and stackup approval workflow | Prevents silent dielectric or trace changes |
What Happens If Material Is Unavailable? | Substitution and customer-approval procedure | Preserves electrical and mechanical intent |
Which Values Are Limits Rather Than Routine Capability? | Written DFM response | Separates feasible prototypes from repeatable production |
14. How PCBSAIL Can Help With a Thickness-Critical Project?
We can review the proposed stackup, finished-thickness requirement, material, copper, holes, impedance targets, and mechanical interfaces before production. This review helps expose connector-fit conflicts, unrealistic tolerances, difficult hole aspect ratios, and incomplete acceptance criteria.
Fabrication, assembly, inspection, and testing are then quoted against the released project files rather than assumed from a general capability value.
14.1. Which PCB Thickness Risks Can Be Reviewed?
A thickness review should connect the board drawing to the stackup, drilling plan, assembly data, and product mechanics.
We can review the following risks during design for manufacturability (DFM) and quotation:
- A nominal thickness or tolerance that conflicts with an edge-card connector, enclosure, guide rail, or press-fit feature
- An unclear definition of whether the finished measurement includes solder mask, surface copper, or a localized connector edge
- A stackup that cannot support the required dielectric spacing, copper weight, layer count, and overall thickness together
- A thick board with small mechanical holes that creates an unfavorable plated-through-hole aspect ratio
- A thin board that may need additional panel support or assembly-handling controls
- An impedance target that changes when dielectric thickness, copper thickness, or material availability changes
- A material substitution that affects thickness, electrical behavior, thermal performance, or regulatory requirements
- Missing inspection locations, measurement methods, coupon requirements, or test acceptance criteria.
Do You Need Any Help?
15. FAQ About PCB Thickness
What is the standard PCB thickness?
A general-purpose rigid FR-4 PCB commonly uses a nominal thickness near 1.60 mm. This is an industry convention, not a universal IPC requirement, so the product drawing and approved stackup control.
How thick is a two-layer PCB?
A two-layer PCB can use several finished thicknesses, including common planning values from 0.60 to 1.60 mm. Select the final value from enclosure, connector, rigidity, copper, handling, and supplier requirements.
What is a typical four-layer PCB thickness?
Many four-layer boards use 1.60 mm, while compact designs may use 0.80, 1.00, or 1.20 mm. Approve the core, prepreg, copper, and impedance structure before releasing critical routing.
Are 1.57 mm and 1.60 mm PCB thicknesses the same?
No. They are separate nominal values, although their manufacturing tolerance ranges may overlap. Use the exact dimension and tolerance stated by the connector or mechanical specification.
Does finished PCB thickness include solder mask?
There is no safe universal assumption. Define whether the measurement contacts solder mask, exposed laminate, copper, or a controlled connector edge, and state the locations in the drawing.
Does a thicker PCB carry more current?
Not automatically. Current capacity depends mainly on copper thickness, trace width, temperature rise, airflow, planes, vias, and the complete cooling path.
References
– [IPC Board Design Standards]
– [IPC Document Revision Table]
– [IPC-6012F: Qualification and Performance Specification for Rigid Printed Boards]
– [IPC-4101E: Base Materials for Rigid and Multilayer Printed Boards]
– [IPC-4562B: Metal Foil for Printed Board Applications]
– [IPC-TM-650 2.2.18: Determination of Thickness of Laminates by Mechanical Measurement]
– [IPC-2152: Current-Carrying Capacity in Printed Board Design]
– [NIST Guide to SI Conversion Factors]
– [ISO 10012:2026: Requirements for Measurement Management Systems]
– [UL Printed Wiring Board Resources]
– [Isola 370HR Laminate and Prepreg Data Sheet]
– [Rogers RO4000 Series Data Sheet]
– [DuPont Pyralux FR Copper-Clad Laminate Data Sheet]
