In a multilayer PCB stackup, core and prepreg usually appear together. Both belong to the dielectric material system of a printed circuit board, and both are often made from glass reinforcement and resin. When someone first reviews a PCB stackup, it is therefore easy to assume that they are similar materials with different names.
In practice, they differ substantially in cure state, physical form, and manufacturing function.
A PCB core is a fully cured, rigid laminate that is usually copper-clad on both sides. Prepreg is a resin-impregnated reinforcement that has not completed its final cure before lamination. It is used to insulate and bond adjacent layers in a multilayer PCB.
In multilayer PCB manufacturing, core and prepreg are normally complementary rather than alternative choices. A core can carry previously formed inner-layer circuitry. During lamination, prepreg resin flows and then cures, joining the core, copper foil, and other inner-layer structures into a complete multilayer board.
Understanding the difference between core and prepreg is important for stackup design, finished board thickness, controlled impedance, lamination reliability, and material selection.
PCB Core vs Prepreg at a Glance
| Feature | PCB Core | PCB Prepreg |
|---|---|---|
| Resin State | Fully cured | Partially cured before lamination |
| Physical Form | Rigid laminate | Semi-cured sheet; not a rigid laminate |
| Copper | Usually copper-clad | Normally supplied without copper |
| Main Role | Provides structural dielectric and carries circuit layers | Bonds and insulates adjacent PCB layers |
| During Lamination | Remains relatively dimensionally stable | Resin softens, flows, and completes curing |
| Circuit Pattern | Can carry etched inner-layer circuits | Does not normally carry circuit patterns |
| Thickness | Defined by cured laminate construction | Final pressed thickness depends on construction and resin flow |
In simple terms, core provides a stable dielectric and circuit foundation. Prepreg connects those structures during lamination and becomes the final interlayer dielectric.
PCB Core: The Fully Cured Base Material
A PCB core is a laminate material in which the resin has already completed its cure.
For a common FR-4 multilayer PCB, a typical core can be represented as:
Copper Foil -> Fully Cured FR-4 Laminate -> Copper Foil
This construction is closely related to copper clad laminate (CCL). A laminate manufacturer first produces a cured, copper-clad sheet. The PCB fabricator then transfers the circuit image to the copper on both sides and etches the required inner-layer circuitry.
After the inner-layer circuits have been formed, these cores enter multilayer lamination together with prepreg, outer-layer copper foil, or other cores.
For example, an unprocessed core may begin as:
Copper -> FR-4 -> Copper
After inner-layer imaging and etching, it becomes:
Inner-Layer Circuit -> FR-4 Core -> Inner-Layer Circuit
This is why a core can directly carry signal, power, or ground layers, while prepreg normally does not carry circuit patterns before lamination.
In engineering communication, the terms core and copper clad laminate sometimes overlap. CCL primarily describes the copper-clad laminate material itself, whereas core usually describes the structural role of that cured material within a multilayer PCB stackup.
PCB Prepreg: The Bonding Dielectric
Prepreg is short for pre-impregnated material.
In a typical FR-4 PCB, prepreg is made from woven glass fabric impregnated with an epoxy resin system that has not completed its final cure. The glass reinforcement provides strength and dimensional support. During subsequent lamination, the resin provides filling, electrical insulation, and bonding.
During material production, the glass cloth is impregnated with resin and partially cured so that the resin enters what is commonly called the B-stage. At this point, the material is no longer liquid resin, but it is not fully cured like a core.
When prepreg is placed in a multilayer PCB layup and enters the lamination press, rising temperature reduces the resin viscosity and allows controlled flow. The resin fills spaces between adjacent copper features, pressure brings the layers together, and the resin then crosslinks and completes its cure.
Prepreg -> Heating -> Resin Flow -> Copper Pattern Filling -> Layer Bonding -> Final Cure
Prepreg is sometimes described simply as the “glue” in a multilayer PCB. That description is convenient but incomplete.
Prepreg not only bonds the layers. In the finished PCB, it becomes an actual dielectric layer and helps determine interlayer spacing, impedance, and the mechanical structure of the stackup.
Why Multilayer PCBs Need Both Core and Prepreg
If core and prepreg can both contain glass reinforcement and resin, why does a multilayer PCB need both materials?
The reason is that they perform different manufacturing functions.
A core is already fully cured. It provides a relatively stable dielectric thickness and mechanical structure, and its copper layers can be processed in advance to form inner-layer circuits.
However, stacking two processed cores directly together does not automatically create a reliable multilayer structure. The cores need a dielectric material that can flow during lamination, fill the height differences created by copper patterns, and bond the adjacent structures. Prepreg performs this function.
For example, an etched inner-layer surface is not completely flat. Areas where copper remains and areas where copper has been removed create different surface levels. During lamination, prepreg resin must flow into these regions, fill the spaces around the circuitry, and bond the adjacent layers.
Core = cured circuit-carrying structure; prepreg = bonding and dielectric material during lamination. Their roles are complementary, not competitive.
How Core and Prepreg Form a PCB Stackup
The easiest way to understand core and prepreg is to examine a multilayer PCB stackup.
A simplified four-layer PCB can be represented as:
Top Copper Layer -> Prepreg -> Inner Copper Layer -> Core -> Inner Copper Layer -> Prepreg -> Bottom Copper Layer
In actual manufacturing, the copper on both sides of the center core is first processed into the Layer 2 and Layer 3 circuits. Prepreg and outer copper foil are then laid up above and below the processed core.
The final layup can be summarized as:
Copper Foil -> Prepreg -> Etched Copper / Core / Etched Copper -> Prepreg -> Copper Foil
After multilayer lamination, the prepreg has completed its cure and the entire construction becomes a stable multilayer PCB.
Six-layer, eight-layer, and higher-layer-count PCBs may use several cores and multiple prepreg layers. The basic logic remains the same: core provides cured, circuit-bearing structure, while prepreg forms the interlayer dielectric and completes the bond during lamination.
There is no universal answer for how many cores and prepreg plies to use or how to distribute their thicknesses. The construction must be selected according to finished PCB thickness, copper thickness, impedance targets, layer arrangement, and available rigid PCB manufacturing capabilities.
PCB Core Thickness vs Prepreg Pressed Thickness
Core and prepreg are controlled differently with respect to thickness.
PCB Core Thickness
Because a core is already cured, its thickness is normally defined by the laminate construction. A PCB fabricator selects an appropriate nominal thickness from the standard core constructions available from the material supplier and integrates it into the target stackup.
In a controlled-impedance multilayer PCB, for example, core thickness may directly determine the dielectric distance between two inner layers or between a signal layer and its reference plane.
Core can therefore be treated as a relatively well-defined cured dielectric thickness. Actual production must still account for material tolerance and the results of the complete lamination build.
Prepreg Thickness After Lamination
Prepreg behaves differently. Before it enters the lamination press, it still contains resin that can continue to flow and cure.
Raw prepreg thickness is not the same as the final pressed dielectric thickness.
The final result is affected by:
- Glass fabric style
- Resin content
- Number of prepreg plies
- Adjacent copper thickness
- Copper pattern density
- Resin flow
- Lamination conditions
- The specific laminate system
For example, an adjacent copper layer with a large retained copper area does not require the same filling volume as a layer from which a large amount of copper has been etched. Even when the same prepreg is used, different copper-pattern conditions can produce different pressed dielectric structures. Raw sheet thickness alone is therefore not enough to predict the result.
When calculating finished PCB thickness, it is not sufficient to add core thickness, raw prepreg thickness, and copper thickness mechanically. A production stackup should be based on the pressed thickness calculated by the PCB fabricator for the specific material construction and manufacturing conditions.
Prepreg Glass Styles and Resin Content
Numbers such as 106, 1080, 2116, and 7628 frequently appear in prepreg datasheets and PCB stackups. They generally identify different glass fabric styles.
Different glass fabrics use different yarn structures, weave patterns, and base thicknesses. Combining those glass styles with different resin contents creates prepreg constructions with different thicknesses and performance characteristics.
A relatively thin glass style may be used for smaller dielectric spacing, while a thicker glass construction can contribute to a larger interlayer distance. The final dielectric thickness cannot, however, be determined from a name such as 106 or 2116 alone.
Resin Content
Resin content is another important prepreg parameter. It generally represents the percentage of the prepreg mass made up of resin.
In PCB lamination, resin must not only form the insulating dielectric; it must also fill the spaces left where copper has been etched from adjacent circuit patterns. Lower inner-layer copper coverage means that more volume may need to be filled with resin.
When choosing a prepreg construction, the PCB fabricator must therefore confirm that enough resin volume is available for both filling and bonding.
Resin content also affects the effective dielectric behavior of the finished material because glass fiber and resin have different dielectric properties. A resin-rich construction and a glass-rich construction should not automatically be assumed to have exactly the same Dk, even when both belong to the same laminate family.
Selecting prepreg is fundamentally a matter of combining glass style, resin content, and resin system.
How Core and Prepreg Affect Impedance and Signal Integrity
In an ordinary low-speed PCB, small differences between core and prepreg may not be the main design limitation. In controlled-impedance and high-speed PCBs, however, dielectric material and final thickness directly enter the transmission-line calculation.
Dielectric Thickness
For microstrip and stripline structures, the distance from the signal trace to the reference plane is one of the key factors that determines characteristic impedance. If the actual pressed prepreg thickness differs significantly from the design assumption, the impedance may move away from the target.
A more reliable process is to confirm a manufacturable core and prepreg stackup with the PCB manufacturer, then adjust trace width and spacing according to that final stackup.
Dielectric Constant
Dk should not be reduced to the statement “FR-4 has a Dk of 4.3.” FR-4 is not one material with one fixed dielectric constant.
Actual Dk depends on resin system, glass style, resin content, frequency, material construction, and test method. Even when core and prepreg belong to the same laminate family, differences in glass-to-resin ratio and construction can produce different effective dielectric properties.
Glass Weave Effect
High-speed signals can also be affected by glass weave. Glass fiber and resin do not have identical dielectric properties. When a high-speed differential pair or narrow trace travels for a substantial distance over different parts of the weave, local differences in effective Dk can occur.
This is normally not a primary issue for an ordinary PCB. For very high-speed or timing-sensitive designs, however, glass weave, routing angle, and laminate construction may require further consideration.
What Happens to Prepreg During PCB Lamination?
Multilayer lamination is the most important manufacturing stage for prepreg.
Before pressing, the inner-layer cores undergo circuit formation, inspection, and any required surface treatment. They are then laid up with prepreg and copper foil in the specified stackup order and placed into a controlled heat-and-pressure cycle.
As temperature rises, the resin viscosity in the prepreg initially decreases and the resin begins to flow.
Fill spaces around etched copper patterns -> Remove voids -> Contact adjacent material surfaces -> Form a stable interlayer bond
As temperature and time continue to progress, the resin crosslinks further and completes its cure. After cooling, the material that entered the press as semi-cured prepreg has become a fully cured dielectric structure within the multilayer PCB.
Prepreg describes the material state and product form before PCB lamination. Once lamination is complete, it has become part of the cured dielectric.
Different laminate resin systems do not use identical lamination temperatures, pressures, heating rates, or cure cycles. A single fixed set of temperature, pressure, and time values should therefore not be applied to every PCB prepreg. The actual press cycle must follow the material supplier’s processing guidelines and a manufacturing process validated by the PCB fabricator.
How Core and Prepreg Are Selected for a PCB Stackup
Core and prepreg are not competing materials, so the question is not which one is “better.” In a typical multilayer PCB they perform different roles. The engineering question is which core and prepreg constructions will satisfy the stackup requirements of the board.
Finished PCB Thickness
If the target finished thickness is 1.6 mm, the total thickness of all cores, pressed prepreg, copper, and final surface structures must remain within the board-thickness tolerance. A design should not choose prepreg plies arbitrarily and expect the press to “compress the board to 1.6 mm.” A manufacturable thickness budget should be established in advance.
Layer Count and Layer Arrangement
Four-layer, eight-layer, and sixteen-layer PCBs have different requirements for core and prepreg quantity and thickness distribution. High-layer-count boards must also account for stackup symmetry, warpage, and dimensional stability.
Controlled Impedance
When a design includes 50-ohm single-ended or 90-ohm or 100-ohm differential impedance requirements, core and prepreg dielectric thickness must be selected together with trace width, copper thickness, and material Dk.
Copper Weight
Thicker inner-layer copper creates more pronounced copper topography. Prepreg must provide enough resin volume to fill the spaces around the circuit pattern. Heavy-copper multilayer PCBs therefore place more demanding requirements on prepreg resin content and lamination design.
Material Family
Core and prepreg should normally be combined within a confirmed compatible material system. Standard FR-4, high-Tg, low-loss, and RF laminates offer different core and prepreg constructions. A hybrid-material stackup should not combine unrelated resin systems without engineering review.
When comparing copper clad laminate grades or using IPC laminate classifications, the material designation still needs to be connected to the exact core, prepreg, and processing construction available for production.
Via Structure
Blind vias, buried vias, microvias, and sequential-lamination structures change the conventional single-lamination stackup. Material selection must therefore account for the lamination sequence and final HDI build-up.
Common Core and Prepreg Mistakes
Treating All FR-4 as the Same Material
Specifying only “FR-4” does not fully define the material performance required for a high-speed or high-reliability PCB. Different FR-4 laminate families can have different Tg, CTE, Dk, Df, and resin systems.
Using Raw Prepreg Thickness as Final Dielectric Thickness
Prepreg undergoes resin flow during lamination, so raw sheet thickness cannot be treated as finished dielectric thickness. Controlled-impedance calculations should use the pressed thickness confirmed in the production stackup.
Selecting Core and Prepreg Independently
Core and prepreg are not completely independent materials. A specified laminate family should use confirmed compatible constructions and account for the processing requirements of both the material supplier and PCB manufacturer.
Finalizing Trace Geometry Before the Stackup Is Confirmed
If controlled-impedance trace width is locked before the fabricator confirms the available core and prepreg thicknesses, the circuit geometry may need to be redesigned.
A more practical high-speed PCB workflow is:
Target Layer Structure -> Fabricator Stackup -> Impedance Calculation -> Final Trace Geometry
PCB Core and Prepreg FAQs
Is Prepreg the Same as FR-4?
No. Prepreg describes a PCB material form and cure state, while FR-4 describes a common family of flame-retardant, glass-reinforced epoxy laminate systems. FR-4 can be supplied as laminate or core and can also be supplied as prepreg. There can therefore be both FR-4 core and FR-4 prepreg.
Is PCB Core the Same as Copper Clad Laminate?
They are closely related, but the terms emphasize different aspects. Copper clad laminate is a cured laminate material with copper on one or both sides. In multilayer PCB manufacturing, a double-sided copper-clad cured laminate is commonly used as a core, and inner-layer circuitry is formed on the copper on both sides. Many common PCB cores therefore originate as copper clad laminate.
Does Prepreg Thickness Change During Lamination?
Yes. During lamination, prepreg undergoes resin flow, consolidation, and final cure. Its final pressed thickness is therefore not identical to its original sheet thickness. The actual result depends on glass style, resin content, copper pattern, copper thickness, the number of prepreg plies, and the specific lamination process.
Why Is Prepreg Used Between PCB Cores?
A cured core cannot provide enough resin flow during lamination to fill the spaces around adjacent circuit patterns and create a reliable interlayer bond. When heated, prepreg resin flows around the copper topography and then cures to form the layer-to-layer dielectric and bonding structure.
Can PCB Core and Prepreg Have Different Dk Values?
Yes. Even when core and prepreg belong to the same laminate family, they may use different glass styles, resin contents, and constructions. Their actual dielectric properties are therefore not necessarily identical. Controlled-impedance and high-speed designs should use data for the specific material construction and should be based on the production stackup confirmed by the PCB manufacturer.
Conclusion
PCB core and prepreg are both essential materials in a multilayer PCB stackup, but they perform different manufacturing and structural functions.
A core is a fully cured laminate structure that is usually copper-clad and can carry inner-layer circuitry. Before lamination, prepreg is partially cured. Under heat and pressure, its resin flows and then completes its cure, bonding and insulating adjacent PCB layers.
The most important distinction is not which material has “better” performance, but which problem each material solves in the multilayer PCB.
Core establishes a stable circuit-bearing dielectric structure. Prepreg creates the interlayer bond and final dielectric spacing.
For an ordinary PCB, these differences primarily affect stackup and finished thickness. For a controlled-impedance, high-speed, high-layer-count, heavy-copper, or HDI PCB, core thickness, prepreg glass style, resin content, and pressed dielectric thickness also affect impedance, lamination reliability, and manufacturing feasibility.
A better design process is to define the complete stackup from the layer count, finished board thickness, copper weight, impedance requirements, material family, and via structure. The PCB fabricator can then use available material constructions to establish a stable, manufacturable production stackup.