What Is the Difference Between PCB Core and Prepreg?
A PCB core is an already-cured dielectric laminate, commonly supplied with copper on both sides. Prepreg is a resin-impregnated reinforcement sheet that is only partially cured before PCB lamination. Its resin flows during the controlled press cycle, bonds the layers, and cures. In the finished board, both provide solid electrical insulation; prepreg does not remain a soft, half-cured layer.
For a conventional glass-epoxy multilayer PCB, think of the core as a circuit-bearing sheet that can be patterned before the stack is assembled. Prepreg supplies the bonding material around those patterned surfaces. They work together, rather than being competing grades of the same product. This comparison concerns conventional rigid PCB construction, not an aluminum metal-core board or every possible flex and RF material system.
| Question | Core | Prepreg |
|---|---|---|
| What is its resin state before board lamination? | Fully cured, often called C-stage | Partially cured, called B-stage |
| Does it normally arrive with copper? | Copper-clad core commonly has copper on both sides | Ordinary prepreg has no copper foil attached |
| What does it contribute? | A cured dielectric base for copper circuitry | Bonding, filling around copper features, and dielectric separation |
| Which thickness should the designer use? | Confirmed dielectric thickness, with the copper convention stated | Fabricator-confirmed finished, pressed dielectric thickness |
| Can one replace the other directly? | No. A changed construction needs a new stackup review. | |
Do not identify them simply as “thick” and “thin.” Thin cores exist, and several prepreg plies can form one dielectric interval. The useful distinction is their condition and function during manufacture. Altium’s core and prepreg discussion also explains why their electrical properties cannot be reduced to one universal FR-4 value.
Where Do Core and Prepreg Sit in a Four-Layer PCB?
In a common four-layer foil-build construction, the central copper-clad core carries layers L2 and L3. Prepreg bonds outer copper foil to each side, creating L1 and L4. Four layers means four conductive copper layers, not four sheets of insulating material.
Read this simplified stack from top to bottom. It illustrates construction, not a recommended electrical layer assignment or a universal factory stackup.
| Position | Material | How to read it |
|---|---|---|
| L1 | Outer copper | Top conductive layer |
| L1 to L2 | Cured prepreg dielectric | Bonded spacing between top copper and the first inner layer |
| L2 | Core’s upper copper | First inner conductive layer |
| L2 to L3 | Core dielectric | Insulation already cured before final board lamination |
| L3 | Core’s lower copper | Second inner conductive layer |
| L3 to L4 | Cured prepreg dielectric | Bonded spacing to bottom copper |
| L4 | Outer copper | Bottom conductive layer |
A stackup drawing may label a finished dielectric interval “prepreg” because that was the material used to make it. The name records the construction history, not incomplete curing in the delivered board. Solder mask is another insulating coating but is not counted as a copper layer.
Other constructions are possible. For your design, compare the actual layer order with the fabricator’s proposed PCB layer stackup, including which copper layer is the reference plane for each impedance-controlled trace. Do not reorder core and prepreg just to make the CAD display look symmetrical.
How Do You Calculate Core and Prepreg Thickness?
Add each finished dielectric interval and each copper layer once, using a consistent definition of thickness. The two common mistakes are using an unpressed prepreg value and adding core copper a second time when it is already included in the quoted core thickness.
A four-layer thickness example
Assume a hypothetical stack has a 1.00 mm core dielectric, two 0.20 mm finished prepreg intervals, and four copper layers taken as 0.035 mm each for this simplified budget. Then:
1.00 + 0.20 + 0.20 + (4 × 0.035) = 1.54 mm
This is an illustrative nominal sum, not a QFPCB stock construction, a finished-board guarantee, or a fabrication tolerance. Actual outer copper must reflect the agreed finished copper requirement. Solder mask, surface finish, measurement location, and manufacturing tolerances must be handled under the fabrication drawing’s thickness definition.
Now suppose the supplier describes that same core as 1.07 mm including its two 0.035 mm copper layers. The equivalent sum becomes:
1.07 + 0.20 + 0.20 + (2 × 0.035) = 1.54 mm
Adding four copper layers to 1.07 mm would count L2 and L3 twice. Ask one explicit question: “Does this core thickness include copper, or is it dielectric only?” Do not round the example to 1.6 mm and assume the resulting board meets a mechanical drawing.
Check the signal’s local spacing, not only total board thickness
If L2 is the reference plane for a trace on L1 in this example, the relevant L1-to-L2 dielectric interval is 0.20 mm, not the total 1.54 mm. A board can meet total thickness while a changed local spacing still requires an impedance recalculation.
For prepreg, ask for the expected pressed thickness for the proposed construction and copper pattern. Multi-Circuit Boards’ material reference explicitly conditions its example pressed thicknesses on inner-layer copper utilization. A glass-style number alone is not a finished-thickness specification.
Why Do Glass Style, Resin Content and Dk Need Separate Checks?
A glass style identifies reinforcement construction; it does not uniquely specify the resin system, cured thickness, or dielectric constant. To select a usable value, match the material grade, construction, resin content, and the frequency and method behind the data.
For example, the Isola 370HR Dk/Df tables, Revision I, February 24, 2026, list these two core constructions:
- 1 × 1080, 58% resin: 0.064 mm nominal thickness and Dk 4.04 at 1 GHz.
- 1 × 1080, 66% resin: 0.076 mm nominal thickness and Dk 4.02 at 1 GHz.
These are two rows for one named material, not universal 1080 prepreg values. They demonstrate why “use 1080” leaves important questions unanswered. The same table also provides values at multiple frequencies; quoting Dk without the measurement context loses useful information.
Dk, relative permittivity, describes a dielectric’s electrical response and is an input to transmission-line modeling. Df, dissipation factor, concerns dielectric loss. Neither is a simple quality score: a lower number does not automatically make a material right for every circuit.
In an impedance-controlled PCB, trace width, copper thickness, reference-plane spacing, and the appropriate dielectric data work together. Ask which design Dk the fabricator uses for the selected construction. A generic datasheet number and the effective permittivity of a particular trace structure are not interchangeable inputs.
How Should You Approve a Core and Prepreg Stackup?
Approve the finished construction and its performance requirements, not merely a list of glass-style names. A useful approval record connects the mechanical drawing, electrical requirements, material designation, and the fabricator’s proposed build.
Step 1: State the requirements before choosing sheets
Provide the copper-layer count, board thickness and tolerance, finished copper requirements, relevant impedance targets, and any mandatory material designation. Separate fixed requirements from preferences. If a material is only a suggestion, say so; if substitutions are prohibited, make that explicit.
Step 2: Review the fabricator’s proposed construction
Map every dielectric interval to its adjacent copper layers. Confirm which dimensions exclude copper, which prepreg dimensions are pressed values, and which material data support the electrical model. For multilayer PCB manufacturing, resolve these points before finalizing impedance-sensitive routing.
Step 3: Freeze the agreed revision and verification plan
Keep the approved drawing with the fabrication files and purchase requirements. Where impedance or dielectric spacing is critical, agree on the relevant coupon, test report, or cross-section evidence and its acceptance criteria before production. A test result is useful only when it can be traced to the agreed construction and requirement.
Save this stackup approval checklist:
- Layer names and order match the design files.
- Each dielectric interval has a finished thickness and an agreed tolerance where required.
- Core dimensions clearly include or exclude copper.
- Core and prepreg material designations, construction details, and approved alternatives are identified.
- Copper requirements distinguish starting foil from finished copper where relevant.
- Impedance targets identify the signal layers, reference layers, geometry, and acceptance tolerance.
- Required validation evidence and material-substitution approval responsibilities are agreed.
- The final stackup revision matches the drawing, order, and released fabrication files.
Isola’s 370HR processing guide treats its recommendations as starting points that the fabricator must validate. It also describes prepreg as tack-free but somewhat brittle, with storage and handling affecting performance. Consequently, neither a photograph nor a generic press recipe replaces controlled material handling and a qualified process.
Which Material Changes Require Another Review?
Reopen the review when a change affects the electrical model, thickness budget, bonding behavior, or an agreed qualification. Equal nominal thickness is not sufficient proof that two constructions are interchangeable.
| Proposed change | What can change | What to request before acceptance |
|---|---|---|
| Different glass style or resin content | Pressed spacing and dielectric properties | Revised construction, thickness prediction, and electrical review where applicable |
| One prepreg ply replaces several | Resin distribution, reinforcement and process behavior | Fabricator confirmation that the revised build meets the agreed requirements |
| Heavier copper or a changed copper pattern | Resin needed around etched features and local spacing | Updated manufacturability and thickness assessment |
| Another laminate or prepreg grade | Compatibility, thermal and electrical properties | Named equivalent, supporting data and approval before production |
| Different total thickness with the same layer count | Mechanical fit and signal-to-plane distance | Revised stackup and any affected mechanical or impedance checks |
For procurement, the useful question is not “Which sheet is cheaper?” It is “Does the proposed construction meet the same documented requirements, and what must be rechecked?” An alternative may be practical, but approval should happen before it becomes an undocumented production change.
PCB Core vs Prepreg FAQ
Is prepreg the same thing as FR-4?
No. Prepreg describes a material form and its pre-lamination cure state. FR-4 refers to a class of glass-reinforced epoxy laminate materials. A compatible material family may be offered as both core laminate and prepreg.
Does prepreg stay partially cured in the finished PCB?
No. It is partially cured when supplied for lamination, then fully cured through the validated manufacturing cycle. “Prepreg” on a finished stackup drawing describes the construction material used.
Does a two-layer PCB need a separate prepreg bonding layer?
A conventional two-layer rigid board can be made from one double-sided copper-clad laminate without a separate multilayer bonding operation. Special constructions may differ.
Can I replace prepreg with a core of the same thickness?
Not as a direct substitution. A cured core does not provide the same flowing resin needed to bond patterned layers. Changing the construction requires the fabricator to propose and validate a workable stack.
Is core always better for high-speed signals?
No. The selected material system, finished geometry, dielectric data and manufacturing control determine suitability. Both core-based and prepreg-based dielectric intervals can be part of an impedance-controlled design.
What Dk should I enter for 7628 prepreg?
There is no universal 7628 Dk. Obtain the value appropriate to the named resin system, resin content, cured construction, and modeling context. A glass-style code alone is insufficient.
Can I keep my CAD tool’s default stackup?
Use it for preliminary work only until you confirm it matches the proposed fabricated board. Update any material, thickness, and impedance assumptions that differ from the approved construction.
What should I send when asking for a stackup review?
Send the fabrication data, proposed layer order, thickness and copper requirements, impedance table if needed, mandatory material specifications, and substitution restrictions. Identify the file revision so the review and quote refer to the same board.
Preparing a multilayer board for fabrication? Contact QFPCB with those files and requirements, and ask for a proposed core/prepreg construction for review. Confirm the pressed dielectric thicknesses, material designations, and any changes before approving the build.
