When an FR-4 layout moves to a ceramic substrate, the circuit itself rarely needs much change. The fabrication data does. Routed outlines, mechanical drilling, V-cut panels and multilayer lamination are either impossible on ceramic or replaced by a different process. Gerbers prepared with FR-4 habits usually lead to several rounds of engineering queries, or to outlines and holes being reworked to the fab's own defaults.
This article covers one question: which parameters in the design files must be rewritten for a ceramic PCB, and which must be confirmed with the fab before release. Material and process selection (Al2O3 vs AlN, DPC vs DBC) is covered in ceramic PCB materials and DPC/DBC processes. Hole forming and singulation in depth are covered in ceramic substrate hole forming and singulation constraints.
Decide two things first: substrate and metallization
Ceramic PCB design rules are not one universal table. Two choices set them:
- Substrate: Al2O3 (alumina) or AlN (aluminium nitride); the SKPCB product page also lists Si3N4. The substrate sets the available thicknesses, thermal behaviour and brittleness.
- Metallization: DPC (direct plated copper: sputtered seed layer, electroplated build-up, photolithographic patterning) or DBC (direct bonded copper: copper foil bonded to the ceramic at high temperature, then etched).
A line/space that is easy on DPC may be impossible on thick DBC copper. The first line of the fabrication notes should therefore state substrate, metallization process and copper thickness. Without it, no other rule has a reference.
Outline: no router, only a laser
On FR-4 the outline is a router path, internal corner radii follow the cutter diameter, and odd shapes cost little extra. Sintered ceramic is hard and brittle. Outlines are usually laser-scribed and snapped, or laser-cut through. That changes the design inputs:
- Separate "scribe" from "cut-through" in the outline layer. Scribe lines run straight from edge to edge and suit rectangular units. Arcs, notches and internal cut-outs need laser cut-through, which takes longer.
- Specify internal corner radii. A sharp internal corner is a crack starter on ceramic. Put the radius requirement on the drawing instead of inheriting a router default.
- Pull copper back from the edge. Scribed and snapped edges are less clean than routed ones; copper at the edge can chip or lift during singulation. Confirm the pull-back with the fab instead of reusing the FR-4 value.
- Choose thickness from the standard range. Ceramic substrates come in fixed thicknesses; you cannot build an arbitrary thickness from prepreg the way you can on FR-4. Ask for the available list before fixing the mechanical design.
Holes: laser holes taper, DBC usually has no plated vias
On FR-4, a hole is the cheapest feature on the board. On ceramic, holes are formed before sintering or laser-drilled afterwards, and both routes are more constrained than mechanical drilling.
- Hole diameter has a lower limit relative to thickness. Laser holes taper: larger at entry, smaller at exit. State in the drill file or drawing whether the diameter refers to entry or exit.
- DPC vias are filled by plating. Whether the via is fully filled or wall-plated only, and whether the surface must be planar, decides if a pad can sit on top. Write it into the data.
- DBC normally has no plated through-vias. The two copper sides are independent. If the FR-4 design relies on vias to connect top and bottom, a DBC version needs single-sided routing, or a move to DPC.
- Mounting and shaped holes are laser-cut and share the edge-chipping risk, so hole-to-copper and hole-to-edge distances should be enlarged to the fab's confirmed values.
Conductors: line/space follows copper thickness
On FR-4 most designers fix line/space first, then pick 1 oz or 2 oz copper. On ceramic, reverse the order: fix copper thickness first, then check the minimum line/space that thickness allows.
- DPC: copper is plated up and patterned by photolithography, so it suits fine lines. Thicker copper means more undercut and more line-width deviation.
- DBC: the foil starts thick and is etched, so minimum spacing is tied directly to copper thickness. Fine-line capability is clearly weaker than DPC. DBC suits high-current power loops, not dense signal routing.
- Large copper areas need a relief rule. Copper and ceramic expand very differently, so a solid copper plane stresses the ceramic during thermal cycling. Confirm with the fab whether planes should be segmented and whether top and bottom copper areas should be balanced.
Actual line/space values come from the fab's capability for the stated substrate, process and copper thickness. Mark critical nets (high-current paths, bond areas, fine-line regions) separately in the files so the fab can check them one by one.
Layer count and surface finish
- Layer count: FR-4 solves routing density with multilayer lamination. Standard DPC/DBC ceramic boards are mostly single- or double-sided. If the original design has four or more layers, first check whether it can collapse to two sides, or whether another substrate fits better.
- Solder mask: ceramic boards often have no solder mask, or only local mask. Fine-pitch pads that rely on mask to prevent bridging need a feasibility check on mask, colour and thickness.
- Surface finish: wire bonding (gold or aluminium), soldering and silver sintering each have their own finish requirements. Define the finish by area, for example "bond area / solder area", rather than one finish for the whole board.
Panelization: no V-cut, tabs need a redesign
FR-4 panels usually use V-cut or mouse-bite tabs. Ceramic has no V-cut. The alternatives are laser scribe and snap, or laser cut-through with retaining tabs.
- Spacing between units must allow for the scribe line or kerf width. Zero-gap V-cut layouts from FR-4 do not transfer.
- Rails, tooling holes and fiducials must be laid out again on the ceramic master card, whose size is set by the incoming substrate format.
- If assembly needs the full panel through reflow before singulation, say so. The fab will choose scribe depth or tab style accordingly.
Data checklist for the fab
| Item | FR-4 habit | Add for a ceramic PCB |
|---|---|---|
| Material | Laminate type + thickness | Substrate (Al2O3/AlN) + metallization (DPC/DBC) + copper thickness |
| Outline | Router path | Scribe vs cut-through, internal radii, copper-to-edge distance |
| Holes | Drill table | Entry/exit diameter definition, filled or not, hole-to-edge distance |
| Conductors | Line/space | Minimum line/space checked against copper thickness, plane relief |
| Finish | One finish | Finish per area: bonding / soldering |
| Panel | V-cut / tabs | Scribe or kerf spacing, master card size, singulation timing |
You can attach this table to the RFQ package. The more of it is filled in, the fewer engineering queries come back.
Ceramic PCB production at SKPCB
The SKPCB ceramic PCB product page lists the available substrates: Al2O3, AlN and Si3N4. Thickness, line/space and hole capability are confirmed per project during engineering review. Send Gerbers with the information above through the quote page to start that review.
Summary
Moving from FR-4 to ceramic usually leaves the circuit unchanged and changes the fabrication data: outlines are written for laser processing, holes are redefined for taper and fill, line/space is checked against copper thickness, and panels drop V-cut. Put substrate, metallization and copper thickness on the first line, and every other parameter has a reference.
FAQ
Q: Can FR-4 Gerbers be used directly for a ceramic PCB?
A: The copper layers usually carry over. Outline, drill, panel and finish information must be supplemented for the ceramic process. Without it, the fab can only apply its own defaults.
Q: Does choosing DPC or DBC change the design rules much?
A: Yes. DPC suits fine lines and vias; DBC suits thick copper and high current but has weaker fine-line capability and normally no plated vias. Choose the process first, then the rules.
Q: Can a ceramic PCB have a non-rectangular outline?
A: Yes, by laser cut-through. Straight rectangular outlines can be scribed and snapped, which is simpler. Shaped outlines take longer and internal corners should have radii.
Q: Can ceramic PCBs be multilayer?
A: Standard DPC/DBC boards are mostly single- or double-sided. Multilayer requirements need a separate evaluation with the fab.
Q: Does a ceramic PCB need solder mask?
A: Many ceramic boards use no mask or only local mask. Designs that depend on mask between fine-pitch pads should confirm feasibility first.
Q: What is the minimum information for a ceramic PCB quote?
A: Substrate, metallization process, copper thickness, board thickness, outline method, hole definition, finish by area and panel method. The table above works as a checklist.