How to Use CNC Grinding to Make a Double-Sided PCB

• 1
  Key takeaways
• 2
  What CNC grinding double-sided PCB work actually removes
• 3
  Layout rules that keep the cutter happy
• 4
  Workholding, leveling and the surface-height map
• 5
  Feeds, speeds and depth per pass
• 6
  Seven steps from blank to finished board
• 7
  CNC grinding vs. etching vs. fab house

The name is misleading. On a PCB, the spindle does not grind in the surface-grinder sense. A small carbide end mill spins at 12,000–24,000 rpm and cuts a shallow channel through the copper foil, isolating the traces you designed. The substrate below is FR-4, Rogers 4350B or an aluminum-backed laminate, and the copper is 18 μm, 35 μm or 70 μm thick.

What makes the process attractive is turnaround. A single board can be cut, drilled and inspected in one day, so a design error costs an afternoon instead of a week. What makes it difficult is depth control, because the useful window between bare laminate and a broken 0.2 mm tool is only a few hundredths of a millimeter.

Two-sided work adds a second problem: registration. When you flip the blank, the bottom pattern must land within about 0.05 mm of the top pattern, or vias will not line up and pads will not meet their traces. Everything in the steps below exists to protect that number.

If your board is more than two layers, or if it carries 0.1 mm traces and 0.2 mm vias, this route is the wrong one. Send it to a fab house. CNC grinding double-sided PCB prototypes pays off between one and twenty boards, at 0.2 mm and coarser.

Design for the tool, not for the etcher. A 0.2 mm two-flute cutter has a real diameter plus runout, so draw traces at 0.25 mm minimum and gaps at 0.2 mm minimum. Anything tighter forces slower feed, more passes and a higher chance of a lifted pad.

Keep copper balanced across the board. Large ground pours on one side and thin traces on the other cause uneven heating during cutting, and thin FR-4 will bow. If you must have a pour, hatch it at 0.5 mm lines with 1.0 mm gaps. That cuts thermal load and gives the cutter an escape route for chips.

Place at least two tooling holes outside the board outline, 3.0 mm diameter, on a diagonal. They become your datum for the flip. Add a third if the panel is longer than 150 mm. Keep 5 mm of clear laminate around each hole so the pin boss does not interfere with the spindle nose.

Pad clearance matters more than trace width in practice. A 0.8 mm pad on a 0.25 mm trace leaves the cutter a 0.2 mm channel to clear on each side. Below that, chips pack into the channel and the tool rubs instead of cutting.

• 1
  Trace and gap floor0.25 mm trace, 0.2 mm gap for a reliable first pass
• 2
  Copper pourHatch at 0.5 mm lines, 1.0 mm gaps
• 3
  Tooling holesTwo or three at 3.0 mm, on a diagonal, outside the outline
• 4
  Board thickness0.8–1.6 mm; thinner stock bows under clamping

Clamp the blank to a sacrificial spoilboard, not to the machine table. MDF or acrylic works; both are flat enough after a facing pass. Face the spoilboard with a 6 mm flat cutter at 0.1 mm depth before every session so the reference surface is true.

Then measure the blank. FR-4 varies 0.05–0.1 mm across a 100 × 100 mm panel, which is more than your whole depth budget. Touch off at four corners plus the center and let the controller build a height map. Most CAM packages store this as a probe grid at 10–20 mm spacing.

Set zero on the copper, not on the laminate. Use a continuity probe or a touch plate. A 0.1 mm error here shows up as either uncut copper or a broken tool on the first pass.

Clean the surface before cutting. Fingerprint oil and dust change the effective depth. Wipe with isopropyl alcohol and let it dry for a minute, then vacuum the spoilboard so chips do not lift the blank off its pins.

Start conservative and tune upward. For a 0.2 mm two-flute carbide cutter in 35 μm copper on FR-4, run 18,000 rpm, 200 mm/min feed, 60 mm/min plunge, and 0.03 mm depth per pass. Two passes reach the 0.05–0.06 mm target.

For a 1.0 mm cutter clearing large areas, 16,000 rpm and 600 mm/min feed with 0.05 mm depth per pass works well. Chip load stays around 0.019 mm per tooth, which is inside the tool maker's range and keeps heat down.

Cut dry. Coolant turns FR-4 dust into a paste that packs the flutes. Use an air blast and a vacuum shoe instead. If the tool squeals, feed is too low. If the edge of the channel looks brown, feed is too high or the tool is dull.

Watch the first 200 mm of travel. If you see a thin copper burr standing along the channel edge, the tool is cutting too shallow. Raise the depth by 0.01 mm and run another test strip before committing to the whole board.