Drilling, reaming and tapping printed holes

Sometimes the fastest and cheapest way to get an accurate hole is not to print it accurately at all, but to print it slightly undersize and finish it with a conventional machine tool afterward. Drilling, reaming and tapping are all routine steps on FDM parts here, but each interacts with layer structure differently than it would with a homogeneous material like aluminium, and getting the technique wrong causes cracking and delamination rather than a clean finish.

Drilling printed parts without delaminating layers

A layer boundary in an FDM part is a weaker plane than the bulk material within a layer. A drill bit that grabs and pulls, rather than cutting cleanly, can pry a layer apart before it cuts through it, especially near the exit side of a hole where there is less material left to resist the axial force. This is the single most common cause of cracked or split holes we see in customer-drilled parts.

1. Use a sharp bit with a standard point angle around 118 degrees, not a heavily worn or aggressive-flute bit intended for metal.
2. Clamp the part firmly and support it directly under the drill point so there is no unsupported span that can flex or crack as the bit breaks through.
3. Run a moderate spindle speed and feed rate rather than pushing hard. Let the bit cut rather than forcing it, since printed plastic melts and smears at excessive speed.
4. Peck-drill for anything deeper than about three times the bit diameter, retracting periodically to clear chips and reduce heat buildup.
5. Slow down and reduce feed pressure just before breakthrough on the far side, where delamination risk is highest.

Undersizing for a reamed final size

When a bore needs a tolerance tighter than printing alone reliably delivers, the standard approach is to print the hole 0.3 to 0.5 mm undersize on diameter and ream it to final size afterward. Reaming removes a thin, controlled shell of material with a cutting edge designed for a light, consistent cut, producing a round, smooth bore that does not depend on how well the printer happened to hold tolerance that day.

Do not try to remove more than about 0.5 mm with a reamer in a single pass on printed plastic. A reamer is a finishing tool, not a roughing tool, and pushing it to remove a lot of material generates heat that can locally melt or glaze the bore surface rather than cutting it cleanly. If more material needs to come out, drill first with an intermediate bit and ream last for the final 0.1 to 0.2 mm.

Tapping threads into printed material

Cutting a thread directly into a printed hole works reasonably well for occasional-use fasteners in stiffer materials like PC, PA12 or PA12-CF, and less well for repeated assembly cycles or soft materials like PLA, where the thread flanks wear down after a handful of insertions. Drill the tap hole to the correct tap drill size for the thread, generally the same sizes used for metal, and cut the thread with a spiral point or spiral flute tap rather than a straight flute tap where possible, since these clear chips forward and reduce the risk of splitting the surrounding material.

For threads that will see repeated assembly, high torque, or need to hold up over the life of the product, a threaded metal insert pressed or heat-set into the printed hole is a more durable answer than a printed or tapped thread, and is covered in the threads cluster of this guide library.

When post-machining is cheaper than tightening the print process

Getting a printed hole to a tight tolerance directly, by fine-tuning slicer settings, running calibration prints and locking down machine parameters, takes engineering time and print iterations that add up in cost, particularly for a single hole on an otherwise non-critical part. A five minute drilling and reaming operation on a finished part is very often cheaper overall, especially for low to medium volumes, because it decouples the hole tolerance from the variability of the print process entirely.

The calculation flips for very high volumes or very large hole counts per part, where the per-part machining time starts to dominate the cost, or for holes that are genuinely impossible to access with a drill or reamer after printing because of surrounding geometry. In those cases it is worth investing the time to tune the print process itself, or to design the part so critical holes are accessible for finishing, or split into halves so the tool has clear access. This tradeoff is exactly the kind of thing we look at during a DFM review before quoting a production run.