Cooling channels get most of the attention in mold deep hole drilling — I wrote about those here. But molds have other holes that need to be right, and some of them are harder than the cooling circuits.
Ejector pin holes, guide pin bores, and insert pockets all have their own requirements. I’ve worked on all of them, and each type has tricks you learn by doing. Getting these holes wrong can ruin a mold that took weeks to design and thousands of dollars to machine.
Ejector Pin Holes: Tight Tolerances Matter
Ejector pin holes are probably the most demanding holes in an injection mold. The pin needs to slide freely but not so loose that plastic flashes out. A gap of 0.02mm is the difference between a good mold and one that produces flashing. I once had a mold rejected because three ejector pins were 0.025mm loose — the plastic flashed through the gap and the parts came out with thin fins that required secondary trimming.
For ejector pin holes up to 50mm deep, I can drill and ream in one setup with a carbide gun drill. The surface finish and diameter control are good enough that reaming isn’t needed in most cases. The key is running a double-margin gun drill with through-coolant. The double margin keeps the drill stable in the hole, and the coolant clears chips that would otherwise score the wall. I aim for a surface finish of 0.8 Ra or better on ejector pin bores.
For deeper ejector holes — say through a tall cavity block — I drill undersized and follow with a reamer. The gun drill gets me close, within 0.03mm, and the reamer takes the last bit to final size. This adds an operation but gives more consistent results on long holes. The reamer also corrects any slight drift in the gun drilled bore.
Guide Pin Bores: Alignment Above All
Guide pin bores determine how the mold halves close. If they’re off, the mold shifts and parts come out with witness lines. In multi-cavity molds, misaligned guide bores mean every cavity produces parts out of position.
The challenge with guide bores is depth. A guide pin bore can be 200-400mm deep in a thick mold base, and the straightness requirement is tight. I use BTA drilling on larger diameters (25mm+) and gun drilling on smaller ones. BTA drilling gives better straightness on larger diameters because the tool is self-piloting through the guide pads.
What I’ve learned: drill the guide bores before the cooling channels. If you drill cooling first and then cut the guide bores, the stress relief from the cooling channels moves the block just enough to throw the alignment off. I found this out the hard way on a mold that measured fine until the trial run. The cavities didn’t align and I had to rework the guide bores with sleeving.
Cooling Channel Design Considerations
When I drill cooling channels in mold components, the channel layout matters as much as the drilling parameters. Cooling channels should follow the cavity contour at a consistent distance — typically 8-12 mm from the cavity surface for uniform cooling. Channels that drift closer to the surface create hot spots that cause part warpage.
The channel diameter depends on the mold size and the heat load. For small molds, I use 6-8 mm diameter channels. For large automotive molds, I go up to 14-16 mm. The coolant flow rate needs to maintain turbulent flow (Reynolds number above 4,000) for efficient heat transfer. Laminar flow in a cooling channel cuts heat transfer by 50% or more.
I also connect cooling channels with cross-drilled holes at the ends. The cross holes need to intersect cleanly — I use a 5 mm radius at the intersection corner to reduce pressure drop. Sharp corners at channel intersections create flow restrictions that reduce cooling efficiency.
Insert Pockets and Cavity Details
Some mold inserts need deep holes for cartridge heaters, thermocouple probes, or core cooling. These are usually smaller diameters, sometimes down to 3-4mm, and the depths can be 200-300mm.
Small-diameter drilling in mold steel is unforgiving. A 4mm gun drill at 300mm is a 75:1 L/D ratio — well within gun drilling range, but the feed rate has to be right. Too slow and the chip comes out as powder, which packs up. Too fast and the drill overloads. I’ve broken more 4mm drills than all other sizes combined.
For small-diameter mold work, I use a peck cycle with 30mm retracts. The cycle time is longer, but I’ve broken fewer drills since switching to this approach. The peck lets coolant flush chips from the flute and prevents the chip packing that causes breakage on small drills.
Material Matters
Not all mold steels drill the same. I keep a reference card at each machine listing the parameters for the mold steels we run most often.
| Material | Cutting Speed | Feed Rate | Coolant Type | Coolant Pressure | Notes |
|---|---|---|---|---|---|
| P20 (pre-hardened, 28-36 HRC) | 70-80 m/min | 0.03-0.05 mm/rev | Emulsion 8-10% | 1000-1500 psi | Most consistent, easiest to drill |
| H13 (hardened, 44-52 HRC) | 40-55 m/min | 0.02-0.04 mm/rev | Oil-based | 1500-2000 psi | Reduce speed 35%, watch for work hardening |
| S7 (toughness grade) | 50-65 m/min | 0.025-0.04 mm/rev | Oil-based | 1200-1800 psi | 20% feed reduction vs P20, tougher on tools |
| 420 stainless (corrosion resistant) | 35-50 m/min | 0.02-0.03 mm/rev | Oil-based only | 1500-2000 psi | Emulsion causes BUE — must use oil |
| 1.2083 (ESR stainless) | 30-45 m/min | 0.015-0.03 mm/rev | Oil-based | 1500-2000 psi | Similar to 420 but more abrasive |
| NAK80 (pre-hardened, 37-43 HRC) | 50-65 m/min | 0.025-0.04 mm/rev | Emulsion 8-10% | 1000-1500 psi | Good machinability for higher hardness |
Pre-hardened P20 is the easiest to work with. Hardened H13 needs more care — the key is keeping the cutting zone cool enough to prevent the material from work-hardening ahead of the drill. I’ve had the best results running oil coolant on all mold work; the improvement in surface finish pays for the added cost on any job that needs to pass inspection.
For applications requiring corrosion resistance, like medical or food-grade molds, I use 420 stainless or 1.2083 ESR. These materials demand oil-based coolant because emulsion-based coolants cause built-up edge on the cutting edge. See my BUE prevention guide for more on coolant selection.
Quality Control and Inspection
Every mold hole gets inspected before the mold goes to assembly. For ejector pin holes, I check the diameter with a pin gauge that matches the pin size. The gauge should slide through with light finger pressure but not drop through under its own weight. That tactile check tells me the clearance is right.
For cooling channels, I run a flow test with water at operating pressure. The flow rate at each channel must be within 10% of the design spec. If one leg of a circuit has significantly lower flow, I check for chip blockage or a drill drift that narrowed the channel.
Guide pin bores get checked with an alignment bar that fits both halves of the mold. The bar slides through both guide bushings and confirms they are coaxial. I also check the perpendicularity of each bore to the mold parting surface with a dial indicator. More than 0.02 mm of tilt over 100 mm of bore length needs correction.
For more on cooling channel drilling specifically, see my detailed guide on mold cooling channels. I also cover hot runner manifold drilling for complex mold components and surface finish requirements that apply to ejector pin bores and guide bushings.
Common Problems and Fixes in Mold Drilling
The most persistent problem I see in mold drilling is chip packing in small-diameter cooling channels. When the drill reaches 150 mm+ depth in a 6 mm channel, the chips have a long path to evacuate. If the coolant pressure drops below 1000 psi at the tip, the chips settle and pack.
I solve this by monitoring coolant pressure at the drill inlet and setting a minimum alarm. If pressure drops below the threshold, the machine pauses and retracts the drill before chips can pack. I also use a peck cycle on every cooling channel over 150 mm deep, regardless of diameter.
Drill walking at the start of a long hole is another issue I deal with regularly. The solution is a proper pilot hole drilled to 1.5-2x diameter depth. I use a short, rigid carbide drill for the pilot. The pilot depth must account for the guide bushing gap — if the bushing is 2 mm from the workpiece, the pilot needs to be that much deeper to guide the long drill.
Surface finish problems in ejector pin holes usually trace back to coolant concentration. I check the coolant at least once per shift when running mold work. A refractometer reading below 8% means the coolant film is too thin and the surface finish will degrade.
Key Takeaways
- Ejector pin holes need 0.02 mm clearance — gun drill then ream for consistent results
- Drill guide pin bores before cooling channels to avoid stress-relief misalignment
- Cooling channels need turbulent flow (Re > 4,000) for efficient heat transfer
- Small-diameter mold drills (3-4 mm) need peck cycles to prevent chip packing
- Each mold steel needs different parameters — H13 needs 35% lower speed than P20
- Oil-based coolant prevents BUE on stainless mold steels like 420 and 1.2083
- A consistent 8-12 mm channel-to-cavity distance prevents hot spots in the mold
- Monitor coolant pressure at the drill inlet and set a minimum alarm for deep channels