Hole Making in Mold Manufacturing: Cooling Channels, Ejector Pin Holes and Threaded Holes

Hole making in mold manufacturing is not one operation but three, and each one fails differently. Cooling channels, ejector pin holes and threaded holes share the same machine and the same spindle, yet they demand different tools, different tolerances and different drilling strategies. Treating them as a single drilling task is where most mold shops lose time.

The gap between what a standard drill can reach and what a mold needs is wider than most process plans assume. Conventional twist drilling holds a practical limit of roughly 3:1 to 5:1 length-to-diameter, extending to about 10:1 with through-coolant high-performance drills, while gun drilling in production use reaches 100:1 (Depth-to-Diameter Ratio: Limits, Selection, 2026-07-23). A cooling channel that must run straight for 400 mm sits well past the first of those numbers.

Hole making in molds covers cooling and heater channels, ejector pin holes, guide pin and dowel bores, fastener holes, vent holes and assembly bores (ALTAY Plastic, Drilling Operations for Injection Mold Manufacturing, 2026-04-03). This guide works through the three that decide mold performance and tooling cost: deep cooling channels, H7 ejector pin holes and threaded holes in hardened steel.

This guide is published by Hiboo Tools, a manufacturer of CNC cutting tools based in Changzhou City, China, producing solid carbide end mills, drills and reamers for precision manufacturing sectors that include mold-making. The company's in-house work covers the design and production of the drills and reamers used for hole making in hardened steels, aluminum and non-ferrous alloys, which is the subject of this article.

Introduction

Hole making in mold manufacturing is not one operation repeated three times. It is three distinct operations with incompatible requirements: cooling channels that must run deep and straight, ejector pin holes that must hold H7 fit, and threaded holes that must survive hardened steel. A strategy that works for one will fail the others.

That distinction matters because the practical limits are unforgiving. Conventional twist drilling holds a depth-to-diameter ratio of roughly 3:1 to 5:1, extending to about 10:1 with through-coolant high-performance drills, while gun drilling in production use reaches 100:1 (Depth-to-Diameter Ratio: Limits, Selection, 2026). Push a standard drill past its class and the hole drifts, the chip packs, and the tool breaks.

Hole making in a mold covers more than cooling lines. It also includes ejector pin holes, guide pin and dowel bores, fastener holes, vent holes and assembly bores, each with its own tolerance and surface requirement (ALTAY Plastic, Drilling Operations for Injection Mold Manufacturing, 2026).

The Three Types of Holes in Mold Manufacturing

Hole making in mold manufacturing splits into three jobs that look alike on a drawing and behave nothing alike at the spindle: cooling channels, ejector pin holes and threaded holes. Each has its own dominant failure mode, and that failure mode, not the hole diameter, decides the tool.

The ejector pin row is a tolerance problem before it is a drilling problem. Ejector pin holes are reamed to H7 and the pins ground to h6 for controlled clearance, with working clearance of roughly 0.02 to 0.05 mm on diameter for 3 to 6 mm pins (Hualong Mold, 2026). The cooling row is a geometry problem: channel wall distance from the cavity surface should stay within 1.5 times the channel diameter, and center-to-center pitch within 3 times the hole diameter (deepholedrilling.org, 2026). Those two constraints pull tool selection in opposite directions.

Why Hole Type Determines Tool Selection

Seven variables separate the three applications, and each one moves the answer to a different tool class.

• Hole depth. Depth-to-diameter ratio drives the failure mode first: chip evacuation at 3:1 to 5:1, coolant delivery at 5:1 to 10:1, tool deflection at 10:1 to 20:1 (deepholedrilling.top, 2026).

• Diameter. Small diameters limit shank stiffness and the coolant volume a tool can pass.

• Tolerance. An H7 ejector pin bore and a nominal clearance hole are not the same operation.

• Mold steel hardness. Pre-hardened and hardened stock change which tool classes survive the cut.

• Blind versus through hole. Blind holes cap chip evacuation and set the usable depth.

• Coolant availability. Through-tool delivery is what makes a carbide deep hole drill with internal coolant viable past roughly 5:1.

• Required surface finish. Finish decides whether drilling alone closes the operation.

Tolerance is the variable readers most often misread. Reaming corrects size, roundness and finish, not position: hole location comes from the drilling setup, and a wrong allowance produces either oversize holes and chatter or residual drilling marks (isocnc.com, undated).

Cooling Channels: How to Drill Deep and Straight Holes

Deep hole drilling for mold cooling channels is a depth-ratio problem before it is a tooling problem. The channel geometry sets the task: conformal cooling design keeps the channel wall within roughly 1.0 to 1.5 times the channel diameter below the cavity surface, with channel pitch held to about 3 to 5 times that diameter, so the hole has to run long and stay where it was aimed. Straightness is a design-and-sequence outcome, not luck. A documented bottle-mold job drilling 4 to 9 mm cooling holes 400 mm deep in cast-iron mold steel held straightness within 0.2 mm over the full 400 mm at a feed of 600 mm/min, a penetration gain of about 500% over the previous method (Deep Hole Drilling Case Studies, Mollart Mexico, retrieved 2026-08-01).

Why Cooling Channel Drilling Is Difficult

The failure mechanism changes with depth ratio, and knowing which one you are fighting tells you what to fix. The ladder runs chip evacuation first, then coolant delivery, then drill deflection, then whipping, then chip transport, then thermal runaway. Below roughly 40:1 length-to-diameter, a CNC mill or lathe with 40 to 70 bar through-tool coolant can carry the job; above 40:1 the process moves to a dedicated deep-hole machine. Gun drilling, the classic answer at the extreme end, holds straightness near 0.001 in/ft, about 0.05 mm per meter.

⚠️ Warning: Above roughly 40:1 L/D, a standard CNC mill stops being the right machine. The dominant failure mode shifts from chip evacuation to thermal runaway, and no drill geometry compensates for that.

How to Choose 3D, 5D, 8D and 12D Deep-Hole Drills

The depth class is the ratio of drilling depth to drill diameter, written as a multiple of D. Conventional twist drilling stays practical to about 3:1 to 5:1 L/D, and through-coolant high-performance drills push that to roughly 10:1. Beyond that, the tool has to be built for the ratio.

Depth variants at 1.5×D, 3×D, 5×D, 8×D and 12×D exist as catalog product lines, and web thickness is the geometry that limits deflection as the ratio climbs (Kyocera Precision Tools, retrieved 2026-08-01).

Do You Need a Spot Drill Before Deep-Hole Drilling?

Not always, but deep holes are far less forgiving of a bad start than shallow ones. Pilot drilling runs 1.5×D to 3×D deep, and inadequate guidance destroys concentricity: an 8 mm drill at 3×D reaches 24 mm before the full-diameter cut even begins (Guehring, Correct deep hole drilling in mould making, 2023-06-28). The standard sequence on a machining centre is finishing, piloting, then deep-hole drilling in stages with successively longer tools for chip control and stability.

Pro Tip: On curved or inclined mold surfaces, a flat drill with a straight main cutting edge can enter up to 45 degrees without deflection, which removes the separate finishing and piloting steps.

Treating every 118-degree drill as universally unsuitable oversimplifies the decision. The question is whether the entry surface and the guidance it provides will hold the hole on location.

Internal Coolant vs. External Coolant

The choice is a pressure and depth band, not a preference. Through-coolant high-performance drills extend the practical limit of conventional drilling to about 10:1 L/D. Below roughly 40:1, a CNC mill or lathe running 40 to 70 bar through-tool coolant handles the work; above 40:1, the process belongs on a dedicated deep-hole machine. External coolant is adequate only for short holes where chips clear on their own and heat has somewhere to go.

Coolant Pressure and Flow for Deep-Hole Drilling

Pressure and flow do different jobs, and the required value depends on drill diameter, depth, material and machine capability rather than a single number. Pressure drives the chip back up the flute and breaks it; flow carries heat out of the cut. Where evacuation is genuinely hard, staged guidance does part of the work: one documented case drilled a 3 mm × 300 mm hole, 100×D, in pre-hardened SKD61 mold steel using a 6.5 mm × 20 mm pilot, a counterbore relief to 140 mm, a guide hole, then continuous drilling (Deep Hole Drilling Case Studies, retrieved 2026-08-01). That sequence exists because coolant alone could not hold the hole straight at that ratio.

Ejector Pin Holes: How to Achieve H7 Accuracy

Ejector pin hole H7 reaming is the step that decides whether a pin slides or binds. An H7 hole paired with an h6 pin is a two-part tolerance system: the hole sets the upper limit, the pin sets the lower one, and the clearance between them is what the mold actually runs on. For 3–6 mm pins, that working clearance is roughly 0.02–0.05 mm on diameter, and the pin protrusion has to stay even within about 0.05 mm across the plate (isocnc.com, What Is Reaming, undated). Miss either half of the pair and the symptom is the same: pins that stick, or flash at the pin.

Why Ejector Pin Holes Require More Than Drilling

Drilling gets you a hole. It does not reliably get you H7. The tolerance band is tight, the surface has to be smooth enough that the pin does not scuff, and the diameter has to hold consistently from the first hole to the last. Reaming is the process that delivers H7 (IT6–IT8) with a surface finish of Ra 0.8–1.6 µm (isocnc.com, What Is Reaming, undated). Four properties have to land together: dimensional accuracy, straightness, surface finish, and a consistent diameter across every pin station. Ejector pin movement depends on all four, because the pin is guided by the full length of the bore, not by its entry.

Drilling vs. Reaming: What Does Each Process Do?

The sequence is spotting, drilling, pre-finishing or enlargement, then reaming. Drilling removes the bulk of the material and creates the hole. Reaming takes the last small allowance and sets final size, roundness, and finish. What reaming does not do is move the hole. It follows the existing bore, so position and straightness are fixed by the drilling setup, not by the reamer (isocnc.com, What Is Reaming, undated). One more caution on specifications: Rz and Ra are different scales, so a drawing that calls out Rz cannot be compared directly against an Ra reaming figure.

Key Takeaway: A reamer follows the existing hole. Position and straightness are set by the drilling setup, not by the reamer.

Drill–Ream Allowance: How Much Material Should Be Left?

A practical starting band is 0.10–0.30 mm total on diameter, or 0.05–0.15 mm per side, which is roughly 2–3% of the hole diameter. The band shifts with size: up to 3 mm, leave 0.05–0.10 mm; at 12–30 mm, leave 0.25–0.40 mm (isocnc.com, What Is Reaming, undated). Those figures are a starting point, not a universal setting. Actual allowance depends on hole diameter, workpiece material, hardness, how accurately the drill held size, and the reamer specification itself. Too much stock pushes the reamer off size and invites chatter; too little leaves drilling marks in the finished bore.

Why Hole Straightness Matters Before Reaming

If a reamed hole comes out off-location, the pre-hole was already off, and the reamer simply followed it. Reaming does not correct position (isocnc.com, What Is Reaming, undated). Straightness is therefore a drilling-stage problem, and the usual causes sit there: drill deflection on deep holes, machine alignment, workpiece setup, and hole entry accuracy. Inadequate guidance destroys concentricity, which is why pilot depths of 1.5×D to 3×D are used to stabilize the drill before it commits to the cut. As a reference point for what a well-controlled deep hole can achieve, gun drilling holds straightness to about 0.001 in/ft, roughly 0.05 mm/m.

Reaming Pre-Hardened vs. Hardened Mold Steel

The H7 target does not change between steel classes, but the reaming strategy does. In pre-hardened grades such as P20, NAK80, and SKD61, the material cuts more predictably and tool wear is slower. Hardened grades such as H13 and S136 shift the balance: cutting parameters come down, coating choice matters more, and the reamer wears faster, so the allowance and the number of holes per tool both need re-checking. The finish and tolerance target stays the same across both classes: H7 (IT6–IT8) at Ra 0.8–1.6 µm (isocnc.com, What Is Reaming, undated). For pre-hardened work, a documented reference case is a 100×D hole drilled in pre-hardened SKD61 mold steel in guided stages, which shows how much of the outcome depends on the drilling setup rather than on the reamer alone.

Threaded Holes: Why Consider Thread Milling Instead of Tapping?

The thread milling vs tapping hardened mold steel decision turns on three variables: steel hardness, whether the hole is blind or through, and whether the machine can interpolate a helical path. Tapping remains the faster cycle when all three favor it. Thread milling becomes the lower-risk choice as hardness rises and as the hole gets harder to recover.

Why Tapping Can Be Risky in Hardened Mold Steel

A tap cuts with multiple teeth engaged at once along its full thread length. That geometry multiplies cutting torque and leaves little room for the chip to clear, and the problem compounds as mold steel hardness rises. In a blind hole the chips have nowhere to go, so they pack into the flutes and drive torque higher still.

The recovery cost is what makes this a tooling decision rather than an inconvenience. A broken tap usually has to be drilled out or burned out, and the removal process can damage the thread flanks around it. Mold assembly tolerances are unforgiving, and a damaged threaded hole in a cavity block is expensive to correct. It does not automatically ruin the mold, but it removes options.

How Thread Milling Works

Thread milling generates the thread by circular interpolation rather than by axial form cutting. The cutter enters the hole, follows a helical path at the thread pitch, and retracts radially before exiting. Because the tool is smaller than the thread diameter, engagement is controlled and the tool can always leave the hole.

That retractable path is why thread milling suits blind holes, where a tap has to reverse out through its own chips. It also means the machine must support helical interpolation, which is the practical prerequisite for the process.

Thread Milling vs. Tapping for Mold Manufacturing

Can One Thread Mill Machine Multiple Thread Sizes?

One thread mill can cover a specified range of thread diameters, which is fewer tools than the equivalent tap set, but it is not one tool for every thread. Two variables set the boundary: the cutter diameter relative to the minor diameter it must enter, and the thread pitch the helical path has to match. A cutter sized for a coarse pitch in a small diameter will not carry the same range as one built for fine pitches.

Select the cutter by the smallest thread it must enter first, then confirm the largest diameter and the pitch range it can interpolate.

How to Select the Right Hole-Making Tool for Mold Manufacturing

Hole making in mold manufacturing comes down to three separate tooling decisions, not one. A cooling channel, an ejector pin hole and a threaded hole each fail for different reasons, so each needs its own selection criteria. Work through the checklist for the hole type in front of you.

For Cooling Channels

Cooling channel drill selection starts with the geometry the mold design already fixed. Channel walls are typically kept to no more than 1.5×D and pitch to no more than 3×D, which sets both the hole diameter and the spacing you have to hit. From there, match the drill to five inputs: hole diameter, depth-to-diameter ratio (3D, 5D, 8D or 12D), whether the machine can deliver through-coolant, the mold steel grade, and how straight the hole must run. If the machine cannot supply high-pressure through-coolant, the practical depth class drops. Deep-hole drilling of mold cooling channels generally needs coolant pressure in the 40–70 bar band, and machines rated around 40:1 depth capability are the threshold for the deeper classes.

For Ejector Pin Holes

Ejector pin hole tool selection is driven by the fit, not the hole. An H7 hole paired with an h6 pin leaves roughly 0.02–0.05 mm of clearance, so the reamer, not the drill, sets the final size. Specify six things: final hole diameter, the H7 tolerance band, hole depth, how accurately the drill can place and align the hole, the reaming allowance left for the reamer, and mold steel hardness. Allowance is not universal. A common working range is 0.10–0.30 mm, banded by diameter, and the achievable tolerance depends on leaving the right amount for the reamer to remove.

For Threaded Holes

Thread milling tool selection depends as much on the machine as on the tool. Confirm six inputs: thread size, pitch, whether the hole is blind or through, mold steel hardness, thread depth, and CNC interpolation capability. That last one is a hard prerequisite. Thread milling is an interpolated operation, so the machine control must support helical interpolation on the relevant axes. Without it, the tool cannot cut the thread regardless of its geometry.

Mold Hole-Making Tool Selection Guide

Hole making in mold manufacturing comes down to matching three variables to one tool: how deep the hole goes, how tight the tolerance is, and how hard the steel is. The table below maps each mold application to its main challenge, the tool that addresses it, and the factors that decide the specification.

Use it as a starting filter, not a final answer. Each row points to the section above that works through the depth class, the drill–ream allowance, or the thread-milling conditions in detail.

Hiboo Tools for Mold Hole-Making Applications

The three hole types in this guide map to three tool classes: deep-hole drills for cooling channels, reamers for ejector pin holes, and thread mills for mold assembly work. Hiboo Tools supplies all three, which matters when you would rather qualify one tooling source than three. The descriptions below stay at the level of capability categories, because no independent test data or published size ranges for these product lines were available for this article.

Carbide Deep-Hole Drills

Hiboo's carbide deep-hole drill line covers the 3D, 5D, 8D and 12D depth classes discussed earlier, with internal-coolant variants for the deeper end of that range. The intended applications are cooling channel drilling and other deep holes where chip evacuation is the limiting factor. If your channel depth falls in the 8×D to 12×D band and your machine has through-coolant capability, this is the class of tool to evaluate against your spindle pressure and flow.

High-Precision Carbide Reamers

For ejector pin holes, Hiboo offers high-precision carbide reamers intended for the finishing pass after drilling. The application requirement they serve is the one set out above: an H7 bore with a surface finish in the Ra 0.8 to 1.6 µm range for precision mold components. Treat that as the target your process must hit, not as a specification quoted from the supplier, and confirm the achievable tolerance against your own material and setup.

Carbide Thread Milling Cutters

Hiboo's carbide thread milling cutters are positioned for mold assembly work, including hardened steel applications and both blind and through threaded holes. Where a single cutter can cover multiple thread sizes, that reduces the tool count you carry for mold work. Custom thread milling solutions are also offered for profiles outside a standard catalog. As with any thread mill, verify the cutter against your thread form, hardness and machine interpolation capability before committing a job to it.

Frequently Asked Questions About Hole Making in Mold Manufacturing

What type of drill is best for mold cooling channels?

A solid carbide deep-hole drill with through-coolant, chosen by depth class rather than by brand. Cooling channels typically run 3×D to 12×D below the cavity surface, and the drill's length-to-diameter rating decides whether it holds straightness and clears chips at that depth. Match the rating to the deepest channel in the mold, not the average.

Should I use a spot drill before drilling a deep cooling channel?

Yes for most deep channels. A spot or pilot establishes the entry point and stops a long drill from walking on an inclined or curved mold surface. Size the spot slightly larger than the drill's web thickness so the chisel edge engages cleanly. On a flat, rigid setup with a stub drill, spotting is optional.

What is the difference between 3D, 5D, 8D and 12D drills?

The number is the drill's maximum depth as a multiple of its diameter, so a 10 mm 8×D drill reaches about 80 mm. As the ratio rises, the tool needs a stiffer shank, tighter runout and higher coolant pressure. A 12×D operation is a different process from 3×D work, not just a longer tool.

When should I use an internal coolant drill?

When depth exceeds roughly 40:1, or whenever chip evacuation fails on an external-coolant setup. Through-coolant drills typically run at 40 to 70 bar, and that pressure flushes chips down the flute instead of letting them pack and snap the tool. If the machine cannot deliver it, reduce depth per pass.

How can I achieve H7 accuracy for ejector pin holes?

Drill undersize, then ream. H7 is a fit tolerance, not a drilling result, and a reamer removes only the small allowance the drill leaves. Keep the drilled hole straight and use a reamer sized to the H7 band for that nominal diameter. The drill sets position and straightness; the reamer sets final size and finish.

Can a reamer correct a misaligned drilled hole?

No. A reamer follows the existing hole, so it cannot pull a hole back to position or straighten a curved axis. Correct the spotting, setup or drill rigidity instead, then re-drill. Reaming a misaligned hole only produces a well-finished hole in the wrong place.

What is the best tool for drilling hardened mold steel?

It depends on hardness. In pre-hardened steel such as SKD61, solid carbide drills still cut and are the usual choice. As hardness climbs into the fully hardened range, drilling becomes marginal and the operation shifts to carbide or CBN alternatives, or to milling the feature. Confirm the actual hardness first.

Is thread milling better than tapping for hardened mold steel?

Often yes, because tapping in hard steel carries high torque and a broken tap is difficult and costly to remove from a mold. Thread milling cuts with a smaller radial engagement and a single tool, which lowers torque and risk. It is not universal: it needs helical interpolation, and cycle time is usually longer.

Conclusion: Matching the Tool to the Hole

Hole making in mold manufacturing comes down to three decisions, and each one follows from what the hole has to do. Cooling channels exist to move heat, so the drill is chosen for depth capability and chip evacuation: a deep-hole drill matched to the depth class, with coolant delivery that reaches the cutting edge. Ejector pin holes exist to locate and guide a pin, so the sequence is drill plus ream, with straightness established before the reamer ever touches the wall. Threaded holes exist to hold a fastener or fitting in steel that may already be hardened, so thread milling gives you the control that tapping cannot reliably deliver at higher hardness.

The payoff for getting these decisions right shows up downstream. Documented mold case studies report cooling-driven cycle reductions from 35 seconds to 20 seconds on a clip component, 19 seconds to 11 seconds on a plastic canister, and 20 seconds to 14 seconds on a circular part whose channels were enlarged from 8 mm to 10 mm (Deep Hole Drilling Case Studies, retrieved 2026-08-01). Process integration compounds it: one mold builder consolidated six setups across two machines into a single hybrid 5-axis operation, saving 6 to 10 hours in the first operation and 10 to 15 percent of total machining time per tool (Deep Hole Drilling Case Studies, retrieved 2026-08-01).

Need help selecting the right carbide cutting tool for your mold?

Send your mold material, hardness, hole diameter, hole depth, tolerance, and thread size, or describe the machining application. Hiboo Tools can recommend a suitable drill, reamer, or thread milling cutter for the operation.