Skip to content
SUS CNC

Home / Guides / Process

Deep Hole Drilling and Tapping Stainless: Where the Cost Appears

Process / 18 Sept 2026

Holes look simple on a drawing. In stainless they are often where the cost quietly lives, because a hole that is slightly too deep or a thread that is slightly too demanding moves the part into a different process.

Depth to diameter, and what each band means

The ratio of hole depth to hole diameter is the number that matters, not the absolute depth.

Ratio Process Cost effect
To 3D Standard jobber drill or insert drill None
3D to 5D Peck cycle, or through coolant drill Small
5D to 10D Dedicated deep hole drill, through coolant essentially required Noticeable
10D to 20D Gun drilling Separate operation, often a separate machine
Over 20D Gun drilling, specialist Separate supplier in many cases

A 5 mm hole 15 mm deep is free. The same 5 mm hole 40 mm deep is an 8D hole and a different conversation.

Why the bands exist: chips have to come out along the flutes, and coolant has to get to the tip. Both get harder as the hole deepens. In stainless both are worse than in carbon steel, because the chips are stringy rather than broken and because the heat has nowhere to go.

Through coolant is the deciding capability. A shop with through spindle coolant and the right drills handles 8D routinely. A shop without it is pecking, which is slow, or it is breaking drills. This is a genuine capability question to ask, not a formality.

Blind versus through

A through hole in stainless is meaningfully easier than a blind one. Chips exit at the bottom, coolant flushes through, and the drill breaks out into air rather than dwelling.

A blind hole has to evacuate everything back up the flutes, and the bottom of the hole is where chips pack. If you have a choice, a through hole costs less.

If the hole must be blind, two things help:

  • Add depth below the functional bottom. A few millimetres of clearance gives the chips somewhere to sit and gives the drill somewhere to break through the work hardened bottom
  • State the drill point condition. A flat bottom blind hole is a separate operation with an end mill. If a standard 118 or 140 degree point is acceptable, say so, because otherwise a cautious shop will price the flat bottom

Tapping, and why taps break

Tapping stainless is the single most common source of scrapped parts late in a process, because it usually happens last, on a part that already carries all its other value.

Three mechanisms:

Work hardening ahead of the tap. The tap deforms material as it forms the thread. In austenitic stainless that deformation transforms austenite to martensite, so the tap is cutting into material it just hardened.

Chip packing. In a blind hole the chips have nowhere to go. Pressure builds until the tap binds.

Heat. Low thermal conductivity means the heat stays in the tap.

What shops do about it:

  • Spiral flute taps for blind holes, which pull chips back out of the hole, and spiral point taps for through holes, which push chips forward
  • Correct hole size for 65 to 75 % thread, never 100 %
  • Thread forming taps on the softer austenitic grades, which produce no chips at all and give a stronger thread, though they need a different hole size and more torque
  • Rigid tapping with the spindle synchronised, rather than a floating holder
  • Through coolant on anything deep
  • Thread milling on large or critical threads, which eliminates tap breakage entirely and costs more cycle time

Thread milling is worth knowing about as a buyer. On an expensive part, a thread milled hole removes the risk of a broken tap destroying a part that already has hours in it. If your part is high value and has a deep or large thread, it is reasonable to ask the shop to thread mill it.

Thread depth, and the number to write

Two numbers, always:

M8 x 1.25 - 6H
Thread depth 12 min
Drill depth 17 min

Give one and the shop guesses the other.

On depth itself, a useful guide for a steel bolt into a stainless part is thread engagement of about 1.5 times the bolt diameter. Beyond 2D the additional pull out strength is negligible, because the load concentrates in the first few threads regardless of how many there are.

So M8 wants about 12 mm of thread, not 24 mm. Specifying 24 mm doubles the tapping time, doubles the tap breakage risk and adds nothing.

Percentage of thread is the other lever. 100 % thread requires a much larger tapping torque than 75 % and is about 5 % stronger. On stainless that trade is clearly wrong. If your drawing is silent, shops will use a standard drill size which typically lands around 70 to 75 %. If you want to be explicit, write it.

Cross holes and intersections

A hole that breaks into another hole is an interrupted cut at the breakthrough, on a surface that may already be work hardened. Drills deflect and break there.

If a cross hole is unavoidable:

  • Say which hole is the primary one, so the shop drills it first and breaks into it rather than out of it where possible
  • Do not put a tight tolerance on the intersection unless it is functional
  • Expect a deburring operation, and specify how the burr at the intersection is to be removed, because reaching a burr inside an intersecting bore is a real problem. Options are hand deburring, thermal deburring, abrasive flow or a specified edge break

Deburring inside intersecting holes on a stainless part is a regular cause of a quote being higher than expected. It is worth asking whether the sharp edge inside the bore actually matters.

What to check on your drawing

  1. Calculate the ratio on every hole. Anything over 5D deserves a second look at whether it needs to be that deep
  2. Through instead of blind wherever the design allows it
  3. Two depths on every blind tapped hole, thread and drill
  4. Thread engagement around 1.5D, not more
  5. Do not specify 100 % thread
  6. State the deburring requirement on intersecting holes, rather than leaving a general note that implies every edge everywhere
  7. Give the tolerance class on threads that will be gauged, per the thread callout guide

If several deep holes are driving the part, it is also worth revisiting the grade. SUS303 drills and taps far more easily than SUS316L, and if the service allows the change it removes the problem at source. See SUS303 vs SUS304 vs SUS316.

Have a part with deep holes or a lot of tapping? Get a quote. An engineer reads it, places it with a shop in our network that has the through coolant and the thread milling capability, and we inspect the parts before they ship. Priced quote within 24 business hours.

Questions

What depth to diameter ratio counts as a deep hole?

Up to about 3 times diameter is a normal drilled hole. From 3 to 5 times needs peck drilling or through coolant. From 5 to 10 times needs a dedicated deep hole drill. Beyond 10 times is gun drilling, a different process with a different machine.

Why do taps break in stainless?

Work hardening and chip packing. The tap deforms the material ahead of itself, creating a hardened layer, while the chips have nowhere to go in a blind hole. The combination loads the tap until it snaps.

Should I specify full depth thread?

No. 65 to 75 per cent thread is standard and is barely weaker than 100 per cent. Full depth thread in stainless dramatically increases tapping torque and tap breakage for almost no gain.

What thread engagement do I actually need?

For a steel bolt into a stainless part, around 1.5 times the bolt diameter is normally sufficient. Beyond 2 times adds almost no pull out strength and adds real cost.

Have a drawing for a stainless part?

Send it and an engineer reads the title block, quotes it within 24 business hours, and if you order we place, manage, inspect and ship the parts on one PO and one invoice.

Get a quote

Related guides