Why Stainless Threads Fail and How to Specify Them

September 21, 2026

Threads are where stainless parts fail most often, and usually for reasons that were set on the drawing rather than in the machine.

Three separate problems

Broken taps. The tool snaps inside the part. On a part that already has hours of machining in it, this is often a scrapped part.

Galling on assembly. The thread cuts fine and then seizes when a fastener goes in. Covered in more depth in Nitronic 60 and galling, because it is a material problem rather than a machining one.

Stripped or deformed threads in service. Usually an engagement depth or a material strength issue.

They have different causes and different fixes.

Why tapping stainless is hard

A tap is doing the worst possible thing to an austenitic stainless: cutting slowly, with a lot of contact area, in a confined space where heat cannot escape.

Work hardening runs ahead of the tool. The pilot hole surface is already hardened by the drill. The tap then cuts into that.
Torque climbs with depth. Each additional thread adds friction and cutting load. In a blind hole the chips have nowhere to go and they pack at the bottom, which adds more torque again.
The material grips. Stainless closes onto the tap as it heats and expands, so reversing out is loaded too.
Chips are stringy. They wrap rather than break.

So the practical rules are about geometry, and most of them are yours to set.

What to change on the drawing

Reduce thread depth. This is the single biggest lever. For a steel fastener in stainless, one and a half times the nominal diameter gives near full joint strength, because the first three or four engaged threads carry most of the load. A drawing that calls for M8 threaded 24 mm deep is asking for three times the risk and cost for no extra strength.

Allow enough clearance at the bottom of a blind hole. A tap needs run out room. Two to three thread pitches beyond the last full thread lets chips fall clear and lets the tap stop safely. If your design cannot give that, say so, because the shop needs to plan for a bottoming tap or thread milling.

Prefer coarse pitch over fine. Coarse threads cut with fewer, deeper passes, clear chips better and gall less. Fine pitch belongs where you need fine adjustment or thin wall engagement, not as a default.

Avoid tiny threads in hard grades. An M2 thread in 316L or in 17-4 PH H900 is a specialist operation. If the design allows M3, the cost difference is significant.

Consider a thread insert. A stainless part with a threaded steel or bronze insert solves galling, allows repeated assembly and often costs less than trying to make the stainless thread survive. On a part that is opened frequently this is usually the right answer.

Tapping against thread milling

	Tapping	Thread milling
Speed per hole	Faster	Slower
Tool cost	Low per tool, one per size	One cutter covers many sizes
Blind holes	Chip packing risk	Chips clear easily
Failure mode	Tap snaps in the part	Cutter retracts, part is recoverable
Thread size control	Fixed by the tap	Adjustable by the program
Large threads	Impractical above a certain size	Comfortable

For volume production of small threads in a well understood part, tapping is normal and correct. For low volume, expensive parts, large threads, blind holes or hard grades, thread milling is the safer route. The decision is the shop’s, but it belongs in the quote conversation because it changes cycle time.

You do not need to specify the method. You do need to give the shop enough information to choose: thread size, pitch, class, depth of full thread and whether the hole is blind or through.

Thread class and fit

Specify a class. In metric that is 6H for an internal thread and 6g for external, which covers most general work. In unified that is 2B and 2A.

Two notes for stainless specifically:

Do not default to the tightest class. A 4H5H internal thread in 316L is harder to cut, harder to inspect and more prone to galling on assembly than a 6H. Tight thread classes are a real requirement in some applications and an expensive habit in most.

Consider the plating. If the part is plated or coated after threading, the coating thickness changes the effective size. Say whether the thread dimensions apply before or after coating.

Galling on assembly, briefly

A stainless fastener in a stainless thread is one of the most reliable ways to seize a joint. The fix, in order of cost:

Use a different material for one half, for example a steel or bronze fastener
Use anti-seize, if the application allows it and the joint is assembled once
Improve the surface finish on the thread flanks, see the surface finish guide
Use a thread insert
Use a galling resistant grade such as Nitronic 60 for one half

If the joint is in food, pharma or medical service, options 2 is usually off the table and the choice narrows quickly. Say in the RFQ that the thread is repeatedly assembled, because that sentence changes the recommendation.

What to put in the RFQ

Thread size, pitch and class, with the standard
Depth of full thread, and whether the hole is blind or through
What mates with it, and its material
Whether the joint is assembled once or cycled
Whether the thread is plated or coated, and which dimensions apply
Whether a thread gauge report is required

The full checklist has the rest of the drawing, and what tolerances cost covers the same discipline applied to dimensions.

Frequently asked questions

Why do taps break so often in stainless?

The material work hardens ahead of and around the tap, so torque climbs as the tap advances. In a blind hole with chips packing at the bottom, torque can exceed what the tap can carry. It is rarely a bad tap, it is usually a hole that was too deep or too small.

Is thread milling better than tapping for stainless?

For larger threads, blind holes and anything where a broken tool would scrap an expensive part, yes. One cutter covers many sizes, chips clear easily and a jam retracts instead of snapping. It is slower per hole, so on high volume small threads tapping still wins.

How deep should a threaded hole be?

For most stainless applications one and a half times the diameter gives essentially full joint strength. Going to two or three diameters adds cost and risk without adding meaningful strength, because the first few threads carry most of the load.

Need a quote for this part?

Send the drawing. We match you with up to 3 stainless shops and reply within 24 business hours.

Get matched with a stainless shop

Figures in this guide are published specification limits or published typical values for the alloy, not measurements of any part. Machinability is rated against free-machining carbon steel B1112 at 100 and PREN is chromium plus 3.3 times molybdenum plus 16 times nitrogen. The conventions are set out in thereference section and the editorial standards.