Chip AtlasThe Machining Encyclopedia

TroubleshootingTool problems

Tap breakage

Why taps break, in the order to check at the machine: the hole bottom, chips, the hole size, alignment and holding, the cycle, depth, wear, coolant and material; how deep to drill a blind hole; the other tapping faults with their causes and remedies; and when a forming tap or a thread mill is the better tool.

LiveUpdated 17 October 20267 min read

torquefracturestub left in the holepacked chipsblind hole

A tap broken in a blind hole, chips packed under the stub

Drill blind holes at least this much deeper than the tap goes (Haas)
0.050 in
Thread depth beyond which the risk of breakage rises sharply (Haas)
1.5 × d
Tap runout above which some taps break (Haas)
0.03 mm
Cutting volume, opening an M8 × 1.25 tap hole from 6.8 to 6.9 mm (Yamawa)
−15 %

Taps are prone to breaking under high loads, Tungaloy notes, narrow ones especially, and getting a broken tap out of a part is difficult and can damage the part. Haas’s troubleshooting guide and the tables of ISCAR and YG-1 name the same causes again and again. Here they are in the order that is quickest to check at the machine; the general background is in tapping.

Check in this order

0 / 10 checked

  1. 01The tap hits the bottom of the hole

    Check
    The drilled depth against the depth the tap is programmed to; the drill point does not count.
    Fix
    Drill blind holes at least 0.050 in (1.3 mm) deeper than the tap goes. ISCAR adds a tapping holder with axial float and a slipping clutch.

    Haas; ISCAR; YG-1

  2. 02Chips pack in the flutes or the hole

    Check
    The tap type against the hole: a spiral-point tap pushes the chips ahead, so it belongs in through holes only.
    Fix
    Spiral flutes for blind holes, a spiral point for through holes; where the material allows, a forming tap makes no chips at all.

    Haas; YG-1; Seco; Tungaloy

  3. 03The hole is too small

    Check
    Measure the hole and compare it with the tap drill and the 6H limits.
    Fix
    Use the right drill. A slightly larger hole cuts the load: Yamawa reports 15 % less cutting volume for M8 × 1.25 when the hole goes from 6.8 to 6.9 mm, and Haas says a 75 % thread needs a third of the cutting force of a full one.

    ISCAR; YG-1; Yamawa; Haas

  4. 04Tap and hole are not aligned, or the tap runs out

    Check
    The runout (TIR) of the tap in its holder, and the spindle against the hole.
    Fix
    Align the tap with the pre-hole. Haas: some taps break if the runout is more than 0.03 mm (0.001 in); YG-1 suggests a floating holder.

    ISCAR; Haas; YG-1

  5. 05The tap slips in its holder

    Check
    Whether the holder drives the tap by its square.
    Fix
    Hold the tap in a positive-drive holder made for taps, such as ER tap collets with a square drive.

    Haas; Sutton

  6. 06Feed and spindle are out of step

    Check
    The cycle (rigid only with the rigid option; G84 right-hand, G74 left-hand) and the feed: pitch × speed.
    Fix
    Correct cycle and feed; with a compensating holder, a little less than the full pitch (Sutton 95 % for spiral-flute taps, Haas 90 %).

    Seco; Haas; Sutton

  7. 07The thread is too deep

    Check
    The thread depth against the diameter.
    Fix
    Stay near 1.5 × d: Haas says the risk rises sharply beyond it, and thread engagement beyond 1.5 times the fastener diameter adds no strength.

    Haas

  8. 08The tap is blunt

    Check
    Wear on the chamfer teeth.
    Fix
    Regrind or replace it.

    ISCAR; YG-1

  9. 09The lubrication is too weak

    Check
    The coolant concentration, with a refractometer.
    Fix
    More lubricant in the coolant: ISCAR finds general-purpose coolant often too lean for tapping and, where the content cannot be raised, suggests a separate unit that feeds concentrated emulsion to the hole or the tap. To see whether the coolant is to blame, Haas suggests a series of holes with tapping oil or compound brushed on the tap instead.

    Haas; ISCAR

  10. 10Hard material, or a small tap

    Check
    Hardness of the work and size of the tap.
    Fix
    Slower speed and a tap made for the material; Tungaloy recommends a thread mill. For small diameters Haas recommends roll (forming) taps, which are stronger, but only in ductile material: Völkel warns that very hard or brittle material leads to cracks or tool damage.

    Tungaloy; YG-1; Haas; Völkel

How deep to drill a blind hole

One of the commonest causes of breakage needs only arithmetic. To get a full thread to depth L, the tap’s tip has to go deeper by the length of its chamfer, which only cuts incomplete threads; the drilled hole has to go deeper still, and the drill point adds a cone below that. Haas also reminds programmers that the tip angle makes a hole shallower than the programmed depth if it is not allowed for.

full thread 15.00chamfer 4.50clearance 1.27point 2.5520.7719.50tapdrill Øfull thread 15.00chamfer 4.50clearance 1.27point 2.55
Program the tap to
19.50 mm
Drill full Ø to
20.77 mm
Including the point
23.32 mm
The depth chain of a blind hole: full thread, chamfer (the upper end of the makers’ range for the form), Haas’s 0.050 in clearance and an assumed 118° drill point. Tap drills to DIN 336; the drawing is to scale and sized to fit. Point at a result to pick out the part of the chain it adds up.

For an M10 × 1.5 thread 15 mm deep with a form C tap (2–3 chamfer threads), the tap goes to 15 + 3 × 1.5 = 19.5 mm, the drill at full diameter to at least 20.8 mm and the drill point to 23.3 mm. A form B tap, with 3.5–5 chamfer threads (4–5 at YG-1), needs up to 3 mm more. That extra depth is why blind holes with little room below the thread take the short chamfers C and E, although ISCAR advises avoiding E where possible and Seco counts using it where a longer chamfer would fit as a common error that shortens tool life. Form B is a through-hole tap in any case: its spiral point pushes the chips ahead (Haas).

Other tapping faults

ISCAR’s and YG-1’s tables pair each fault with its usual causes:

FaultLikely causesRemedies
Oversize threadWrong tap for the material; misalignment; the tap jams; chips pack; galling; a tap reground off centreA tap for the material group; align; better lubrication and a corrected speed; spiral flutes or a spiral point; regrind concentric
Undersize threadTap limits too small (YG-1)An oversize tap; YG-1 also corrects the chamfer and the cutting angle
Bell-mouthed entryToo little or wrong starting pressureMore starting pressure; a holder with axial float
Stripped threadWrong geometry; spindle and feed out of stepA tap for the material; check the feed, axial float
Rough or torn threadA blunt or badly reground tap; a chamfer too shortRegrind or replace; a longer chamfer (YG-1)
Chipped teethPoor lubrication; chips jamming; the tap hits the bottom; too short a lead after regrindingMore and better coolant; a different tap or speed; a deeper hole; keep the lead when regrinding
Rapid wearIrregular material; wrong speed; lean coolant; a work-hardened pre-holeAdjust speed and coolant; drill the pre-hole carefully; a coated or vanadium HSS tap (YG-1)
GallingMaterial welding to the tapA thread-relieved tap, a surface treatment, proper lubricant, lower speed, a larger hole (YG-1)

Forming taps fail differently

A forming tap does not jam on chips, but it is sensitive to the hole and the lubrication. DC Swiss warns that a hole that is too small gives too big a profile and needs more torque, and that if the lubricant supply is interrupted, cold welding quickly ends the tool’s life. Dormer gives the correction from the thread itself: if material is pushed up at the entry, choose a slightly larger drill; if the profile is not filled, a slightly smaller one. Völkel adds that forming takes about 40–50 % more torque than cutting, so the machine needs that reserve.

When to change the method

Where taps keep breaking, Tungaloy suggests a thread mill: it cuts intermittently with a low and steady cutting force, makes short broken chips, and if it does break, only its fragments have to be removed. The price is programming, since a thread mill follows a helical path (G02/G03 with Z) instead of a fixed tapping cycle. For small threads, Haas recommends forming taps, which are stronger than cutting taps.

Sources (14)

Every value and quotation on this page comes from the documents below.

  1. Haas Automation, Tap breakage troubleshooting guide (last updated 29 March 2023)
  2. Haas Automation, G84 tapping (AP-602, April 2016)
  3. ISCAR, Threading Catalog 62, viewer p. 392: taps troubleshooting
  4. ISCAR, Threading Catalog 62, printed p. 378 (viewer p. 380): chamfer forms to DIN 2197
  5. ISCAR, Tapping Tools user guide (coolant for tapping, p. 21)
  6. YG-1, Synchro taps catalogue section, troubleshooting guide pp. 19 and 21, hosted by Cutwel
  7. YG-1, Prime taps YE-PT19 (troubleshooting), hosted by Cutwel
  8. R. Zdanowski (Seco Tools), “Step-by-step guide: how to choose the right threading tap”, Modern Machine Shop, 1 July 2026 (sponsored content)
  9. Yamawa, AU+SP / AU+SL product sheet, hosted by HH Tools
  10. Sutton Tools, Technical Information application guide (export edition), “Notes on Tapping”, p. 417
  11. Tungaloy, “Troubled by frequent tap breakage? Try a thread mill!”
  12. DC Swiss, thread former catalogue pages
  13. Dormer Pramet, Forming taps brochure (excerpt)
  14. Völkel, “Thread forming: chip-free, clean, reliable”, 3 December 2025