Tap Drill Depth: How Deep to Drill a Blind Tapped Hole
Tap drill depth for a blind hole is the full-thread depth plus room for the tap's chamfer and chips. How machinists size it and how to put it on a print.
Ask five machinists about tap drill depth and you'll get five numbers. They'll all agree on one thing, though: the drill has to go deeper than the thread.
How Much Deeper Than the Thread Should You Drill a Blind Hole?
At least the length of the tap's chamfer, plus room for chips. Give the full-thread depth you need on the drawing, and either give a drill depth or leave the shop room to set one.
An r/Machinists thread called "Drill depth for taps" shows the spread. One machinist said that if it's left up to him, he drills 2×D and threads 1.5×D. Another's shop asks engineers for 1.5 to 3 pitches of extra drill depth, so a 1/4-20 with .500" of full thread gets drilled to .600". A third designs the full drill diameter 5 pitches deeper when possible, the figure NASM33537 gives for blind holes that take helical coil inserts. Those are shop habits, not one standard.
Why the chamfer sets the minimum
The first threads on a tap are ground away so it can start, and they only cut partial forms. Yamawa's hand tap guide lists a 9-thread chamfer on a taper tap, 5 on a plug and 1.5 on a bottoming tap. Those are Yamawa's hand-tap figures. Machine taps vary by maker.
Do the math on a 1/4-20 with .50" of full thread. Pitch is .05", so a 5-thread plug chamfer needs about .25" below the last full thread. That puts the full-diameter drill depth around .75". With a bottoming tap you could get away with less, but you'd still want chip room.
Putting tap drill depth on the print
A complete blind-hole callout looks like "1/4-20 UNC-2B ↓ .50, .201 DRILL ↓ .75". The drill depth is measured to full diameter. The drill point goes past it, so leave material under the point. If the hole mustn't break through, add a note.
Don't ask for more thread than the joint needs, either. Extra depth costs cycle time and gives a blind-hole tap more chances to bottom out. The same partial-thread problem shows up at shoulders, which is what thread relief deals with.
Titanium raises the stakes. See how deep you can safely tap a blind hole in titanium and tap drill percentage for titanium vs mild steel.
Sending it to DigiForge
Put the full-thread depth on every blind hole, and the drill depth if you care about it. Our CNC capability page says the quote checks hole diameter and depth-to-diameter ratio automatically, and every quote is reviewed by an engineer. If you only give a thread depth and want to know what drill depth we'd use, ask us when you quote.
Need a part made?
Upload your file for an instant price.