How do you write a blind tapped hole thread depth callout?

What belongs in a blind tapped hole callout?

A complete callout gives the number of holes, the thread designation with its class, and the depth of usable thread. Everything else, including the drill, is optional and should appear only when it controls something the thread designation does not.

Read left to right, a typical inch note looks like this: 4X 1/4-20 UNC-2B ↧ .50. The count (4X) is the number of holes; the designation gives size, threads per inch, series and class, with B marking an internal thread. The depth symbol, the downward arrow defined in ASME Y14.5, replaces the older word DEEP, and the value after it is the thread depth. The metric equivalent follows the same order: 4X M6x1-6H ↧ 12, where 6H is the tolerance class of the internal thread and the depth is in millimeters because the drawing is.

ASME Y14.6 sets how threads are represented, specified and dimensioned on drawings, but not the thread sizes themselves, which come from the thread standards. The drawing standard says where information goes; the thread standard says what the class means.

Two items are easy to leave off and expensive to guess: the class, which a supplier will otherwise default, and the depth. A note that gives the thread without a depth lets the machinist choose how far to go, and that choice will suit the tool, not the screw.

Should the drawing specify the tap drill size and drill depth?

Usually not the drill size, and only sometimes the drill depth. The thread class already fixes the minor diameter limits, so naming a drill repeats that requirement in a less precise form and turns a product requirement into a process instruction.

The minor diameter tolerance is the real requirement, and any drill, reamer or core that lands inside it is acceptable. The handbook tabulates probable hole sizes precisely because drills normally cut oversize, so naming a drill locks the shop into one route without guaranteeing the class.

Drill depth is different. It deserves a dimension when the bottom of the hole controls something: the remaining wall above a sealed cavity or a cooling channel, a hole close to a mating face, or a thin cast section where breakthrough would scrap the part. In those cases, give a maximum drill depth or a minimum wall, as its own dimension, and leave the thread depth as a minimum usable length. That pair tells the machinist exactly how much room there is for the tap to finish.

The handbook also shifts the recommended hole size with engagement length, so a drill picked from a chart can be wrong for a very short or very long thread. The table summarizes those rules.

For a sense of scale, the same appendix gives the class 2B minor diameter of a 1/4-20 UNC thread as 0.196 to 0.207 in, and lists a #7 drill that is expected to cut about 0.2048 in, roughly 70 percent of basic thread height (NBS Handbook H28, Table A3.1). The drawing needs only the class; the drill is how the shop meets it.

How much deeper than the thread does the drilled hole need to be?

The drilled hole has to be longer than the full thread by the length of the tap's chamfer plus the drill point, with some room for chips if the tap cuts. The exact margin depends on the tap style, so it is better controlled by a maximum drill depth or minimum wall than by a fixed rule on the drawing.

The tap chamfer is the first allowance: in typical shop usage a bottoming tap has a chamfer of about one to two threads and a plug tap three to five, and those threads become the vanish thread the handbook excludes from useful thread. The drill point is the second: a common 118-degree point leaves a cone about three tenths of the drill diameter deep, which is plain geometry.

A cutting tap also needs room for chips; a forming tap does not, but starts from a larger pilot. Either way, a minimum full-thread depth plus a maximum drill depth lets the shop pick the tap and gives the inspector two numbers to check.

If there is no space, give a maximum drill depth and let the supplier propose a bottoming tap or thread milling, which can bring full thread closer to the bottom than a tap and is routine on CNC milling centers.

How do you call out a tapped hole in a cored die-cast hole?

Dimension the cored hole as a cast feature with its draft, then give the thread callout as a separate machined requirement. The casting rules decide how deep and how tapered the core can be, and the thread note decides how much full thread must exist after machining.

Coring the pilot saves a drilling step, but the core pin has draft, so the hole is larger at the entry than at the bottom. The zinc die-casting design rules published by the International Zinc Association suggest coring a hole that will be tapped without a full thread so that it allows about 60 percent of a full thread at the larger end and about 75 percent at the other; if a full thread is essential, they recommend machining out the taper before tapping, and they advise that threaded depth should not exceed twice the nominal screw diameter (IZA zinc die casting design rules). The same rules call for tap and chip clearance beyond the last thread, or a through hole, and a countersink at the entry for easier tapping and assembly.

On the drawing that becomes two notes: the cored hole with its draft, marked as cast, and the thread with its depth plus, if full thread must run through the taper, DRILL OUT CORE BEFORE TAPPING. Aluminum die-casting alloys such as ADC12 and A380 follow the same logic; the ADC12 vs A380 guide covers how their silicon content affects machining, and the die casting page describes how castings from partner foundries are machined at our lead CNC plant.

This is where drawings sent overseas most often go wrong. If the drawing does not say whether the pilot is cored or drilled, a cored pilot with draft can gauge fine at the mouth and loose at the bottom, and with parts cast and machined overseas and assembled in the US or Europe, that surfaces at incoming inspection. Ask the supplier to state in the quote which holes will be cored and how full-thread depth will be checked.