Process & DFM
Tapped Holes: Design, Callouts and Quoting
The short answer
A tapped hole is a drilled hole with an internal thread cut or formed into it. To quote one correctly a shop needs five things: the thread size and pitch, the fit class, whether the hole is blind or through, the full thread depth, and how many there are. A STEP file usually carries the drilled hole but not the thread, so those details have to come from a drawing or a note. In an OpenSpindle RFQ, tick Threads / Tapped Holes under Advanced options, enter the count, and put each size and depth in the part note or on an attached drawing.
What a tapped hole is
A tapped hole starts as a plain drilled hole, the tap drill, sized slightly larger than the minor diameter of the thread you want. A tool then puts the thread into the wall of that hole. The screw goes straight into the part, with no nut on the other side.
That is the whole appeal. A tapped hole saves a fastener, saves assembly access to the back of the joint, and lets a part be taken apart and put back together. It is why nearly every machined housing, bracket and plate has them.
There are two basic kinds. A through hole is threaded all the way through the material, and the tap can pass out the far side. A blind hole stops inside the part, which means the thread has to stop too, and that is where most of the cost and most of the drawing mistakes live.
Tapped holes are not the only way to put a thread in a part. In soft or thin material, a helical coil insert, a press-in or clinch nut, or a heat-set insert in plastic will often hold better and survive more assembly cycles than threads in the parent material.
Three ways a shop makes the thread
You rarely need to specify the method, but it helps to know what the shop is choosing between, because each one changes the tap drill size, what happens at the bottom of a blind hole, and which materials are a problem.
| Method | How it works | Good at | Limits |
|---|---|---|---|
| Cut tapping | A fluted tap cuts the thread and makes chips | The default for most sizes and materials, fast on a CNC | Chips can pack a blind hole, small taps break in tough alloys |
| Form (roll) tapping | A fluteless tap displaces metal into the thread shape | No chips, a work hardened thread that is often stronger, aluminum and other ductile metals | Needs a larger tap drill, not suited to brittle material such as cast iron, higher torque |
| Thread milling | A rotating cutter follows a helical path around the hole | Hard materials, large diameters, threads close to the bottom of a blind hole, one tool for many diameters of the same pitch | Slower cycle on small holes, the smallest sizes need very fragile cutters |
How deep a thread needs to be
Past a certain depth, more thread adds cost and almost no strength. Most of the load in a threaded joint is carried by the first few engaged threads, so the question is how much engagement the material needs before the screw breaks rather than the thread stripping.
The usual rules of thumb express engagement as a multiple of the nominal diameter, D. They are starting points for a design review, not a substitute for calculating a critical joint.
For most joints there is little benefit in going beyond about 3 x D of full thread. If a part needs more holding power than that, a larger or finer thread, a through hole with a nut, or a thread insert is usually the better fix.
| Material being tapped | Typical minimum engagement | Notes |
|---|---|---|
| Steel, stainless steel, titanium | 1 x D | Parent material is roughly as strong as the screw |
| Aluminum, brass, bronze | 1.5 x D | Consider an insert for parts assembled many times |
| Cast iron, zinc and magnesium castings | 1.5 to 2 x D | Check porosity at the hole location on castings |
| Rigid plastics | 2 x D or more | Heat-set or press-in inserts usually outperform threads cut in plastic |
Blind holes: thread depth is not hole depth
A tap does not cut a full thread all the way to its tip. Its leading end is chamfered so it can start in the hole, and the threads along that chamfer are incomplete. A plug tap, the common default, has roughly three to five incomplete threads at its end. A bottoming tap has one to two. On top of that, the drill leaves a conical point below its full diameter.
So a blind tapped hole has three depths, and a drawing should be clear about which one it means. The drill depth is the deepest. Above it are the incomplete threads. Above those is the full thread depth, which is the only one that holds a screw.
If your design calls for 12 mm of full thread in a pocket that is only 13 mm deep, the shop has to use a bottoming tap or a thread mill, take more care with chips, and accept more risk of a broken tap in the part. That costs time on every hole. Leaving a few pitches of extra drill depth below the full thread, where the part allows it, is one of the cheapest changes you can make.
Watch the far side as well. A blind hole drilled close to an opposite face or an internal pocket can break through, and a thread near an edge can bulge or crack the wall. Keep at least about one diameter of material around a tapped hole where you can.
How to call out a tapped hole on a drawing
A complete callout gives the thread, the fit class, and the depth of full thread. For blind holes, add the tap drill diameter and its depth. For through holes, THRU replaces the depths. The symbol that looks like a small downward triangle is the depth symbol, and a plain DEEP in text works just as well.
State the full thread depth, not the depth you want the tap to go. If you only give the hole depth, the shop has to guess how much of it must be full thread.
When the same thread appears several times, a count prefix such as 4X saves repeating the callout. For how to read each field of the thread designation, see the thread callout guide. For the drill size under each thread, see the tap drill chart.
| Callout | What it tells the shop |
|---|---|
| 4X 1/4-20 UNC-2B THRU | Four inch coarse threads, class 2 fit, through the part |
| 2X 1/4-20 UNC-2B, 0.50 DEEP, 0.201 DRILL 0.62 DEEP | Blind: half an inch of full thread, #7 drill a further eighth of an inch below it |
| 6X M6x1-6H THRU | Six metric coarse threads, general purpose fit, through the part |
| M6x1-6H, 12 DEEP, 5.0 DRILL 15 DEEP | Blind: 12 mm of full thread over a 15 mm deep 5 mm drill |
| M4x0.7-6H, 8 DEEP, FORM TAP | Use only when the method matters, for example to avoid chips in a sealed part |
What makes tapped holes expensive
Most tapped holes add very little to a quote. A handful of details push the price up, and nearly all of them are decisions made in CAD.
| Detail | Why it costs more | Cheaper alternative, where it works |
|---|---|---|
| Very small threads in tough material | Taps below about #4 or M3 break easily in stainless and titanium, and a broken tap can scrap the part | Move up a size, or use a thread insert |
| Full thread to the bottom of a blind hole | Needs a bottoming tap or thread milling, and more chip management | Leave extra drill depth below the thread |
| Deep threads, beyond about 3 x D | Longer cycle and more breakage risk for little strength gain | Shorten the thread or change the joint design |
| Many different thread sizes on one part | Every size is another tool change and another tap in the setup | Standardize on one or two sizes |
| Holes on angled or curved faces | May need an extra setup or a 4 or 5 axis machine | Add a flat spot face square to the hole |
| Uncommon pitches or special fit classes | The tap may be a special order with its own lead time | Use UNC, UNF or metric coarse with a 2B or 6H fit |
| Threads in parts that get plated or anodized | Coating builds up on the thread flanks and can stop a gauge from entering | Mask the threads, tap oversize, or chase the threads after finishing |
Model the tap drill, not the thread
Most CAD programs show a thread as a cosmetic feature: the model contains a plain hole and the thread is a note or a texture laid over it. When you export a STEP file, that information is usually lost. What the shop receives is a round hole of some diameter and nothing to say it should be threaded.
Two habits prevent most problems. First, model the hole at the tap drill diameter, not the thread major diameter, so the geometry the shop measures matches what they will drill. A hole modeled at 6 mm could be an M6 thread or a 6 mm clearance hole, and neither the software nor the shop can tell which. Second, never rely on the model alone to communicate a thread. Put it on a drawing, or in a note that names every threaded hole.
If you design in a tool with a hole wizard, it is worth checking that its thread specifications match the depths you want, because many default to a full thread depth that is deeper than the joint needs.
Adding tapped holes to your OpenSpindle RFQ
The quote form has a dedicated place for threads, and using it changes what comes back. Shops generally price tapping by the hole, and a thread they cannot see is either missing from the quote or added later as a change.
For each part that has threads:
Step 1: Upload the model. Add the 3D model as usual, with threaded holes modeled at the tap drill diameter.
Step 2: Tick Threads / Tapped Holes. Open Advanced options on the part and find it under Secondary operations. Enter the total count of tapped holes on that part, counting every hole rather than every size.
Step 3: Write the details in the Note. In the part Note, list each thread size with its count, whether it is blind or through, and the full thread depth for blind holes. If a thread fit class other than 2B or 6H matters, say so here.
Step 4: Attach a drawing. Under Reference Files & Technical Drawings, attach the drawing if you have one. A PDF with callouts is best. A screenshot of the model with the threaded holes circled and labeled works well when you have no drawing yet.
Step 5: Flag any inserts. If any holes should get a helical insert, clinch nut or other hardware instead of a cut thread, tick Inserts as well and name the part number and location of each.
If no depth is given, the default is to drill to the depth in your CAD model and thread it using standard shop practice and tooling. That is a reasonable result for through holes and a gamble for blind ones, which is why the depth is the single most useful thing to write down.
| What to include | Example note | Why it matters to the quote |
|---|---|---|
| Thread size and pitch | M6x1, 1/4-20 UNC | Sets the tap, the drill and the risk of breakage |
| Count per size | 4X M6x1, 2X M4x0.7 | Tapping is priced per hole and per tool |
| Blind or through | 4X M6x1 THRU | Blind holes take more care and sometimes a second tool |
| Full thread depth (blind) | 2X M4x0.7, 8 DEEP | Decides whether a standard plug tap will reach |
| Fit class, if not standard | 3B, or 4H5H | Tighter classes can need special taps and gauging |
| Finish after tapping | Mask threads during anodize | Avoids threads that no longer accept a screw |
| Inserts instead of threads | 4X helical insert M5, stainless, 1.5D | Adds hardware, an install step and a larger drilled hole |
A complete example
Here is the kind of note that lets a shop quote tapped holes without a single follow-up question. It covers an aluminum enclosure lid with mounting holes and a sensor bracket:
6X M4x0.7-6H THRU for the lid screws. 4X M3x0.5-6H, 6 DEEP full thread, blind, on the underside bosses, at least 1 mm of extra drill depth where the boss allows. 2X 1/4-20 UNC-2B THRU for the tripod mount. Mask all threads during anodize. Drawing attached, threaded holes circled on page 2.
With that, Threads / Tapped Holes ticked, and a count of 12, a shop in the network can price every hole the first time. If you are not sure what depth or size a hole should be, write that in the note instead. A shop can recommend a size and depth for the load you describe, which is a better outcome than a quote built on a guess.