Why threads deserve their own design pass
Threaded holes look simple on a model, yet they cause a large share of questions during quoting. Depth, thread class, tap drill size and the way the hole ends at the bottom all affect cost, strength and whether the part can be made at all. This guide works through those choices in the order a designer usually meets them.
Step 1: pick the thread standard and size
Most machined parts use ISO metric coarse threads, such as M3, M4, M5, M6 and M8, or Unified threads in inch-based designs, such as 4-40, 6-32, 8-32, 10-32 and 1/4-20. Stick with common sizes. Standard taps and gauges are always on hand, while odd sizes or fine pitches may need special tools and longer lead time.
Fine-pitch threads, for example M8 x 1 instead of M8 x 1.25, have their place: thin walls, fine adjustment or vibration resistance. In most cases coarse threads are faster to cut, more tolerant of soft materials and less likely to cross-thread.
Step 2: decide how deep the thread must be
Thread strength comes from engagement length, but after a point extra depth adds nothing. A practical rule:
| Material of the threaded part | Typical useful engagement |
|---|---|
| Steel and stainless steel | ~1 to 1.5 × nominal diameter |
| Aluminum alloys | ~1.5 to 2 × nominal diameter |
| Brass and bronze | ~1.5 × nominal diameter |
| Plastics | ~2 × nominal diameter, or use an insert |
With engagement of about 1.5 diameters in steel, the bolt typically breaks before the thread strips, which is the preferred failure mode. Deeper threads take longer to cut, increase the risk of tap breakage and rarely help. A thread depth of 3 diameters is a warning sign that should be reviewed.
Step 3: design the bottom of a blind hole
In a blind hole the tap cannot cut full thread all the way to the bottom. Standard taps have a tapered lead of a few threads, and the drilled hole must be deeper than the full thread so chips and the tap end have space.
Thread depth versus drill depth
Call out the full thread depth you need and let the drill go deeper. A common allowance is roughly 3 to 5 thread pitches beyond the full thread, depending on tap type. If drawing space allows, show both depths.
Drill point
Drilled holes end in a cone, typically 118° or 135°. Do not dimension the hole depth to the tip of the cone; dimension the full-diameter depth.
Flat-bottom holes
If a flat bottom is truly needed, say so. It needs an extra operation and limits how close the thread can run to the bottom.
Step 4: tap drill and thread percentage
The tap drill determines how much of the thread form is cut. Full 100% thread is hard to tap and barely stronger than about 75%. Shops normally choose drill sizes that give about 65–75% thread in metals, which balances strength with tap life. You usually do not need to specify the tap drill; specify the thread and class, and the shop selects the drill.
Step 5: thread class and fit
For metric threads, 6H for internal threads and 6g for external threads are the normal medium-fit classes. For Unified threads, 2B and 2A are the common classes. Tighter classes, such as 4H or 3B, need special gauges and more inspection effort. Use them only where function demands it.
Threads are normally inspected with go and no-go plug gauges. The go gauge must enter the full length; the no-go must not enter more than a small amount. If threads must be gauged after coating, say so.
Step 6: think about cutting method
Cut tapping
The classic method. Produces chips and works in almost any material.
Form tapping
Displaces material instead of cutting it, creating a stronger thread with no chips, but only in ductile materials such as aluminum and mild steel. Requires a slightly larger pilot hole.
Thread milling
A rotating cutter follows a helical path. Excellent for large threads, hard materials, threads close to the bottom of a blind hole and expensive parts where a broken tap would scrap the part. It also allows the thread size to be adjusted precisely. You can leave the method to the shop in most cases. Point out when a thread must run very close to the bottom of a hole, because that may require thread milling.
Step 7: protect threads in soft materials
Threads in aluminum and plastics wear and strip with repeated assembly. Inserts solve this.
- Helical coil inserts give strong, wear-resistant steel threads in aluminum
- Key-locking inserts handle high loads and are easy to replace
- Heat-set or press-in inserts suit plastics
- Self-tapping inserts work well in softer metals and some plastics
When using inserts, the drawing should call out the insert part number and the final thread size, because the tapped hole is larger than the final thread.
Edge distance and wall thickness
Keep enough material around threaded holes. Threads too close to an edge can bulge or crack the wall during tapping or tightening. A common guideline is to keep the hole center at least about one diameter from the edge, and more in plastics or thin sections. Similarly, leave enough material below a blind hole so the drill point does not break through or leave a very thin floor.
Countersinks and entry chamfers
A small chamfer or countersink at the hole entry protects the first thread from damage, prevents raised burrs and helps the screw start. Many shops add one by default; if the surface is a sealing face or must remain sharp, say so.
Through holes versus blind holes
Through holes are easier to tap because chips can exit and taps can run through. Where the design allows, use through holes. If a blind hole is needed, keep it shallow and leave chip space.
Threads and finishing
Coatings change thread fit. Anodizing, plating and powder coating all add material on the thread flanks. For coated parts, mask threads, cut them oversize for the coating or chase them after finishing. Stating which approach you expect avoids gauge failures at final inspection.
Common thread problems and their causes
Broken taps
Usually caused by threads that are too deep, blind holes without chip room, or very small taps in hard materials. Removing a broken tap can scrap the part, which is why shops prefer thread milling on valuable parts.
Stripped threads in service
Often the result of too little engagement in soft material or repeated assembly. Inserts or longer engagement fix this.
Gauge failures after finishing
Coating built up on the flanks. Plan masking or allowance from the start.
Misaligned fasteners
Threads not perpendicular to the mating face, often in angled or curved surfaces. Add a flat spot face so the tap and the screw head sit square.
A clear thread callout
A good callout lists size, pitch where not coarse, class, depth and any special requirement:
- M6x1.0-6H, thread depth 12, drill depth 16
- 1/4-20 UNC-2B, thread depth 0.50
- M4-6H through, mask before anodize
- Install helical insert, M5x0.8, length 1.5D
Avoid "tap through" notes on blind holes, and avoid "full thread to bottom" unless you truly need it and accept the extra cost.
Checklist before you upload
- Common thread sizes and coarse pitch used where possible
- Thread depth around 1.5 to 2 diameters, not more without reason
- Drill depth deeper than thread depth on blind holes
- Enough edge distance and floor thickness
- Inserts specified for soft materials or frequent assembly
- Coating effects on threads addressed
- Thread class stated if tighter than standard
Threads modeled as cosmetic threads in CAD are fine, but the drawing or quote notes should list the thread specification, because some exported files lose that information.