Use a free-machining alloy such as 12L14, 1215, C360 brass or 303 stainless, and set the largest diameter at a standard bar size. Allow a 0.005–0.015 in (0.13–0.38 mm) inside corner radius, keep drilled holes under about 6× diameter, give threads 2 pitches of runout, and expect ±0.001 in (±0.025 mm) on diameters and 0.0005–0.001 in TIR in one chucking.
SSG MFG · design guideDG-08 · 13 rules
13 rules, in the order you meet them on a model. Every value is typical; the principal quoting your part confirms its own limits.
| # | Rule | |
|---|---|---|
| 01 | Use free-machining alloys12L14 or 1215 steel, C360 brass, 303 stainless | 12L14 or 1215 steel, C360 brass, 303 stainless |
| 02 | Design to stock bar sizesLargest OD at a standard round or hex size, such as 0.500 or 0.750 in; 12 ft (3.7 m) bars | Largest OD at a standard round or hex size, such as 0.500 or 0.750 in; 12 ft (3.7 m) bars |
| 03 | Match slenderness to the machineUp to about 3:1 length-to-diameter unsupported; over 10:1 on Swiss-type | Up to about 3:1 length-to-diameter unsupported; over 10:1 on Swiss-type |
| 04 | Allow a tool nose radiusInside corner radius of 0.005–0.015 in (0.13–0.38 mm) | Inside corner radius of 0.005–0.015 in (0.13–0.38 mm) |
| 05 | Limit drilled hole depthAbout 6× diameter standard; 6–12× with peck cycles; beyond that, gun drilling | About 6× diameter standard; 6–12× with peck cycles; beyond that, gun drilling |
| 06 | Keep small drills shortBelow 0.040 in (1 mm) diameter, hold depth to about 3× diameter | Below 0.040 in (1 mm) diameter, hold depth to about 3× diameter |
| 07 | Keep tapped threads shortFull thread about 1.5× diameter; drill 3 pitches deeper than full thread | Full thread about 1.5× diameter; drill 3 pitches deeper than full thread |
| 08 | Provide thread runoutAt least 2 pitches of runout, or a relief groove below the minor diameter about 2–3 pitches wide | At least 2 pitches of runout, or a relief groove below the minor diameter about 2–3 pitches wide |
| 09 | Chamfer edges0.010–0.020 in (0.25–0.5 mm) × 45° | 0.010–0.020 in (0.25–0.5 mm) × 45° |
| 10 | Allow a cutoff nubCenter pip up to about 0.010 in (0.25 mm), or specify a back-faced end | Center pip up to about 0.010 in (0.25 mm), or specify a back-faced end |
| 11 | Keep cross features on the machineCross holes, flats and slots sized for live tools or a cross-drill attachment | Cross holes, flats and slots sized for live tools or a cross-drill attachment |
| 12 | Hold concentric features in one setupExpect 0.0005–0.001 in (0.013–0.025 mm) TIR within one chucking | Expect 0.0005–0.001 in (0.013–0.025 mm) TIR within one chucking |
| 13 | Tolerance only what mattersDefault to ±0.001 in (±0.025 mm) or looser on non-critical diameters | Default to ±0.001 in (±0.025 mm) or looser on non-critical diameters |
These build on the short list on the screw machining process page, with the failure each rule prevents and a drawing for each.
Change a drilled hole's depth and diameter and see where standard drilling gives way to peck drilling and then gun drilling, and what each does to cycle time.
HOLE ⌀0.250 IN · DEPTH 0.75 IN
Works: drills in one pass
3.0× diameter clears chips in one pass with a standard jobber drill.
Typical thresholds: about 4× diameter for a standard drill, peck drilling beyond that, and gun drilling past about 10×.
Each rule with its typical value, the reason behind it and what happens on the floor when it's ignored. Switch any drawing between Do and Avoid; point at a callout to pick it out.
Rule 01
12L14 or 1215 steel, C360 brass, 303 stainless
Standard: ASTM A108, ASTM B16, ASTM A582
Rule 02
Largest OD at a standard round or hex size, such as 0.500 or 0.750 in; 12 ft (3.7 m) bars
Fig. 1Design to bar stock
Do. Set the largest diameter at a standard bar size, such as 0.500 or 0.750 in, and the bar's own surface becomes the part's OD.
Avoid. A largest diameter just over a stock size forces the next bar up; every part turns that difference into chips and cycle time.
Rule 03
Up to about 3:1 length-to-diameter unsupported; over 10:1 on Swiss-type
Rule 04
Inside corner radius of 0.005–0.015 in (0.13–0.38 mm)
Fig. 2Internal corner radius
Do. Corner radius a little larger than the cutter radius lets the end mill arc through the corner at full feed.
Avoid. A sharp inside corner can't be milled: a rotating tool always leaves its radius, so a square corner means EDM or a broach, at several times the cost.
Rule 05
About 6× diameter standard; 6–12× with peck cycles; beyond that, gun drilling
Fig. 3Drilled hole depth
Do. A blind hole about 4× its diameter deep drills in one pass; call the full-diameter depth and let the 118° point sit below it.
Avoid. Deep holes pack chips and let the drill wander off the axis; past about 6× you're into peck cycles, and past about 10× gun drilling.
Rule 06
Below 0.040 in (1 mm) diameter, hold depth to about 3× diameter
Rule 07
Full thread about 1.5× diameter; drill 3 pitches deeper than full thread
Standard: ASME B1.1, ISO 965
Fig. 4Tapped hole depth
Do. About 1.5× D of full thread carries the bolt to failure in steel; the tap drill runs a few pitches deeper so a plug tap never bottoms out.
Avoid. Thread past 1.5–2× D adds almost no strength, and a tap that bottoms in a blind hole packed with chips breaks off in the part.
Rule 08
At least 2 pitches of runout, or a relief groove below the minor diameter about 2–3 pitches wide
Fig. 5Thread runout and relief
Do. A relief groove at least two pitches wide, cut to the minor diameter, gives the threading tool room to exit and the nut a full thread to seat against.
Avoid. Without relief the last threads are incomplete: the nut stops short of the shoulder and the tool can crash into it.
Rule 09
0.010–0.020 in (0.25–0.5 mm) × 45°
Fig. 6Edge break
Do. A small 45° chamfer on every outside edge removes the burr, guides assembly and costs almost nothing when it's in the program.
Avoid. A sharp edge keeps its burr: it cuts hands and seals, and stops mating parts from starting straight.
Rule 10
Center pip up to about 0.010 in (0.25 mm), or specify a back-faced end
Rule 11
Cross holes, flats and slots sized for live tools or a cross-drill attachment
Rule 12
Expect 0.0005–0.001 in (0.013–0.025 mm) TIR within one chucking
Fig. 7Setups
Do. Features grouped on one or two faces machine in one or two setups, with every feature referenced to the same datum.
Avoid. Each extra face is another fixture, another setup charge and another chance for position error between features.
Rule 13
Default to ±0.001 in (±0.025 mm) or looser on non-critical diameters
Standard: ASME Y14.5, ISO 286
Typical values for production screw machines. Tight values rely on Swiss machines with in-process gauging, reaming, burnishing or centerless grinding.
| Feature | Typical | Tight | Cost of tight |
|---|---|---|---|
| Turned diameter | ±0.001 in (±0.025 mm) | ±0.0002–0.0005 in (±0.005–0.013 mm) | Moderate |
| Length and shoulder location | ±0.002–0.005 in (±0.05–0.13 mm) | ±0.001 in (±0.025 mm) | Moderate |
| Drilled hole diameterTight holes are reamed | ±0.002 in (±0.05 mm) | +0.0005/−0 in (+0.013/−0 mm) | Moderate |
| Concentricity, one chucking | 0.001 in (0.025 mm) TIR | 0.0005 in (0.013 mm) TIR | Moderate |
| Thread class | 2A/2B or 6g/6H | 3A/3B or 4h/4H5H | Moderate |
| Surface finishRoller burnishing or grinding | Ra 32–63 µin (0.8–1.6 µm) | Ra 16 µin (0.4 µm) or better | Moderate |
| Chamfer size | ±0.005 in (±0.13 mm) | ±0.002 in (±0.05 mm) | Low |
Basis: ASME Y14.5, ISO 286, ASME B1.1. Put a general tolerance note on the drawing and tighten only the features that need it; every tight callout is priced. See the tolerance guide.
The same screw machining rules shift with the alloy or compound.
The fastest-cutting steel for screw machines. Lead content makes some customers ban it, so 1215 is the usual lead-free substitute, and neither is a good choice for case hardening or welding.
Drills, taps and knurls faster than any steel and gives short, clean chips. Specify a lead-free brass for potable-water parts that must meet lead limits.
The free-machining stainless, with added sulfur. It machines well but resists corrosion and welds less well than 304 or 316, so reserve those for parts that need it.
Gummy and work hardening, so cycles run slower and deep small holes are risky. Keep drilled depth nearer 4× diameter and allow larger radii.
Cut annealed or prehardened to about 28–32 HRC. Parts hardened after turning grow and distort, so leave grind stock on critical diameters.
Common on Swiss machines for medical pins and screws. Expect slow speeds, short tool life and a piece price several times that of stainless.
Run these against the model before it goes out for quote. The builder's DFM check catches most of them on an uploaded part.
0 of 12 checked
Standard drilling handles about 6× the drill diameter in one plunge. Peck cycles reach roughly 12× by retracting to clear chips, at the cost of cycle time. Deeper holes need gun drilling or coolant-through drills. Small drills under 0.040 in (1 mm) are best kept near 3× diameter because they break easily at screw machine feed rates.
A thread relief, or undercut, is a groove turned just below the thread's minor diameter at a shoulder, typically 2–3 pitches wide. It gives the threading tool or die room to exit, so full threads run right up to the shoulder and a nut or mating part can seat flat. Without it, allow at least 2 pitches of incomplete thread.
Peck drilling is a cycle where the drill feeds a short distance, retracts to clear chips, then feeds again. It lets a standard drill reach about 6–12× its diameter without packing chips in the flutes. Each retract adds time, so a deep pecked hole can become the slowest station on a screw machine.
The part breaks free from the bar just before the cutoff tool reaches center, leaving a small pip, often up to about 0.010 in (0.25 mm). If the end must be flat, call for a back-faced end so the shop adds a pickoff spindle or second operation. Leave the pip where it does not affect function.
12L14 cuts fastest and is the default for steel pins, fittings and spacers. 1215 is the common lead-free alternative. Use 1018 or 1045 when the part must be welded or case hardened, and 4140 when it must be through hardened for strength. Each step away from free-machining grades adds cycle time.
Features cut in one chucking commonly hold 0.0005–0.001 in (0.013–0.025 mm) TIR, because the guide bushing supports the bar at every cut. Moving the part to a second operation usually loosens that to 0.002 in or more. Put every concentric diameter, bore and thread on the same end or on the sub-spindle in one cycle.
Check your part against these rules.
Drop a STEP file in the builder for an instant DFM check and a budgetary estimate, then send it to principals who run screw machining every day.
