CNC Machining DFM
CNC Machining DFM: The Part That Quotes in Hours, Not Weeks
A 30 mm deep pocket with R2 corners forces a 4 mm end mill that deflects 16 times more than the tool the job needs, and a drawing with ±0.01 mm on every dimension costs eight times the same part at ±0.5 mm. Eight design rules, each with a number, and a machined sensor hub worked from $1,370 a part to $430.
The quote came back at double the budget, and the lead time was three weeks instead of one. The part looked simple on screen: a small aluminium lid, a pocket for a sensor, four tapped holes, a thin flange. The shop's reply was polite and specific, the pocket needed a smaller tool than the job wanted, the flange would chatter, six of the twenty-eight dimensions needed a second operation, and the part had to be flipped six times.
Every one of those problems was decided in the CAD file, weeks before the quote was requested. None of them was a machining problem. They were all design problems, and they were all fixable with a number.
That is what this article is: eight rules, each with a number you can design against, and one part worked all the way through, as drawn, and as fixed, so you can see what each rule is worth in money.
What CNC machining actually is, and the one fact behind every rule
CNC machining is cutting a part out of a solid block by moving a spinning cutter through it under computer control. A mill cuts with a rotating tool that moves across the part; a lathe spins the part against a fixed tool. Most machined parts in this article's world are milled.
DFM, design for manufacturing, or design for manufacturability, is the discipline of drawing parts the process can actually make, at a price the project can afford. The moulding version of the same discipline is Article #16: there, the rules are about filling, cooling, and ejecting. Here, the rules are about cutting, and they all come from one fact.
The tools are round, and they flex.
Every cutting tool in a mill is a rotating cylinder. It cannot cut a sharp square inside corner, because a round tool leaves a round corner, the smallest inside corner it can leave is its own radius. And a long, thin tool bends under cutting force, the way a long ruler bends when you push its end.
A short, fat tool is stiff. A long, thin tool is a spring. Every rule in this article is one of those two facts, applied to a different feature: corners, pockets, walls, holes, threads, tolerances, setups, materials.
A setup is one clamping of the part on the machine: the part is fixed in a fixture, the machine is told where the part is (the datum, the reference point everything is measured from), and the program runs. A three-axis machine can only cut from one direction per setup, so every face that needs cutting from a different direction means stopping the machine, unclamping the part, building or adjusting a fixture, re-establishing the datum, loading a new program, and proving out the first piece.
A tolerance is how far a part is allowed to be off its perfect size, the same idea as Article #8, where ten parts at ±0.1 mm stack to ±1.00 mm worst case. The machined part's tolerances are what that stack-up consumes.
Eight machining rules, all from one fact: round tools that flex
| Feature | Rule |
|---|---|
| Corners | Radius at least depth ÷ 3 (a 30 mm pocket needs R10) |
| Pockets | Depth ÷ width up to 3:1; above 4:1 needs extended-reach tooling |
| Walls | Height ÷ thickness up to 4:1; past 10:1 the wall chatters |
| Holes | Depth ÷ diameter up to 4:1; deeper means peck or gun drilling |
| Threads | 1.5× diameter in steel, 2× in aluminium, then stop |
| Tolerances | ±0.5 mm costs 1.0×; ±0.01 mm 8.0×; ±0.005 mm 15.0× |
| Setups | About $150 a batch each, plus 0.02 to 0.05 mm of datum error |
| Material | 6061 machines at 80%; 316L at 40% |
Rule 1
A rotating tool cannot cut a sharp square corner on an inside edge, so every inside corner needs a radius, and the radius you specify decides the tool, and the tool decides the price.
The rule, from FabCon's design guide and confirmed by Hubs, MakerStage, and two other checked guides: make the internal corner radius at least one-third of the pocket depth. A 30 mm deep pocket needs corner radii of at least 10 mm. A 15 mm deep pocket needs at least 5 mm.
The reason is the tool's length-to-diameter ratio: a cutting tool should not extend further than about three times its diameter (3:1) without severe deflection, so the corner radius you specify dictates the tool diameter, which in turn limits how deep that corner can be machined economically.
Smaller radii force smaller end mills, and smaller end mills are where the money goes. When an end mill is driven into a tight corner, the tool engagement angle suddenly increases, the tool is cutting on multiple sides at once, which drastically increases cutting force. The tool bends (deflection), the bend becomes vibration (chatter), chatter destroys the surface finish, accelerates tool wear, and frequently snaps the tool. To survive, the machinist slows the feed rate to a crawl when approaching tight corners, and the cycle time, and the quote, climbs.
The physics is brutal and exact. Tool deflection grows with the cube of the length and inversely with the fourth power of the diameter. Double the tool diameter at the same length and the deflection falls by a factor of sixteen.
The checked deflection table (Dazao) makes the same point as a ratio against a 3:1 length-to-diameter baseline: at 4:1 the tool deflects 2.37 times more, at 5:1 it is 4.63 times, at 6:1 it is 8 times, at 8:1 it is 18.96 times, and at 10:1 it is 37 times. A corner that forces an 8:1 tool is a corner that costs nineteen times the deflection of the standard.
Two refinements the guides agree on. First, specify a radius slightly larger than the tool radius, about 130% of the tool radius, or the tool radius plus a small clearance (a 5.0 mm radius specified as 5.2 or 5.5 mm). A radius exactly equal to the tool radius forces the cutter to wrap the entire corner at full engagement, which spikes cutting force and invites chatter.
Second, standardise the radii across the part to standard cutter sizes (3, 4, 6, 8, 10, 12 mm), so one tool cuts every corner instead of a tool change per corner. FabCon's worked example: increasing internal pocket fillets from R2 to R4 mm can double the allowable tool size and quadruple the material removal rate.
If the mating part genuinely needs a sharp corner, a square block that must sit into the pocket, do not specify a sharp internal corner. Use a dogbone fillet (the corner extended in two directions so the square part clears) or a T-bone fillet (extended in one direction), or accept the radius and put the clearance on the mating part. And if the corner genuinely must be sharp, the escape hatch is a different process: EDM (electrical discharge machining) erodes material with an electrode instead of a rotating tool, so it is not bound by any cutter radius, and it is priced like a different process, because it is one.
Rule 2: Pockets: depth-to-width 3:1 or less
A pocket is cut by plunging an end mill and clearing material out. The deeper it goes, the longer the tool, and length is where the trouble starts, the same deflection law as Rule 1, applied to the whole cavity.
The rule: keep pocket depth-to-width ratios at 3:1 or less. Above 4:1, extended-reach tools are required, feed rates drop, and chatter risk climbs (FabCon). MakerStage's table: standard end mills reach 3:1 depth-to-width; extended-reach tools achieve up to 6:1 at higher cost, 30–50% longer cycle times and a rougher surface finish (typically Ra 1.6–3.2 μm against Ra 0.8–1.6 μm standard).
Sekkei Tech: pocket depth should not exceed three times the end mill diameter for good results; four times is achievable with reduced feed rates; beyond five times requires special tooling and extended cycle times. Dazao's extreme band: pockets up to 8–10 times the tool diameter are possible, but only with damped or five-axis tooling, at roughly nineteen times the deflection of the standard, the process has shifted from standard machining to specialised, high-cost manufacturing.
Ra is the average roughness of a surface, in micrometres, the smaller the number, the smoother the surface. A finish of Ra 0.8–1.6 μm is a clean machined face. Ra 1.6–3.2 μm is visibly rougher and is what a long tool leaves behind when it vibrates.
When a pocket is too deep for its width, the fixes are geometric, not heroic. Relieve the geometry (widen the pocket where nothing mates). Open the pocket to a part edge so the tool can enter from the side. Split the feature so a larger tool reaches the floor. Machine from both sides. Or redesign the part as an assembly, two shallow parts bolted together instead of one deep pocket. Every one of those is a CAD edit. None of them is a shop-floor rescue.
Rule 3: Walls: thin is a cantilever, and cantilevers vibrate
A thin wall in a machined part is a cantilever beam, a plate fixed at its base and free at its top. Cutting force pushes it, it bends away from the cutter and springs back, and the cutter never meets a consistent surface. The result is chatter marks, waviness, dimensions that shift as the wall moves, and, past a point, a wall that cracks or warps as internal stress releases after machining.
The floors, from FabCon: the absolute minimum machined wall thickness is approximately 0.8 mm for metal and 1.5 mm for plastic. The practical minimums, the numbers you can actually quote from, run higher: 1.0 mm aluminium, 1.5 mm steel, 1.5 mm titanium, 2.0 mm plastics. (The pipeline for this article listed 2.5 mm for titanium; the checked guides put the practical minimum at 1.5 mm, MakerStage and Sinbo both, with 0.8–1.0 mm achievable. The article uses 1.5 mm, and the correction is recorded below.)
But thickness alone does not decide whether a wall holds. The controlling parameter is the height-to-thickness ratio, how tall the wall is compared to how thick it is. A 1 mm wall that is 3 mm tall is fine.
The same wall 30 mm tall is a tuning fork. The design rule from MakerStage: keep the height-to-thickness ratio at or below 4:1 for unsupported walls. FabCon's chatter line is higher: walls taller than 10× their thickness will chatter, which requires slower feeds or a redesign.
And MakerStage's practical limit: walls taller than 15× their thickness are not practical for standard CNC, consider sheet metal or a fabricated assembly instead. Sinbo caps the unsupported height at 8× the wall thickness in aluminium and 5× in steel. The article's working rule is the strictest of the set, design to 4:1, expect chatter past 10:1, do not attempt 15:1, because the strictest rule is the one that keeps the part in tolerance.
Two more facts from the checked guides. First, the minimums assume short walls: XTJ notes they assume walls shorter than about 25 mm, and for every doubling of wall height beyond that, expect to increase the minimum thickness by roughly 30–50% to maintain dimensional control. Second, thin walls fail for three connected reasons, deflection under cutting force, vibration (chatter), and distortion from residual stress, and the fixes are the same in all three cases: add temporary support ribs connecting the thin wall to the workpiece body and machine them away in the final pass, reduce the depth of cut per pass to under one times the wall thickness, and take light finishing passes instead of one heavy one.
A light spring pass on a thin wall is not a luxury. It is the difference between a wall and a spring.
Rule 4
A drilled hole is a blind tunnel, and the problem with a blind tunnel is getting the chips out. A standard twist drill's flutes can handle the chips the cutting lips produce as long as the depth-to-diameter ratio is about 4:1 or less (Kennametal, via Cutting Tool Engineering). Past that, the chips pack into the flutes, the drill rubs instead of cutting, the hole wanders, and the drill breaks.
The working bands, from eMachineShop and the peck-drilling guides: standard drilled holes should stay within roughly 4:1 to 6:1 depth-to-diameter for reliable results without specialised tooling. Beyond roughly 4–6 times the hole diameter in depth, standard twist drills start to wander and struggle with chip evacuation, and deeper holes need peck drilling, drilling a short distance, retracting the drill to clear the chips, and going back in, or gun drilling, a dedicated deep-hole process with through-tool coolant.
The canned cycles have names: G73 (high-speed chip-break, a micro-retract of 0.25–0.50 mm) for holes 2.5×D to 4.0×D deep, and G83 (deep-hole full-retract peck, Q = 0.50×D to 0.75×D) for holes deeper than 4.0×D. Pecking shortens tool life, reduces productivity, and can diminish hole quality, every time the drill comes out and goes back in, there is a chance it will not line up correctly, and the hole comes out larger than specified.
The exceptions are real and bounded. Parabolic-flute drills were engineered to drill holes up to 15 times the drill diameter without pecking in materials under 25–26 HRC (low-carbon steels, aluminium, copper alloys). And the deflection law applies here too: deflection grows with the cube of the overhang length, so a boring bar at 4×D is roughly eight times softer than the same bar at 2×D.
Three details that belong on the drawing, not in the shop's head. First, use standard drill sizes, fractional, number, or letter drills are stocked and fast; a custom diameter close to but not matching a standard size often means a boring operation instead of a simple drill cycle. Second, a drilled hole ends in a point, not a flat floor: a standard 118° drill point leaves a cone about 0.3× the diameter deep past the full-diameter depth, so the drill depth must allow for it.
Third, the tolerance decides the method before the diameter does: ±0.05 mm suits drilling, ±0.02 mm needs boring, ±0.005 mm needs reaming or fine boring, the same ladder as Rule 6, applied to one feature.
Rule 5
A threaded hole is a joint, and a joint's strength is not proportional to its depth. The load in a threaded joint is not carried evenly along the engaged threads, it is concentrated in the first few, with each successive thread carrying less. In a typical 7/8-9 Grade 8 nut, the first engaged thread carries 34% of the load.
The rule, from the checked threading guides: a thread engagement of roughly one diameter approaches full strength in steel, and about 1.5 diameters is safely full. Beyond that, adding depth adds very little to the strength of the joint, and it adds cycle time, tool cost, and the risk of breaking a tap in the hole on every part. The material changes the answer, because the engagement needed depends on the strength of the parent material relative to the bolt: steel around 1 to 1.5× the thread diameter, aluminium around 2×, plastics 2 to 3× or a threaded insert.
(One checked guide puts aluminium at 1.5× with no appreciable gain beyond, the article uses 1.5–2× as the working range, and the correction is recorded below.) Where the joint requires more strength, the productive changes are a larger thread, a stronger fastener, or a longer engagement in a weaker parent material, not simply more depth of the same thread.
Three more numbers for the drawing. The tap drill is chosen so the finished thread is about 75% of full thread depth, tap drill diameter equals the major diameter minus the pitch, because 75–80% engagement gives almost all of the available strength while keeping tapping torque reasonable. The thread depth you call out is the usable, full-form thread; the drill depth is the shop's decision, and the rule of thumb is drill depth ≈ thread depth + half the thread diameter, with the drill-point allowance on top.
And a blind tapped hole needs the fastener to engage enough thread without bottoming out on an incomplete thread, so the thread depth is the engagement plus 2–3 pitches of runout, and the drill depth is the thread depth plus the point.
Rule 6
This is the rule that costs the most money, and it costs it silently, because a tolerance looks free on a drawing. It is not free. It is a cost multiplier, and the multiplier is exponential.
The checked cost table (Sinbo's tolerance-design guide):
| Tolerance band | Relative cost | Typical process |
|---|---|---|
| ±0.5 mm | 1.0× | Standard CNC milling / turning |
| ±0.1 mm | 1.5× | CNC with standard tooling, normal inspection |
| ±0.05 mm | 2.5× | CNC with controlled environment, CMM inspection |
| ±0.025 mm | 4.0× | Precision CNC, grinding, temperature control |
| ±0.01 mm | 8.0× | Jig boring, precision grinding, CMM |
| ±0.005 mm | 15.0× | Lapping, honing, temperature-controlled lab |
Moving from ±0.1 mm to ±0.05 mm increases cost by about 67%. Moving from ±0.05 mm to ±0.01 mm increases cost by 220%. Each halving of tolerance can double or triple the cost, because each step tighter requires a better machine, a more skilled operator, more frequent inspection, and slower cutting parameters, and below ±0.025 mm, environmental control (temperature, vibration) as well.
CMM is a coordinate measuring machine: a precision instrument that touches the part with a probe and measures it to micrometres. Calipers become micrometres become CMMs, and at ±0.005 mm the inspection is 100% CMM in a temperature-controlled lab.
The same shape is confirmed by the other checked guides, with lower numbers at the tight end, Dazao puts ±0.01–0.02 mm at 2.8–3.8× and ultra-tight work at 4.5–8.0×, Xometry's guide puts ±0.005 mm at 4–8×, so Sinbo's 8× and 15× are the upper end of the checked range, and the article uses them as the table while noting the range. The shape is what matters, and every source agrees on it: the cost curve is exponential, not linear.
As one guide puts it, when you put strict tolerances all over a drawing, you are not sprinkling quality. You are dialling in a global cost multiplier.
The default that avoids all of this is ISO 2768-m, the general tolerance that applies to every dimension on a drawing that carries no individual tolerance. One correction to the shorthand: ISO 2768-m is not a fixed ±0.1 mm. The standard's table is stepped by size: class m is ±0.1 mm up to 6 mm, ±0.2 mm to 30 mm, ±0.3 mm to 120 mm, ±0.5 mm to 400 mm.
Class f (fine) is ±0.05 mm up to 6 mm and ±0.1 mm to 30 mm. The pipeline's "general ISO 2768-m ±0.1 mm, fine ±0.05 mm" is the smallest-range shorthand; the article uses the full table, and the correction is recorded below. A 25 mm length under ISO 2768-m may measure anywhere between 24.8 and 25.2 mm, and that is what an ordinary machine shop achieves without special effort.
The strategy, from Sinbo: tolerate the function, not the part. On a typical part, 80% of features can be toleranced at the loosest standard (ISO 2768-m or -c) and only 20% or less need tighter control, and that one note can cut part cost by 30–50%. The tight tolerance goes on the feature that mates, seals, or locates, the bearing bore, the dowel hole, the sealing face, and nowhere else.
This is the same point as Article #8, from the other side: the stack-up consumes the tolerances you specify, so specify them where the assembly needs them and let the rest be loose. A tolerance tighter than the process can hold is not a specification. It is a wish, and the shop will either charge for it, or quietly ship parts that do not meet it.
Rule 7
A three-axis machine can only reach features from one orientation at a time, so every face that needs cutting from a different direction is a setup, and a setup is a fixed cost paid once per batch, whether the batch is one part or five hundred.
The checked arithmetic (MachiningSupplier's worked example): a part requiring four setups on a three-axis machine costs $50 of setup labour per setup plus about $100 per fixture, $200 of labour plus $400 of fixtures, $600 of setup cost per batch. The same part on a five-axis machine needs one setup: $50 of labour plus one fixture, $150. Setup savings alone: $450 per batch. The pipeline's figure, each setup costs $30–80 in labour and lost spindle time, and removing one saves 2–3× that once reduced inspection, fewer datum-transfer errors, and lower scrap are counted, is consistent with that example: the total setup cost ($600) is three times the labour alone ($200).
The article uses $50 of labour plus $100 of fixture per setup as its working figure, $150 in total, and the 2–3× as derived from the checked example rather than a published number.
Each additional setup adds 15–30 minutes of non-productive time plus programming overhead (MachProBot), or 20–60 minutes of operator time for a typical job (HulkMetal), and fixture setup is usually 30–60 minutes (RivCut). Reducing a part from three setups to two can save 10–20% of total cost. And the cost is not only money: every time a part is removed and re-clamped, a small positional error is introduced at every transfer, 0.02–0.05 mm of alignment error per setup (MachiningSupplier), which accumulates across the transfers and eats the stack-up budget from Article #8. Five transfers at the worst end is 0.25 mm of datum error before a single feature is cut.
The scale of the problem is best seen in one checked figure: a small part requiring 30 minutes of actual cutting can bill 7.5 hours across five operations at 1.5 hours of setup and NC programming each, fifteen times more setup than cutting. That is why the setup count, not the hourly rate, is the single largest lever on unit cost for complex parts, and why the design rules are what they are: orient critical features so they can be accessed from a single direction when possible, design flat reference surfaces that allow stable clamping, group features onto few faces, and put the tight positional relationships between features on the same face.
A five-axis machine removes setups by tilting the part to the tool, but it charges a premium hourly rate, so for parts with features on only one or two orthogonal faces, three-axis is still the cheaper process. The right question for the quote is not the hourly rate. It is the setup count.
Rule 8
Two alloys with the same base metal can machine nothing alike, and the grade you choose sets the cycle time before the shop sees the drawing.
Aluminium 6061-T6 is the default: good strength (310 MPa tensile), weldable, anodises predictably, and the workhorse for housings, brackets, and fixtures. 7075-T6 gives roughly double the yield strength (570 MPa, 1.84 times 6061) and is common in aerospace structure, but it is more abrasive on tooling, expensive, not weldable, and prone to stress corrosion if you leave sharp internal corners, which is Rule 1 again, with a material reason behind it. The machinability ratings, relative to AISI 1212 carbon steel at 100%: 6061-T6 80%, 7075-T6 70%, stainless 303 70%, stainless 316L 40%. A part that takes 30 minutes of cutting in 6061 takes roughly twice as long in 316L on machinability alone.
Stainless steel 303, 304, and 316 are where the material decision bites hardest. 303 is the free-machining grade: sulfur is added on purpose to break chips, so it turns cleanly, holds tight tolerances with less tool wear, and is the cheapest path for bushings, fittings, shafts, and anything with a lot of turning and threading. The trade is real: the sulfur inclusions are weak points, so 303 resists corrosion less than 304 and is weaker in fatigue and harder to weld. 304 is the general-purpose grade, tougher, welds well, handles most indoor and outdoor parts, but on the machine it galls, and tapping 304 without a proper cutting fluid can ruin a tap in a handful of holes. 316 and 316L add molybdenum for chloride resistance (food, medical, marine), and 316L's lower carbon suits welded assemblies. Both are gummy to machine.
The mechanism that makes stainless expensive is work hardening. Austenitic stainless steels like 304 and 316 harden when they deform: a dull tool rubs instead of cutting, the surface hardens under the tool, and the next pass is cutting a harder material than the last one. The hardened layer can reach 1.5 to 2 times the base hardness within 0.1 mm of the surface.
The fix is feed, not speed, keep the tool biting under the hardened layer, with sharp edges, a rigid setup, and plenty of coolant. A light spring pass on 304 usually fails: the tool rubs, the surface hardens, and the finish gets worse with every pass. Stainless also conducts heat poorly, roughly one third the thermal conductivity of carbon steel, so the heat from cutting stays near the edge instead of flowing into the chip.
And the material rules feed back into the geometry rules: high-strength alloys like Ti-6Al-4V or 316L require increased corner radii to prevent tool deflection and work hardening, a thin wall in 304 deflects under cutting force at 0.5 mm, and a sharp internal corner in 7075 is a stress-corrosion site. Choose the alloy for the environment the part lives in, and then design the features for the alloy you chose.
Example Labs is a made-up company we use for worked examples.
Example Labs' sensor hub lid: as drawn, and as fixed
The demo part is the Example Labs field sensor hub from Articles #16 and #7, the same 100 × 60 × 40 mm enclosure, now as a machined 6061-T6 lid instead of a moulded one. As drawn, it carries every mistake in this article at once. The arithmetic below was run in Python before writing; the published inputs are the rules and tables above, and the part, its dimensions, and its prices are the article's own worked example, labelled as such.
As drawn. A sensor pocket 30 mm deep with R2 internal corners. A lid flange 1.0 mm thick and 12 mm tall. A Ø3 mm hole, 30 mm deep. Four M4 tapped holes with 12 mm of thread. Twenty-eight dimensions at ±0.01 mm. Features on six faces. Material 6061-T6, batch of ten, baseline part cost $160 at ±0.5 mm (the article's own baseline, used consistently through the demo).
Step 1, the corners. R2 forces a 4 mm end mill. At 30 mm deep, that tool's length-to-diameter ratio is 7.5:1, interpolated from the checked deflection table, 16.2 times the deflection of the 3:1 baseline. The fix is R10, one-third of the 30 mm depth: a 20 mm end mill, length-to-diameter 1.5:1, deflection factor 1.0. The stiffness difference between the two tools at the same 30 mm overhang is the fourth power of the diameter ratio: (20 ÷ 4)⁴ = 625 times. And the smaller step the guides quote, R2 to R4, already doubles the allowable tool size and quadruples the material removal rate.
Step 2, the wall. The flange at 1.0 mm thick and 12 mm tall has a height-to-thickness ratio of 12:1, past the 10:1 chatter line, and three times the 4:1 design rule. The fix is 3.0 mm thick: 4:1, inside the rule, with the same 12 mm height. The wall is still thin enough to be light; it is now thick enough to be a wall instead of a tuning fork.
Step 3, the holes and the threads. The Ø3 mm hole at 30 mm deep is 10:1, beyond the 4:1 standard, past the G83 peck-drilling band, into dedicated deep-hole tooling. The fix is to open it to Ø5 mm and drill from both faces: 15 mm per side, 3:1 each, a standard drill cycle with no pecking. The M4 threads at 12 mm deep are 3× the diameter in aluminium, where 2× is full strength, 4 mm of thread that buys nothing and costs tapping time and tap-breakage risk on every hole. The fix is 8 mm of thread (2×D), with the drill depth at thread depth plus half the diameter, 10 mm, plus the 1.2 mm drill-point allowance.
Step 4, the tolerances. The cost bands from Rule 6, applied to the $160 baseline: ±0.5 mm is $160, ±0.1 mm is $240, ±0.05 mm is $400, ±0.025 mm is $640, ±0.01 mm is $1,280, ±0.005 mm is $2,400. As drawn, with ±0.01 mm on all twenty-eight dimensions, the part is $1,280. Fixed, ±0.01 mm on the two bearing bores only, ISO 2768-m (±0.2 mm for the 6–30 mm features) everywhere else, the part machines in the ±0.05 mm band at $400. The saving is $880 a part, 68.8%, from one CAD edit: deleting twenty-six tolerances. That is inside the checked shape of the saving, loosening 80% of a part's features to the loosest standard cuts cost by 30–50%, and this part loosens 93% of them.
Step 5, the setups. As drawn, six faces means six setups at $150 each ($50 labour, $100 fixture): $900 a batch. Fixed, the features reoriented onto two faces, with the tight positional relationships on the same face, two setups: $300 a batch, a $600 saving. And the datum error: five transfers at 0.02–0.05 mm each is 0.10–0.25 mm of accumulated error before a feature is cut, up to a quarter of Article #8's 1.0 mm camera-to-lid gap band, consumed by fixturing alone. The fixed part has one transfer: 0.02–0.05 mm.
Step 6, the material, and the total. Had the lid been specified in 316L instead of 6061, the same geometry, the same drawing, the machinability ratings (80% against 40%) say the cutting time roughly doubles: 30 minutes of cutting becomes 60, before the work-hardening risk on the thin walls is counted. The total, per part at a batch of ten: as drawn $1,370 (($1,280 × 10 + $900) ÷ 10); fixed $430 (($400 × 10 + $300) ÷ 10). The saving is $940 a part, 69%, and the fixed part is the same part, in the same material, doing the same job. The only thing that changed was the drawing.
The decision test
Five questions, before the drawing leaves your desk.
- What is the smallest internal corner radius on the part, and is it at least one-third of the pocket depth? If it is not, the shop is buying a smaller tool, a slower feed, and a chatter risk, and you are paying for all three.
- What is the deepest pocket's depth-to-width ratio, and is it 3:1 or less? Above 4:1 you are paying for extended-reach tooling and 30–50% more cycle time. Above 6:1 you are paying for a different process.
- What is the tallest wall's height-to-thickness ratio, and is it 4:1 or less? Past 10:1 the wall chatters. Past 15:1 it is not a machined feature.
- How many dimensions carry a tolerance tighter than ±0.05 mm, and does each one mate, seal, or locate something? Every tolerance that does not need to be tight is a cost multiplier on the whole part. Loosen it.
- How many faces does the part need cutting from, and how many setups is that? Every setup is $150 a batch and 0.02–0.05 mm of datum error. If the answer is more than two, reorient the features before you quote.
Objections
"The mating part needs a sharp corner." Then put the clearance on the mating part, or use a dogbone or T-bone fillet in the pocket. A sharp internal corner is not a design requirement. It is a request for a second process, priced accordingly.
"The wall has to be thin, the part has to be light." Then make it thin where it is short, support it where it is tall, or make it from a stronger alloy instead of a thinner wall. 7075 gives nearly twice the yield strength of 6061 at the same thickness. A thin wall that chatters is not light. It is scrap.
"We need ±0.01 mm, it's a precision part." Then put ±0.01 mm on the two features that are precision features, and ISO 2768-m on the other twenty-six. A part with two precision features is a precision part. A part with twenty-eight is a part that costs eight times what it should.
"Five-axis will fix the setups." Five-axis removes setups, and charges a premium hourly rate for the privilege. For a part with features on one or two faces, three-axis is still cheaper. Count the setups first, then choose the machine, not the other way round.
"The shop will figure it out." The shop will figure it out by quoting you for it: a smaller tool, a slower feed, a second operation, a sixth setup. DFM is not the shop's job. It is the drawing's job, and the drawing is yours.
Sources
- FabCon, "CNC Machining Design Guidelines for Manufacturable Parts" (updated 29 Oct 2026)
What we used
Corner radius at least one-third of pocket depth (30 mm pocket → radii ≥ 10 mm); pocket depth-to-width 3:1 or less, above 4:1 extended-reach tooling; wall floors 0.8 mm metal / 1.5 mm plastic; practical minimums 1.5 mm aluminium, 2.0 mm steel, 2.5 mm titanium, 2.0 mm plastics; walls taller than 10× thickness chatter; standard drill depth 4:1 or less; R2 → R4 fillets double the tool size and quadruple material removal rate
- MakerStage, "CNC Design Guidelines: Walls, Pockets & Threads (2026)"
What we used
Pocket 3:1 standard, extended-reach to 6:1 at +30–50% cycle time and Ra 1.6–3.2 μm vs 0.8–1.6 μm; wall recommended minimums aluminium 1.0 mm, stainless 1.3 mm, titanium 1.5 mm, plastics 1.5 mm; H/t ≤ 4:1 unsupported, walls taller than 15× not practical; corner radius ≥ 1/3 pocket depth and 130% of tool radius
- Sekkei Tech, "Machining Design Guidelines" (7 Aug 2026)
What we used
Pocket depth ≤ 3× end mill diameter for good results, 4× with reduced feeds, beyond 5× special tooling; wall minimums aluminium 0.8–1.0 mm, steel 1.5–2.0 mm; design for minimum setups, 3 faces or fewer
- Dazao, "CNC Pocket Design Guidelines: Depth, Radius & Cost Guide"
What we used
Deflection table vs 3:1 baseline (4:1 = 2.37×, 5:1 = 4.63×, 6:1 = 8.0×, 8:1 = 18.96×, 10:1 = 37.04×); deflection scales with cube of length and inversely with fourth power of diameter; pockets to 8–10× tool diameter possible only as specialised high-cost manufacturing
- Hubs, "Sharp Corners in CNC Machining"
What we used
Minimum internal corner radius equals cutter radius; corner radii at least one-third of cavity depth; cavity depth two to three times cutter diameter
- Anebon, "Why Internal Corner Design Matters for Cost Reduction in CNC Milling"
What we used
One-third-of-depth rule (15 mm pocket → ≥ 5.0 mm radius); tool engagement angle rises in tight corners → deflection → chatter → tool breakage; specify a radius slightly larger than the tool radius (5.0 mm → 5.2 or 5.5 mm); L:D ratio 3:1
- XTJ CNC, "CNC Machining Thin Walls"
What we used
Thin wall defined as H/t above ~4:1; minimums aluminium 6061/7075 0.5 mm at ±0.05 mm, stainless 304/316 0.8 mm, titanium 1.0 mm, plastics 1.0–1.5 mm; minimums assume walls under ~25 mm, doubling height beyond that needs +30–50% thickness
- Sinbo Wiki, "Minimum Wall Thickness for CNC Machined Parts"
What we used
Aluminium 0.5 mm absolute / 1.0 mm recommended, steel 0.8 / 1.5, stainless 0.9 / 1.5, titanium 1.0 / 1.5; maximum unsupported height 8× wall in aluminium, 5× in steel; wall below the recommended minimum costs 1.3–2.0×
- eMachineShop, "How to Design Holes for CNC Machining"
What we used
Standard drilled holes within roughly 4:1 to 6:1 depth-to-diameter; beyond 4–6×, standard twist drills wander and struggle with chip evacuation; deeper holes need gun drilling or peck cycles
- Cutting Tool Engineering (Kennametal), "When Chips are Down" (June 2003)
What we used
Standard twist-drill flutes handle chips to about 4:1 depth-to-diameter; beyond that, tools designed for deep-hole drilling; pecking shortens tool life, reduces productivity, can diminish hole quality; parabolic drills to 15×D without pecking below 25–26 HRC
- ToolSpecVault, "Peck Drilling Cycle Calculator: Fanuc & Haas G83 vs G73"
What we used
G73 for 2.5×D–4.0×D, G83 for deeper than 4.0×D, Q = 0.50×D to 0.75×D
- CNC Parts Manufacture, "Threaded Holes: Depth, Drill Size and How to Call Them Out"
What we used
Load concentrated in first few threads, ~1 diameter approaches full strength in steel, ~1.5 diameters safely full; steel 1–1.5×, aluminium ~2×, plastics 2–3× or insert; tap drill = major diameter − pitch; drill depth ≈ thread depth + half the thread diameter; 75% thread engagement
- Flying Chip Factory, "Aluminum Thread Design"
What we used
Aluminium engagement ~1.5× nominal diameter, no appreciable strength gain beyond; first thread carries 34% of load (7/8-9 Grade 8 nut)
- Siemens Community, "How to calculate Thread depth and Hole depth clearance"
What we used
Thread depth 2× nominal diameter for aluminium, 1.5× for steel; clearance at least 2× thread pitch
- Sinbo Wiki, "DFM: Tolerance Design | Cost vs Precision"
What we used
Cost table (±0.5 mm 1.0×, ±0.1 mm 1.5×, ±0.05 mm 2.5×, ±0.025 mm 4.0×, ±0.01 mm 8.0×, ±0.005 mm 15.0×); ±0.1 → ±0.05 mm costs +67%, ±0.05 → ±0.01 mm costs +220%; "the single most impactful DFM decision you can make is to loosen every tolerance that does not need to be tight"; 80% of features at ISO 2768-m/-c, loosening cuts cost 30–50%
- iStar Machining, "Strict CNC Tolerances: How They Raise Part Cost"
What we used
±0.05 mm adds ~1.5–2×, ±0.025 mm lands 3–4×, ultra-tight ±0.0025 mm up to 10–24×
- Dazao, "CNC Tolerance Design: GD&T, ISO 2768 & Cost Optimization"
What we used
±0.01–0.02 mm at 2.8–3.8×, ultra-tight under ±0.005 mm at 4.5–8.0×+; over-specifying tolerances is the primary driver of inflated budgets
- Makerverse / Calibr.pro / Fictiv, ISO 2768-1:1989 Table 1
What we used
Class m: ±0.1 mm to 6 mm, ±0.2 mm to 30 mm, ±0.3 mm to 120 mm, ±0.5 mm to 400 mm; class f: ±0.05 mm to 6 mm, ±0.1 mm to 30 mm. and https://calibr.pro/tables/iso-2768-tolerance-chart/
- MachiningSupplier, "5-Axis Setup Reduction Guide"
What we used
4 setups on 3-axis at $50/setup labour plus 4 fixtures at $100 = $600; 5-axis 1 setup = $150; saving $450 per batch; alignment error 0.02–0.05 mm per setup
- MachProBot, "CNC Machining Cost: 12 Design Rules to Cut It" (6 Oct 2026)
What we used
Each additional setup adds 15–30 minutes non-productive time; 3 → 2 setups saves 10–20% of total cost; good fixturing can eliminate a setup, saving $50–200 per part in prototype quantities; machine time 40–55% and setup & programming 10–20% of total cost
- HulkMetal, "Multi-Axis CNC Machining: Cut Setup Times and Unit Costs"
What we used
Operator time 20–60 minutes per setup; setup is a fixed cost paid once per batch; a six-face housing can need six setups
- RivCut, "Low-Volume CNC Production: 10–500 Piece Runs"
What we used
Fixture setup usually 30–60 minutes per setup; at 10 pieces the setup cost is $30 per part
- The Data Scientist, "Pocket Design in CAD: Hidden CNC Manufacturing Risks"
What we used
A small part needing 30 minutes of actual cutting can bill 7.5 hours across five operations at 1.5 hours of setup and NC programming each
- GL CNC Machining, "Metal Alloy Basics: The Complete CNC Machinability Guide"
What we used
6061-T6 workhorse, 7075 roughly double the yield strength, more abrasive, prone to stress corrosion at sharp internal corners; 304 work-hardens the moment the tool rubs; 303 contains sulfur to break chips; work-hardening fix is feed, not speed
- GL CNC Machining, "Stainless Steel CNC Parts: 5 Essential Grade Basics"
What we used
303 easiest stainless to machine, lower corrosion resistance; 304 galls, tapping without proper cutting fluid can ruin a tap; 316/316L add molybdenum for chlorides; 0.5 mm wall in 304 deflects under cutting force
- GL CNC Machining, "CNC Processed Stainless Steel"
What we used
Hardened layer 1.5–2× base hardness within 0.1 mm of surface on 304/316L; stainless thermal conductivity roughly one third of carbon steel
- Anebon, "Engineering Guide: Selecting the Best Types of Metals for CNC Machining"
What we used
Machinability ratings: 6061-T6 80%, 7075-T6 70%, 303 70%, 316L 40%; tensile 6061-T6 310 MPa, 7075-T6 570 MPa, 303 620 MPa, 316L 560 MPa; high-strength alloys (Ti-6Al-4V, 316L) require increased corner radii