Every week I quote parts that could cost 30-50% less with small design changes. Not major redesigns. Not different materials. Just geometry tweaks that most engineers don't know to make because nobody taught them the manufacturing side of design.
This checklist is what I run through mentally when I look at a drawing for quote. These are the things that drive up machining cost, and the specific changes that bring it back down. I've ordered them by cost impact — #1 is the biggest lever, #25 is for fine-tuning.
The pre-release DFM checklist
1. Internal corner radii: the single most expensive feature on most parts
A sharp internal corner requires EDM (slow, expensive) or a broaching operation. A corner with a standard radius equals an end mill corner — it's cut as part of the normal milling cycle at no added cost.
Rule: Minimum internal corner radius = 0.5× the largest end mill that can reach into the pocket. For a 50mm deep pocket, you need at least a 50mm long end mill, so minimum corner radius is typically 3-6mm. Shallower pockets can use smaller tools and tighter corners.
Cost impact: A part with sharp internal corners vs radiused corners on the same geometry — the sharp-corner version can cost 2-5x as much because EDM or broaching is a separate operation with its own setup, tooling, and cycle time.
Fix: If a mating part has a sharp corner where yours has a radius, add an undercut or relief to the mating part. If the corner serves no mating function, radius it and move on.
2. Deep pockets are exponentially more expensive than shallow ones
A pocket deeper than 4× the tool diameter is a deep pocket. The tool deflects, so you reduce radial engagement, slow the feed, and take more passes. At 6× diameter, it takes roughly 3x as long to machine as a 2× deep pocket of the same area.
Rule: Keep pocket depth under 4× the smallest required corner radius diameter. If you need a 3mm corner radius (6mm end mill), keep the pocket under 24mm deep. If it must be deeper, increase the corner radius to accept a larger tool.
Cost impact: A 50mm deep pocket with 3mm corner radius costs 4-5x what a 20mm deep pocket with 6mm corner radius costs. The machine time difference is that dramatic.
3. Internal threads in deep holes cost extra tooling
A tapped hole deeper than 2.5× diameter requires a bottoming tap (separate tool, separate operation). A blind threaded hole needs clearance at the bottom for chips and the tap lead-in.
Rule: Thread depth = 2× diameter for through-holes, 1.5-2× for blind holes. If you need more thread engagement, increase the hole diameter rather than the depth — a larger thread has more engagement area per unit length.
Cost impact: Minor on a per-part basis (extra tool change), but significant over thousands of parts. Also avoids the joy of broken taps in deep blind holes.
4. Undercuts are a pain but sometimes necessary
An undercut (relief groove, O-ring groove, snap ring groove) that's perpendicular to the tool axis requires a T-slot cutter or a keyseat cutter — special tooling, a separate operation, and an extra tool change. An undercut on a turned part at the shoulder requires a specific insert geometry.
Rule: If the undercut is on the internal wall of a bore, make sure there's tool access — the T-slot cutter's shank needs clearance through the bore entrance. If the undercut is on a turned part at a shoulder, check that standard threading/grooving inserts can produce it before going custom.
Cost impact: One undercut with tool access = one extra operation, minor cost. Seven undercuts with varying diameters = seven tool changes. Consolidate sizes where possible.
5. Reduce setups — each one costs money
Every time a part comes out of a vise for repositioning, you lose accuracy and add labor. A part that needs 3 setups costs about 3x the handling cost of a single-setup part.
Rule: Design parts so all critical features are accessible from one or two sides. If you need features on 5 faces, talk to the shop about whether 5-axis or a tombstone fixture could reduce handling — the machine cost is higher but the part cost may be lower.
Cost impact: Reducing a part from 3 setups to 2 usually cuts cost by 25-35%. Reducing from 2 to 1 cuts it by another 15-25%.
6. Wall thickness: too thin is a machining problem
Thin walls deflect under cutting pressure. They chatter. They generate dimensional variation because the tool pushes the wall away during cutting and it springs back after. Below a certain thickness, you slow down, take lighter passes, and sometimes scrap parts that chatter beyond tolerance.
Rule: Minimum wall thickness for metals: 0.5mm for small features under 10mm tall, 1mm for features up to 25mm tall, scaling upward. For plastics, double these numbers — plastics deflect more and have lower stiffness.
Cost impact: A part with 0.5mm walls that should be 1.5mm costs 2-3x more than the thicker version because of conservative machining parameters and higher scrap rate.
7. Datum features should be machinable in the first setup
The datum is what everything else references. If the datum face is machined in setup 1, and all other features reference that face in setup 2, the tolerance stack is minimal. If the datum is a cast surface or a face that isn't machined until setup 3, every subsequent setup adds positioning error.
Rule: Specify datums on surfaces that are machined early in the process sequence. If your drawing has datum A as the bottom face, datum B as a side face, and datum C as an end face, all of these should be machined in the first setup.
8. Holes should be standard drill sizes
A 5.1mm hole is a standard 5.1mm drill — cheap, in stock, ground to a standard tolerance. A 5.23mm hole requires a custom drill or an end mill circular interpolation pass — slower, more expensive, and harder to hold consistent diameter.
Rule: Use standard metric drill sizes (whole and half mm under 10mm, whole mm above). Check a standard drill chart before finalizing hole callouts on the drawing. If you need a precise diameter for a press-fit pin or bearing seat, that's fine — but don't use a non-standard size for a clearance hole when 5.5mm would work instead of 5.35mm.
Cost impact: Small on a per-hole basis, but cumulative — a part with 15 non-standard hole sizes needs 15 custom or interpolated operations instead of 15 standard drills.
9. Counterbores and countersinks: standard angles and depths
A standard flat-head screw uses an 82° or 90° countersink. If you spec an 87° countersink because that's what the CAD default gave you, the shop now needs a custom tool. Same for counterbores — standard socket head cap screw counterbore diameters and depths are published. Use them.
10. Engraving and marking: laser is cheaper than machining
Engraved text via CNC is a small end mill tracing letters — slow and fragile. Laser marking (done after machining) is faster and cheaper for batch quantities. Unless the engraving depth has a functional requirement (grip texture, fluid channel), use laser marking or chemical etch instead of machined engraving.
11. Stock size awareness reduces material cost
Standard aluminum plate comes in specific thicknesses: 6mm, 8mm, 10mm, 12mm, 16mm, 20mm, 25mm, etc. If your part is 21mm thick overall, it comes from 25mm plate and 4mm gets machined away. If you can make the part 19mm thick, it comes from 20mm plate and only 1mm gets removed — less cycle time, less material cost, less waste.
Rule: Design overall part thickness to be 0.5-2mm less than the next standard plate thickness. Check with your shop about which thicknesses they stock — different regions have different standard inventories.
12. Surface finish: only specify what you need
Ra 0.8 μm is a standard as-machined finish. Ra 0.4 μm requires an extra finishing pass (or grinding). Ra 0.2 μm is a polishing operation. Every step down in Ra number roughly doubles the cost of achieving it on that surface.
Rule: Only specify surface finish on functional surfaces — sealing faces, bearing seats, sliding contact surfaces. General external surfaces get the standard as-machined finish. If you blanket-specify Ra 0.8 on every surface, the shop might quote it that way. If you specify Ra 0.8 on three faces and leave the rest unspecified, they'll machine them to standard finish and you'll pay less.
13. Tolerances: tight tolerances on everything = expensive parts
A ±0.13mm tolerance is achievable in one pass on most materials. ±0.05mm needs attention but is standard. ±0.025mm needs specific tooling, slower feeds, and possibly temperature compensation. ±0.01mm needs a controlled environment, specific machine, and in-process measurement.
Rule: Only use tight tolerances on features where they matter — bearing bores, dowel pin locations, sealing surfaces, mating interfaces. General external dimensions: ±0.13mm is fine. Hole positions for clearance bolts: ±0.13mm is plenty.
Cost impact: A part with five ±0.01mm features costs 2-3x the same geometry with standard tolerances. Most of that cost is in inspection, not machining.
14. Avoid deep, narrow slots
A slot narrower than 3mm and deeper than 10mm eats small end mills. The tool deflects, chatters, and eventually snaps. The shop runs conservative feeds to keep the tool alive, which means longer cycle time and higher cost.
Rule: Slot width to depth ratio under 1:4. A 3mm wide slot should be no deeper than 12mm. Wider is better — a 5mm wide slot at the same depth machines twice as fast because you can use a larger, more rigid tool.
15. Design for the largest possible tool
A part machined with a 12mm end mill will cost less than the same part machined with a 3mm end mill — the 12mm tool is more rigid, removes material faster, and has longer tool life. Your design controls the minimum tool size through the smallest internal radius.
Rule: Every time you reduce the minimum internal radius from 1mm to 3mm, you roughly double the material removal rate in that feature. Crank up internal radii wherever the design allows.
16. Through-holes are cheaper than blind holes
A through-hole clears chips naturally — they exit the far side. A blind hole traps chips, requires a peck drilling cycle to clear them, and needs a bottoming tap if threaded. Through-holes are always cheaper.
Rule: If the hole doesn't need to be blind (no sealing requirement, no cosmetic constraint), make it through.
17. Avoid partial holes and hole intersections
A hole that breaks out the side of the part is a partial hole — the drill walks on entry, the hole is oval, and deburring the breakout is manual work. A hole that intersects another hole creates a burr at the intersection that's nearly impossible to remove.
Rule: If a hole needs to be near an edge, keep the full diameter at least 0.5mm inside the part boundary. If holes must intersect, the larger hole should be drilled first so the smaller hole's burr is at a predictable location.
18. Tapped holes in soft materials need more engagement
In aluminum, brass, and plastics, threads strip more easily than in steel. Standard thread engagement of 1.5× diameter works for steel. For aluminum and brass, use 2× diameter. For plastics, use 2.5× diameter or thread inserts.
Rule: If the material is aluminum and the thread is M6, specify at least 12mm of thread depth. If the material is PEEK or PTFE, use threaded inserts — plastic threads creep under sustained load and eventually loosen.
19. Symmetric parts are easier to fixture
A part with two parallel flat faces can go in a standard vise. A part with no parallel faces needs a custom fixture or a 5-axis setup. Symmetry makes fixturing easy; random shapes make it expensive.
Rule: If your part is free-form organic, budget for fixture cost in the quote. If you can add two parallel reference flats to an otherwise organic shape, do it — the fixturing becomes straightforward and the quote drops.
20. Radius external corners if possible
A sharp external corner on a milled part naturally forms where two perpendicular faces meet. But if the corner needs to be deburred, a radius (0.5mm or larger) is easily programmed and eliminates the manual deburring step. Sharp external corners catch on things (hands, packaging, mating parts) and almost always need breaking.
21. Keep features on orthogonal faces where possible
A hole at 23° to the main face requires either a compound-angle setup (time-consuming to indicate) or 5-axis machining (more expensive machine time). A hole that's perpendicular to a face is a simple drill operation.
Rule: Not every hole needs to be orthogonal — sometimes function demands an angle. But if you have 20 holes and 2 are at odd angles while 18 are square to faces, you've just added setup complexity. Consolidate angles where the design lets you.
22. Part size and machine selection
A 600mm long part needs a machine with 600mm travel. Most CNC machining centers have 500-1000mm X travel. Above 1000mm, the available machine pool shrinks and prices rise. If your part is 1050mm long and could be 950mm with a small redesign, you just went from "large format, limited shops" to "fits most standard VMCs."
23. Plating and coating: thickness affects machined dimensions
Type III hard anodize adds 25-50 μm to the surface — roughly half is penetration and half is buildup. A 10.00mm hole that gets hard anodized will end up at about 9.98mm. If the hole needs to be 10.00mm after finishing, either machine it oversize (10.02mm pre-plate) or mask it before anodize and accept that the masked hole won't be anodized.
Rule: State on the drawing whether dimensions are pre-finish or post-finish, and which features get masked during finishing. Ambiguity here causes scrap.
24. Batch quantity changes the economics
At quantity 1-5, setup and programming dominate the cost. At quantity 50-200, cycle time and material cost dominate. At quantity 500+, automation (bar feeding, pallet changers, robot loading) becomes viable and the per-part cost drops again.
Rule: Design for your target quantity. For prototypes (qty 1-10), optimize for speed of delivery and flexibility — don't over-DFM. For production (qty 100+), the DFM rules in this checklist pay back significantly. For high volume (qty 5,000+), invest in DFM optimization — every second of cycle time saved is real money.
25. Talk to the shop before locking the design
This one belongs at the top but I'm putting it at the bottom because it's the last thing anyone does and it should be the first. Send a preliminary drawing before the design is frozen. Let the shop look at it with their tools, their experience, and their cost structure. They'll spot things your CAD screen doesn't show you.
A ten-minute conversation during the design phase has saved my customers more money than any amount of post-design cost negotiation. The earlier you involve the shop, the more flexibility you have to change things without delaying the project.
Quick pre-release check
Before you send the RFQ, run through these five questions:
- Are all internal corners radiused at ≥0.5× the deepest pocket's expected tool diameter?
- Are tolerances tight only where function demands it, not blanket-specified?
- Are threads standard sizes, standard depths, and through-hole where possible?
- Can the part be held in a standard vise or does it need a custom fixture?
- Has a machinist looked at this drawing before it was signed off?
If the answer to #5 is no, get a second pair of eyes on it. The money you save will be your own.
Send us your drawing before it's final. We'll review it for free and tell you what to change before you lock the design. We do this every day and most of the feedback takes five minutes to review.