How we use this list
Every drawing we receive passes through a single manufacturing engineer before pricing is touched. That engineer has this checklist open on a second monitor and annotates the drawing in a bright colour for any item that fails — wall too thin, thread ambiguous, tolerance blanket, etc. The annotated drawing comes back to the customer with the quote, so what was flagged is always visible.
The goal isn't to reject drawings. It's to fix them cheaply, at the quote stage, before any metal has been cut. A 10-minute design change that moves a wall from 0.3 mm to 1.0 mm saves three days of hand- finishing at the back end, and the customer keeps their schedule.
The 24 items below are grouped the way an engineer walks through a drawing — geometry first, then features, then tolerance, then finish, then the drawing package itself. Run through them in the same order before you send and you'll shave days off your quote cycle.
0.8 mm minimum for metals, 0.5 mm for plastics — walls below this chatter during finishing and fail FAI. If weight is critical, add ribs rather than thinning walls further. We flag any wall under this threshold in the quote response.
No sharp 90° internal corners — tool radius drives the minimum. Default to the tool radius you're willing to pay for: a 3 mm radius uses a common Ø6 end mill and runs fast; a 0.5 mm radius requires a Ø1 mm end mill and adds 30 – 50 % cycle time. Call out the radius you can accept — don't let us guess.
4:1 is standard and cheap. 6:1 requires peck drilling — add ~20 % cycle. 10:1 requires gun drilling on a specialised machine and doubles the operation cost. If your depth is >10:1 consider splitting into two counter-bored holes.
Smallest feature we can machine is ~0.2 mm, but only on a 3-axis straight-down cut. An 0.2 mm feature at the bottom of a 20 mm pocket needs a Ø0.4 mm end mill running at 80,000 rpm — we have the spindle, but expect +40 % cost for the extra setup. Put deep features on an accessible face where possible.
Undercuts on a 3-axis part require EDM or hand-finishing and cost more than adding a second setup. A 5-axis part handles undercuts in stride but at 5-axis shop rate. Side-drilled holes need either a 4th axis or a secondary op with a dedicated fixture — let us know if they're present, because we'll price one way or the other.
Tapped thread depth = 1.5× diameter for steel, 2× for aluminum. Anything deeper doesn't add thread engagement and wastes cycle time. For blind holes, leave at least 0.5× thread pitch as unthreaded relief at the bottom to protect the tap.
Use full callout: 'M6×1.0 — 12 deep, fully threaded 10 deep, fits ISO 2 (6H)'. Avoid ambiguous 'M6 tapped' — we'll default to ISO 2 6H at 2× thread depth, which may not match your application.
M1 – M1.6 threads aren't tapped, they're thread-milled with a specialised cutter. Per-hole cost is ~3× a standard M3 tap. For a design with many small threads, consider self-tapping inserts or press-fit threaded inserts — they're often cheaper at >10 holes per part.
Specify the fastener head standard (ISO 10642 for countersunk M-series, ANSI for UNC). 'Countersink for M4' is ambiguous — we'll default to ISO 10642 (90°) but some customers expect 82° (ANSI) and reject parts. Just write the standard.
Specify the insert size and the pre-tap hole diameter — two different numbers. 'M5 Heli-Coil' is a M5 final thread, but the pre-tap is Ø5.4 mm × 1.3D deep, which is bigger than a regular M5 tap. This trips up first-timers frequently.
Write 'ISO 2768-m' or 'ISO 2768-f' in the title block. Anything undimensioned then falls under that grade. If you don't specify, we default to ISO 2768-m. Calling out every tolerance individually is both slower for you and error-prone.
Star (★) or box-frame the dimensions that drive assembly. CMM inspection is added to these and only these — blanket CMM on every dimension doubles inspection cost. We ask for a drawing with critical dimensions marked; if none are marked, we assume nothing is critical.
Provide a datum reference frame (A, B, C). Without it, we have to pick the largest flat face as A and guess B and C — usually fine, but not if the part has a non-obvious mounting orientation. For high-mix jobs, a clean DRF reduces CMM re-runs and shipment delays.
A profile tolerance of 0.2 mm on an entire surface is not the same as ±0.1 mm on each point — profile is tighter because it includes form. Call out profile only on critical surfaces like mating faces and O-ring grooves.
We hold flatness 0.02 mm on faces machined in one setup. Perpendicularity between a machined face and a datum face is ~0.03 mm on parts up to 200 mm. If you need tighter, specify and we'll add a grinding step — typically +2 days lead, +15 % cost.
Ra 0.8 μm on every face of a part adds polishing time for no benefit on hidden surfaces. Call out Ra only on faces that need it: sealing surfaces, aesthetic surfaces, sliding bearings. Hidden internal surfaces stay at default machined finish (Ra 1.6 – 3.2 μm) without callout.
All sharp edges need a deburr step — standard is a light break, 0.2 – 0.3 mm chamfer. For appearance parts specify 'break all edges 0.3 mm chamfer'. For parts going into assembly with gaskets, 'break edges ≤ 0.1 mm' prevents gasket damage.
Black Type II anodize is reliable to a hair's variation between batches. Red, blue, bronze anodize is dye-based and can shift 1 – 2 Pantone units between batches. If you need exact color across a production run, specify a reference sample and expect higher QC cost.
Specify plating thickness in microns — 'zinc plate' without a thickness defaults to ~8 μm. For high-strength steel (DP780 and above) plating requires a bake at 200 °C for 24 hours to relieve hydrogen embrittlement; we add this automatically but flag it in the quote because it's a 2-day lead adder.
STEP (.step/.stp) is the 3D standard — preferred. Parasolid (.x_t), IGES, and native SolidWorks (.sldprt/.sldasm) are also fine. 2D drawing must be PDF — never image exports of 2D views, which lose dimension links and are error-prone.
Include isometric for visual reference, plus front / top / side orthogonal views. Add section views for internal features (bores, pockets). Add detail views (2:1 or 5:1 scale) for features under 2 mm. A 2D drawing without detail views on sub-2 mm features gets flagged for re-issue.
Write the unit in the title block — 'ALL DIMENSIONS IN mm' or 'inches'. For projection method write 'Third Angle' (US/UK/Japan) or 'First Angle' (Europe/China). A drawing without projection notation is ambiguous on any drawing with internal features.
For multi-part assemblies, send a BOM with part number, quantity, material, and finish for each. A BOM prevents us from guessing which part is 'the big one' and reduces quote cycle from days to hours. Use the same part numbers on the STEP assembly tree.
Include a revision letter or date on every drawing. 'PartA.pdf' and 'PartA v2.pdf' sitting in the same email attachment is a cost bug waiting to happen. Use 'PartA-Rev-B-2026-04-19.pdf' and destroy old revisions in your own archive. We quote the latest revision only, and flag any mismatch between STEP and PDF.
What happens after a DFM flag
A flagged item doesn't kill the quote — it comes back to you as an annotation on the drawing with a suggested fix. In ~80 % of cases the fix is trivial (add a tolerance block, specify the thread class, bump a radius), and the customer re-submits the next day. In the other ~20 %, the flag reveals a design intent that needs discussion — a deliberate sharp corner for a seal groove, a blanket tight tolerance because of an unusual fit — and we get on a call with the customer's engineer to find the right manufacturing approach.
Either way, the flag prevents a worse outcome: a part that looks fine on the drawing, fails on the shop floor, and shows up late. The checklist above is the same one we've been sharpening for a decade across Japanese, American and European customer bases — the number of flags per drawing has dropped as customers have adopted it, and quote cycles have compressed from 3–4 days to under 24 hours for clean submissions.