Every part we machine starts as a drawing. Some drawings let us hit a price target with no problems. Some drawings have a single dimension that turns a $200 part into a $2,000 part — and the engineer who drew it had no idea. This is the checklist we run before quoting anything.

Geometry (12 checks)

Wall thickness — under 0.060" in aluminum, under 0.040" in steel? Expect deflection and chatter.
Internal radii — sharp corners require EDM or special tooling. Round to ⅛" or larger when possible.
Deep pockets — depth-to-width ratio over 4:1 requires long endmills, slow speeds, and tight tolerances cost extra.
Thin floors — pocket floors under 0.030" will deflect and chatter; consider stepping the depth.
Undercuts — require special tooling (T-slot, dovetail, or EDM). Call them out clearly.
Multiple setups — every datum face that needs to be the "up" face is a separate setup. Count them.
Threaded holes — bottom-tap blind holes need a relief; through-tap when possible.
Cosmetic surfaces — call out the face. Don't make us guess.
Through-holes vs blind — through is always cheaper.
Cross-holes — drilling into a curved or angled surface requires a flat or a spot-drill.
Slots — endmill diameter limits minimum slot width. Check our tooling library.
Draft — required on cast and molded parts; ignored on machined parts.

Tolerances (8 checks)

Default tolerance block — ±0.005" on three-place, ±0.010" on two-place is the standard. Tighter is more money.
Tolerance stack-up — does your assembly require ±0.001" on each part to work? Loosen what you can.
Position tolerance vs size — MMC/LMC modifiers can dramatically loosen real-world manufacturing.
Surface finish — 125 µin Ra is standard mill finish; 63 µin needs a finishing pass; 32 µin needs grinding or polishing.
Flatness / parallelism / perpendicularity — under 0.001" per inch usually requires grinding.
Concentricity — tight concentricity between two diameters often needs a single-setup turning op.
Datum scheme — every dimension should reference a clear datum chain.
Critical-to-function callouts — flag the dimensions that actually matter so we can focus inspection.

Material (6 checks)

Alloy and temper — "aluminum" isn't enough. 6061-T6 vs 7075-T6 vs 2024-T3 machine very differently.
Stock size — drawing nominal vs available bar/plate stock. Round up to the next standard size.
Heat treat — pre- or post-machining? Affects workholding and dimensional stability.
Coatings / plating — anodize, black oxide, zinc plate. Add to dimension or before/after?
Material certs — required for aerospace, defense, medical. Spec it on the drawing.
Magnetic permeability — for sensor housings, this matters. 304 stainless can become slightly magnetic after machining.

Threads & features (6 checks)

UNC vs UNF vs metric — pick one system and stick to it.
Thread depth — 1.5×D for steel, 2×D for aluminum is the rule.
Class of fit — 2B is standard; 3B is tight; ask before specifying 4B or higher.
Helicoils / Keenserts / PEM inserts — call out the part number and torque spec.
Chamfers and deburring — "break all edges" means something specific. Spec the chamfer size if it matters.
Knurling, engraving, marking — type, font size, location, depth, content.

The silent killers

These are the things that don't look like a problem on a drawing but blow up the price:

A 0.250" ±0.0005" bore (needs reaming or boring head, not drilling)
A 4-inch deep tapped hole on the back side (5th-axis or two setups)
Ra 16 finish on an internal pocket (probably needs ECM or polish)
±0.0002" flatness on a plate (grinding, lapping, or both)
A weld-then-machine sequence (distortion will move your tolerances around)
Tight concentricity between features in different setups (needs a single-op turning center with live tooling)

What we do when we see a tight feature

When we quote a part, our programmer flags every feature tighter than ±0.002" and every surface finish under 32 µin Ra. We reach out before we send a number and ask: does this really need to be this tight? Half the time, the answer is "no, we just used the default." That single conversation saves customers thousands per part.

If you're designing a part and want a free DFM review, send us the model. We'll mark up the things that will cost you the most and send it back, even if you don't end up buying from us.