Most machining cost overruns are designed in, not machined in. Design for manufacturability (DFM) is simply reviewing a part the way a machinist will — asking what tool reaches each feature, how the part is held, and what has to be measured. Run this 12-point checklist before your next RFQ goes out; each item takes a minute to check and can save days of back-and-forth.
An end mill cannot cut a sharp internal corner. Specify internal radii slightly larger than a standard tool radius (e.g., R0.135 in for a 1/4 in end mill) so the tool can sweep the corner instead of dwelling in it. Sharp internal corners in pockets force EDM or broaching — a different process and price class.
Tools cutting deeper than roughly 3–4x their diameter start to deflect and chatter; beyond that, cycle time climbs steeply as the shop drops to lighter cuts. If a deep pocket is unavoidable, allow a larger corner radius at depth so a bigger, stiffer tool can do the work.
Walls below roughly 0.030 in in metal (thicker for tall walls) flex during cutting, causing chatter, taper, and scrap risk. Add ribs, thicken sections, or accept looser tolerances on thin features. Large thin floors in pocketed parts can also bow from residual stress — flag them so stock and stress-relief can be planned.
A hole at a standard drill or reamer size is one operation; an odd diameter means boring or interpolating. Check clearance holes against standard sizes and reserve custom diameters for genuine fits.
Specify the full designation (e.g., 1/4-20 UNC-2B), thread depth, and whether the hole is blind or through. Keep thread depth to ~1.5–2x diameter — deeper threads add little strength and much tapping risk. For soft materials under repeated assembly, consider inserts and say so on the drawing.
Choose datums on functional mounting surfaces the shop can actually fixture on. If every dimension chains from an edge no fixture can reach, inspection and machining both get harder. Three well-chosen datums beat six decorative ones.
A sensible title-block tolerance with feature-specific tight callouts is the single biggest cost lever on the drawing. Every tightened feature adds machining and inspection time — spend precision only where function demands it.
Call out finish on sealing, bearing, and cosmetic surfaces; leave the rest at a standard machined finish. A blanket fine-finish note quietly adds finishing passes to every face on the part.
Each machining direction is potentially a setup. Consolidating features onto fewer faces — or keeping compound-angle features compatible with 5-axis positioning — cuts setups, handling, and stack-up error.
Know your shop's work envelope before designing a monolithic part. For reference, Dynamics Group mills parts up to 51 x 22 x 20 in and turns diameters up to 14.96 in. Oversized weldments-then-machined or split designs are options, but they should be decisions, not surprises at quote time.
State alloy, temper or condition, and spec (e.g., 6061-T651 per AMS-QQ-A-250/11). Exotic grades and non-standard stock sizes can dominate lead time; if an equivalent common grade works, allow it on the drawing ("or equivalent, approval required").
Send a STEP model plus a PDF drawing. Native CAD is welcome but STEP is universal; DXF only helps for flat profiles. If the drawing and model disagree, state which governs. Include revision level on both — mismatched revisions are a classic source of quoted-wrong-part errors.
The best time for this review is before release, when changing a corner radius costs nothing. The second-best time is at RFQ, when a shop can still flag issues before metal is cut. Our team routinely returns DFM feedback with quotes — details on our capabilities are on the CNC machining page.
Have a design ready for a manufacturability check? Upload your model and drawing through our Request a Quote form — Dynamics Group responds within 24 hours.