Most expensive parts are not expensive because of the material. They are expensive because the drawing fights the process. A DFM review before cutting catches the choices that add setups, break tools, or drop yield — usually without changing the part's function at all. We run this review on every quote, because a half-hour conversation at the drawing stage beats a $3,000 scrap run after the steel is cut. These are the five decisions we flag most often, and what each one costs you if you leave it alone.
1. Internal corner radii
A mill cuts with a round tool, so a true sharp internal corner is impossible without EDM. Specifying R0.5 on a pocket that a 6 mm end mill reaches means either a smaller tool, more passes, and a longer cycle, or a wire EDM operation that adds a whole process step. Give the corner a radius near your smallest practical cutter and the pocket mills in one tool. We regularly save 30–40% cycle time just by opening internal radii from R1 to R3 on aluminum housings.
The same logic pushes into the choice of machine. Deep pockets with tight internal radii that also need compound angles are exactly where 5-axis machining earns its keep: the tool can tilt to reach the wall in a single setup instead of us re-fixturing three times. When we see a radius that seems to demand EDM, we first ask whether a slightly larger radius or a tilted approach removes the need entirely, because every extra setup is a chance to lose accuracy and add lead time.
2. Thin walls and islands
Walls thinner than about 0.5 mm in aluminum, or 1 mm in steel, chatter and deflect unless the whole strategy is built around them. The mistake is specifying a uniform thin wall across the entire part when only one local feature needs it. If the wall only needs to be thin locally, keep the rest of the web thick and relieve just the feature. Function usually does not require a uniform 0.4 mm wall across the whole part, and the thicker web stops the part from singing on the spindle.
When a thin wall is genuinely required everywhere, we change the sequence rather than the tool. Roughing leaves 0.2–0.3 mm and we finish with a low radial depth and a sharp, well-supported cutter, often climbing to keep forces pushing the wall into the stock instead of away from it. Trochoidal paths help on long walls. The point is that thin walls are a process decision, not just a number on the print, and the process should be decided before the material is on the table.
3. Deep holes
Drilling depth should stay under about 4× diameter with a standard twist drill before chip evacuation and peck cycles become a real problem. A Ø3 mm hole 40 mm deep is asking for a broken drill and a scrapped part. If the geometry allows, open the hole from both sides, or step up to a gun drill for true deep-hole work. We have seen a "through hole both sides" note cut drilling scrap from 6% to near zero on a 300-piece batch.
Interrupted holes are worse than deep ones. A hole that breaks out into a slot halfway down sees the drill tip lose support and walk. We either pre-bore a relief or schedule the drilling before the slot is cut. And if the hole carries a tolerance tighter than ±0.05 mm at 10×D, plan on a reamer or a boring operation up front — the twist drill will not hold it, and hoping it does is how batches get rejected at incoming inspection rather than caught on our floor.
4. Non-standard threads
A standard M6×1.0 or ¼-20 taps from stock in seconds. A custom 5.2×0.9 thread means a special tap, longer lead time, and a single-source tool. Unless the thread is doing something a standard one cannot, specify the catalogue size. The same logic applies to hex sizes, keyways, and O-ring grooves — standards are standards because the tooling already exists on the shelf and the lead time is zero.
Thread callout style matters too. A full-depth profile on a soft material like 6061 is fine; the same depth on 17-4PH will work-harden under the tap and snap it. We often suggest a modified minor diameter or a roll-tap on ductile materials to extend tool life. And on a rapid prototyping job, we may swap a tapped hole for a Helicoil or a pressed insert if it gets the function without waiting two weeks for a custom tap — the prototype proves the fit, not the thread spec, and the production print can carry the real thread later.
5. Tolerance stacking and material choice
The classic error: every dimension on the print gets ±0.01 mm, including ones that never touch a mating part. Each tight callout forces a slower process and a measurement. Tighten only the dimensions that function, and open the rest to ±0.05 or ±0.1. We reviewed one bracket where dropping non-critical dims to ±0.1 mm removed two inspection points and let the shop use a faster roughing strategy — 18% cheaper, no function lost.
We also watch the datum chain. A position callout referenced to a datum far down the chain inherits every error in front of it, so a ±0.02 requirement lands on a feature that can drift ±0.05 before you start. Re-anchoring the DRF to the functional surface often relaxes the number you actually need to hold. The tolerance is not free money — spend it where the part fits something, and stop spending it where it does not.
The print and the material are not separate decisions either. A feature that is hard in 4140 is easy in 6061, and a wall that chatters in steel may be calm in aluminum. When a customer asks for 17-4PH on a part with thin walls and deep holes, we suggest a conversation about whether the hardness is needed everywhere or only at the wear surface. Free-machining grades like 1215 or 360 brass cut clean and hold tolerance with less effort; 316L work-hardens and needs sharp edges and constant feed. Raise it during the review, while the drawing is still a drawing.
6. DFM checklist and what it changes on the floor
- Open internal radii to at least the smallest practical cutter, not a sharp corner that needs EDM.
- Localize thin walls — keep the surrounding web thick unless the whole part truly needs to be thin.
- Cap hole depth near 4× diameter, or plan a gun drill or a both-sides break-through.
- Use catalogue threads and standard keyways unless a custom one earns its cost.
- Tighten only functional dims and let the rest sit at ±0.05 mm or looser.
| Drawing choice | Left alone | After DFM pass |
|---|---|---|
| Internal corner radius | R0.5, EDM needed | R3, mills in one tool |
| Thin wall | 0.4 mm uniform, chatters | local relief, stable cut |
| Deep hole | Ø3×40 mm, 6% scrap | both sides, near 0% |
| Thread | custom tap, 2-week wait | M6×1.0 stock tool |
| Tolerance | all ±0.01 mm | ±0.1 mm non-critical |
"Tight tolerances are free on paper and expensive at the machine. Spend them where the part actually fits something."
7. How we run the review and the payoff
Our DFM pass is a written note attached to the quote, not a handshake at the counter. It lists each flagged feature, the suggested change, and the reason, with a rough cost or yield effect where we can estimate one. The customer signs off or tells us to leave it — either way the decision is recorded before metal moves. That paper trail matters: when a tolerance is intentionally opened, the FAI and control plan reflect it, so the part is never measured against a requirement nobody intended to hold.
A DFM pass is not us negotiating your design down. It is finding the version of the print that makes the same part for less, with better yield. For a recent robotics flange, three of these five changes took the piece price from $14.20 to $9.80 at 1,000 pieces — same function, same material, fewer fights with the process. The customer kept the design intent and dropped the cost.
Send the drawing early, not after the first batch fails. A 20-minute DFM review beats a $3,000 scrap run every time, and on a prototype turn it often means the difference between a part that assembles on arrival and one that needs a second operation nobody budgeted for. The review pays for itself the first time it removes a single EDM operation from the build.
This is a short version — the full list of design rules is on our DFM guide.