DFM Checklist for Metal Parts: 20 Things to Check Before Sending to Vietnam

Design for Manufacturing (DFM) review catches the design decisions that make parts unnecessarily expensive or difficult to produce — before tooling or fixturing is built. This checklist covers the 20 most common DFM issues we see when buyers send drawings for CNC machined, die cast, sheet metal, and injection molded metal parts. Each item includes the specific requirement for Vietnam manufacturing conditions.

A real example of what DFM review is worth: on a 6061-T6 aluminum bracket ordered at 15,000 pieces/year, relaxing three over-specified tolerance callouts from ±0.01mm to ±0.05mm (which the functional assembly actually required) reduced unit price from $18.40 to $15.00 — an 18% reduction, or $51,000/year at that volume. The tolerances weren't wrong — they just had no functional basis.

Section 1: CNC Machining (Items 1–6)

1. Tolerance Callouts vs Process Capability

CNC machining on standard equipment (Fanuc-controlled machining centers) reliably holds ±0.05mm on most features. Tighter than ±0.025mm typically requires additional setups, slower feeds, and Mitutoyo or Zeiss CMM verification on every part — which multiplies cost. Tolerances tighter than ±0.01mm are achievable on DMG Mori or Mazak 5-axis equipment but represent premium territory.

Check: For each tolerance callout on your drawing, ask: "What breaks functionally if this is ±0.05mm instead of the callout I have?" If nothing breaks, relax it.

2. Deep Pockets and Thin Walls

Machined pockets deeper than 4:1 (depth:width ratio) require long-reach tooling, which is slower and more prone to chatter. A pocket 10mm wide and 50mm deep is a 5:1 ratio — it's machinable but at premium cost. At 6:1 or higher, deflection becomes significant and tolerances suffer.

Minimum wall thickness: 0.8mm for aluminum, 1.0mm for steel. Below these values, fixturing becomes complex and scrap rates increase.

3. Internal Corner Radii

Every internal machined corner requires a radius at least equal to the cutter diameter. Specifying sharp internal corners (R0) is impossible in machining — it requires EDM or hand filing. Use internal radii of at least 0.5mm (R0.5), and where possible R1.0 or larger. A common mistake is specifying R0.2 internal corners on pockets because it looks clean in CAD — these add significant cost or are simply not achievable without special tooling.

4. Thread Specifications

Specify threads using standard designations (M6×1.0, 1/4-20 UNC, etc.) with thread class called out (6H/6g for metric, 2B/2A for unified). Non-standard thread pitches require special taps that may not be stocked locally, adding lead time. For blind holes, specify minimum thread depth (not full depth) — a 20mm deep blind hole needs only 12mm of thread for most applications; requiring 18mm of thread in a 20mm hole creates tool breakage risk.

5. Surface Finish Callouts

Ra 3.2 µm is the standard machined finish from a properly maintained machine with appropriate feeds/speeds — no additional cost. Ra 1.6 µm requires a finishing pass. Ra 0.8 µm requires grinding or fine finishing operations. Ra 0.4 µm and below requires polishing or superfinishing and is a significant cost adder. Callouts like "32 µin" (Ra 0.8 µm) on non-functional surfaces add cost with no benefit.

6. Material Specification

Materials stocked locally in Vietnam (available within 1–2 weeks): 6061-T6, 6063-T5, 7075-T6 aluminum; A36, 1020, 4140 steel; 304, 316 stainless; ADC12 aluminum die cast alloy; ABS, PP, PE, PC plastics.

Materials requiring import (add 4–8 weeks to lead time): 7068 aluminum, 465 stainless, titanium 6-4, Inconel, most PEEK grades, some glass-filled engineering plastics. If your design specifies these, flag it early.

Section 2: Die Casting (Items 7–11)

7. Draft Angles

Every surface parallel to the die-pull direction requires draft — taper that allows the part to release from the die. Minimum draft for aluminum die casting: 1° per side for external walls, 2° for internal walls and cores. Features without adequate draft cause die sticking, pulled metal, and torn surfaces. Common mistake: a designer specifying 0.5° draft because it "looks right" — this leads to die galling and high scrap rates.

8. Minimum Wall Thickness (Die Casting)

Aluminum HPDC: 1.5mm minimum wall thickness for small parts (under 100cm²), 2.0mm for larger parts. Thinner walls cause cold shuts, porosity, and filling defects. Maximum wall thickness without porosity risk: approximately 6mm; beyond this, manage with coring (adding internal cores to reduce thickness) rather than designing solid walls.

9. Parting Line Placement

The parting line is where the two halves of the die meet — it will always leave a visible line on the part. Specify acceptable parting line location on your drawing or mark it "cosmetically acceptable." Placing the parting line on a functional sealing surface, bearing bore, or Class A face requires extra die polish and often secondary machining, both of which add cost.

10. Undercuts and Side Actions

Features that are perpendicular to the die-pull direction require side actions (lifters or sliders) in the die. Each side action adds $1,500–$4,000 to die cost and increases die complexity. Review every undercut on your design: if it can be eliminated through design change (e.g., converting an undercut groove to a chamfer), do it. If it's functional, the side action is necessary — just understand the cost implication.

11. Achievable Tolerances (Die Casting)

Standard HPDC tolerances (as-cast, without secondary machining): ±0.2mm on most linear dimensions. Features requiring tighter tolerance need secondary CNC machining — bore diameters, bearing bores, sealing surfaces, thread hole locations. Design with this in mind: specify which features are as-cast and which require post-machining. Trying to hold ±0.05mm as-cast from a die is not reliable and leads to sorting costs.

Section 3: Sheet Metal (Items 12–15)

12. Bend Radius

Minimum inside bend radius for sheet metal (laser cut on Amada or Trumpf equipment, formed on press brake): 0.5× material thickness for mild steel and aluminum, 1× thickness for stainless. Specifying a sharper bend than the material allows causes cracking, particularly in work-hardened stainless or 7075 aluminum. For 3mm aluminum: minimum inside radius = 1.5mm. Calling out R0.5 on 3mm aluminum is a common mistake.

13. Hole-to-Edge and Hole-to-Bend Distance

Minimum distance from a hole center to a part edge: 1.5× hole diameter. Minimum distance from a hole to a bend: 2.5× material thickness + bend radius. Violating these minimums causes hole deformation during bending and punching burrs that affect part function.

14. Flat Pattern Feasibility

Sheet metal parts must unfold into a flat pattern that can be cut from standard sheet. Review your part's flat pattern in CAD before sending. Common issue: a part that looks feasible in 3D has a flat pattern that requires cuts through critical features, or has bends that conflict with each other during forming sequence.

15. Sheet Metal Tolerances

Standard laser cut tolerance: ±0.1mm on cutout dimensions. Press brake bend angle: ±0.5°. Overall length/width after bending: ±0.3mm. Calling out ±0.05mm on a bent sheet metal part is not achievable without fixturing and secondary operations — and usually unnecessary. If tight tolerances are required on specific features (hole pattern for assembly, for example), call those out specifically rather than applying tight tolerances globally.

Section 4: Injection Molding (Items 16–20)

16. Wall Thickness Uniformity

Injection molded parts should have uniform wall thickness throughout — ideally within ±25% of nominal. Thick-to-thin transitions cause sink marks, warpage, and fill issues. Design rule: nominal wall 2.5–4mm for most structural plastic parts; if you need thicker sections for strength, use ribs (0.6× nominal wall thickness, height ≤ 3× nominal wall) rather than solid thick sections.

17. Draft Angles (Injection Molding)

Minimum draft for injection molding: 1° per side for smooth surfaces, 1.5° for lightly textured, 3–5° for heavily textured or deeply grained surfaces. Draft enables part ejection without drag marks or stick. A common mistake: designing snap-fit features with no draft on the cantilever arm — this causes tearing on ejection and flash on the mold side.

18. Gate Location

The gate (where plastic enters the mold) leaves a small vestige on the part. Gate location should be specified or approved by the buyer — placing it on a cosmetic face or functional seating surface is a common mistake that requires expensive mold modification. Discuss gate location with the tooling supplier before mold build begins.

19. Plastic Material Selection

Materials readily available in Vietnam for injection molding: PP, ABS, PC, HDPE, LDPE, Nylon 6, Nylon 66, POM (Delrin-equivalent), TPU, TPE. Specialty materials (PEEK, PPS, LCP, PEI/Ultem) require import and have longer material lead times. If your application permits a standard material, confirm that your tolerance and mechanical requirements are actually met — PEEK is sometimes specified "to be safe" when PC or Nylon 66 is perfectly adequate.

20. Achievable Tolerances (Injection Molding)

Standard injection molding tolerance (PP, ABS, PC): ±0.2mm on most linear dimensions. Tight tolerance: ±0.1mm with careful process control and SPC monitoring. Holding ±0.05mm on injection molded plastic is possible on small, rigid, amorphous materials (PC, ABS) with well-tuned tooling and process — but it's premium territory and requires Mitutoyo CMM verification. Semi-crystalline plastics (PP, Nylon, POM) have higher shrink variability and are harder to hold tight tolerances on.

Quick Reference: Process Limits