Most injection molding projects fail quietly. The part ejects, the dimensions look right, and nobody notices the problem until month three of production: cycle times have crept up, one cosmetic zone shows witness marks, and the scrap rate will not go below two percent. Almost every one of those failures traces back to a design decision made before a single piece of steel was cut.
Design for Manufacturing (DFM) is the discipline of reviewing part geometry against the realities of the injection molding process while changes are still free. This checklist covers the eight factors that decide tooling cost, cycle time and part quality, the same list a competent mold designer runs before quoting your tool.
1. Why DFM Happens Before Steel, Not After
The economics are brutal and simple: a geometry change costs almost nothing on a CAD model and roughly 10x more once the cavity is machined. A change made after heat treatment can mean re-machining, re-polishing, re-texturing and a second T1 trial, two to three weeks and a five-figure rework bill for something that was an afternoon of CAD work during design review.
Professional mold design follows a fixed sequence: part review → mold flow simulation → 3D mold design → machining → T1 trial → corrections → production. DFM belongs at step one. Mold flow simulation (Moldflow or equivalent) fills the cavity virtually, so gate location, fill balance, weld line positions, air traps and cooling performance are all validated on screen before they cost anything.
2. Wall Thickness: The Single Biggest Cost Driver
Injection molding punishes wall thickness mistakes twice, once in the mold, once in the part. The governing principle is uniformity, not thinness.
- Keep all walls within ±25% of nominal thickness. Transitions should be gradual (tapered, not stepped) so melt flows smoothly without hesitation or over-pack.
- Typical production windows: ABS 1.5–2.5 mm; PC 1.5–2.5 mm; PP 1.2–2.0 mm; PA6/PA66 1.5–3.0 mm; glass-filled grades sit slightly higher.
- Too thin causes short shots, poor fill in long flow paths and brittle knit lines. Too thick causes sink marks, internal voids, longer cycles and higher material cost per shot.
- Need more strength? Add a rib, not thickness. A rib at roughly 60% of the adjacent wall thickness adds stiffness with minimal sink risk. Thick bosses are the classic sink-mark generator, core them out or use a gab between ribs instead.
- Unavoidable thick sections should be cored out from the inside, bringing the effective wall back in line with the rest of the part.
| Material | Typical Wall (mm) | Common Trap |
|---|---|---|
| ABS (e.g. PA-757) | 1.5 – 2.5 | Thick bosses behind cosmetic surfaces → sink marks |
| PC | 1.5 – 2.5 | Sharp corners at stress points → crack initiation |
| PP | 1.2 – 2.0 | Living hinges need controlled thinness, not uniform thinness |
| PA6 / PA66 | 1.5 – 3.0 | Moisture → streaks and hydrolysis; dry before molding |
| PA6-GF30 (glass-filled) | 1.5 – 3.0 | Anisotropic shrinkage → warpage on flat plates |
| POM | 1.5 – 3.0 | Gas evolution → venting critical |
3. Draft Angles: The Requirement That Hides Until Production
Draft (taper on vertical faces) is what lets the part release from the cavity and core without dragging. It never shows up as a dimensional error on a first-article report, it shows up as scuffing, ejection damage and rising ejection force once you are running thousands of shots.
- Baseline: 1° per side on untextured vertical faces.
- Textured surfaces: +1.5° per 0.025 mm of texture depth. A VDI 27 texture (about 0.025 mm) needs roughly 2.5° total draft.
- Deep draws, glossy cosmetic surfaces and filled resins push requirements higher, evaluate per surface, not per part.
- Draft is cheaper than ejection hardware. Adding 1° of draft costs nothing in function; compensating for its absence with stripper plates and air poppets adds mold cost and maintenance.
4. Gate Location and Runner Strategy
The gate is where melt enters the cavity, and its position determines fill pattern, weld line locations, air trap positions and how the part packs out during holding. Gate design is a joint decision: the part designer knows where cosmetics and loads matter; the mold designer knows how melt behaves.
- Fill thick-to-thin. Gates should feed the thickest sections first so thinner sections fill last under full holding pressure.
- Keep weld lines out of cosmetic and load-bearing zones. Weld line strength is always lower than the base material; position matters more than process tuning.
- Choose gate type by part and automation needs: edge gates for most parts; submarine (tunnel) gates for automatic degating; pin-point gates for 3-plate tools; valve gates for large or multi-cavity tools needing sequential fill control.
- Balance the runner. In multi-cavity tools, every cavity must fill at the same moment and pressure, an unbalanced runner means one cavity short-shots while another flashes.
5. Cooling Design: Where Cycle Time Is Won or Lost
Cooling typically accounts for 60–80% of total cycle time. A mold that cools unevenly produces parts that are dimensionally different from shot 1 to shot 10,000, and dimensional drift is the defect customers notice last and complain about loudest.
- Channel geometry: 6–12 mm diameter circuits, positioned about 1.5–2 channel diameters from the cavity surface, spaced 2.5–3 diameters apart center-to-center.
- Uniformity beats volume. A few well-placed circuits outperform a maze of poorly placed ones. The goal is the same heat extraction rate everywhere.
- Hot spots need special hardware. Deep cores and thin ribs cannot be cooled conventionally, beryllium copper inserts (3–4x the thermal conductivity of tool steel) solve them.
- Measure the payoff. Aggressive, well-designed cooling routinely cuts cycle time 15–30% on typical parts; on thick-wall parts the saving is larger.
6. Ejection Strategy
How the part leaves the mold determines witness marks, deformation risk and long-term mold maintenance.
- Default to ejector pins on non-cosmetic surfaces, simple, cheap, maintainable.
- Cosmetic surfaces call for stripper plates, sleeve ejectors or air poppets to avoid pin witness marks.
- Undercuts should be released by lifters, slides or collapsible cores rather than by force-stripping the part.
- Plan ejection early. Ejection layout drives core/cavity layout; retrofitting it after machining is expensive.
7. Corner Radii and Material Flow
Sharp internal corners concentrate stress and interrupt melt flow, the two fastest routes to field failure. Specify radii generously: they cost nothing in function, improve fill, reduce residual stress and extend mold life. Where sharp corners are functionally required (sealing edges, electrical contact points), call them out explicitly so the mold designer does not "fix" them.
8. The T1 Trial Checklist
T1 (the first samples from a completed mold), is where design quality becomes visible. Run the first trial against this checklist, not against hope:
- Dimensional report on all critical features (CMM or equivalent), not just a few caliper checks
- Short-shot study to confirm fill pattern and gate balance across cavities
- Weld line locations photographed and compared against the design review agreement
- Cosmetic surfaces inspected under production lighting for sink, flow marks and witness marks
- Cycle time recorded with target cooling achieved (not the "best case" of a cold mold)
- Ejection verified over a continuous run, no drag, no deformation, stable ejection force
- Shrinkage data from measured samples fed back into the design for any needed cavity correction
Putting It Together: The Quick Reference
| Design Factor | Target / Rule |
|---|---|
| Wall uniformity | Within ±25% of nominal; tapered transitions |
| Wall thickness (ABS/PC) | 1.5–2.5 mm typical production window |
| Ribs | ~60% of adjacent wall thickness |
| Draft angle | ≥1°/side; +1.5° per 0.025 mm texture depth |
| Cooling channel | 6–12 mm dia, 1.5–2 dia from cavity, 2.5–3 dia spacing |
| Gate strategy | Fill thick-to-thin; weld lines off cosmetic/load zones |
| Corner radii | Generous unless functionally sharp |
| Ejection | Pins off-cosmetic; stripper/air for cosmetic surfaces |
None of these rules are exotic. What separates good mold projects from expensive ones is whether somebody ran this list before the steel was ordered. If your part is heading toward tooling and nobody has done this review yet, that is the cheapest conversation you can have this quarter, send the geometry over and get the report before the cutter starts.