A plastic part is moldable when fifteen specific features are inside process limits, and the five that cause most tooling rework are wall thickness, draft angle, rib-to-wall ratio, corner radius and undercut direction. SkillsProto reviews every submitted model against this list and returns annotated DFM feedback inside 24 hours, before aluminium tooling at 7-10 days or steel tooling at 15-25 days is committed, because a change on a drawing costs nothing and a change after the cavity is cut costs a re-cut.

Why DFM happens before the tool, not after
A molded part has two designs: the one on the screen and the one the tool can actually produce. The gap between them is not a matter of skill, it is a matter of physics — polymer shrinks as it cools, and it shrinks unevenly wherever the section changes.
Every item on this list is a way of controlling that shrinkage or of letting the tool release the part. None of them are aesthetic preferences. A part that ignores them will still fill, and will still eject, but it will do so with sink marks, warp, short shots or a tool that needs hand-fettling on every cycle.
The economics are asymmetric. Changing a wall from 3.5 mm to 2.5 mm takes ten minutes in CAD. Discovering the same problem in T1 samples costs 1-2 weeks and a tool modification, and discovering it in production costs the tool plus the scrap.
The checklist, with the numbers
| # | Check | Target | What happens if missed |
|---|---|---|---|
| 1 | Nominal wall thickness | 1.5-2.5 mm (ABS, PP, PC/ABS) | Sink marks, long cycle, warp |
| 2 | Wall uniformity | Within 25% of nominal | Differential shrink, warp |
| 3 | Draft on vertical walls | 1-2° minimum, 0.5° absolute floor | Scuffing, ejection damage, white marks |
| 4 | Rib thickness | 50-60% of nominal wall | Sink line on the opposite face |
| 5 | Rib height to thickness | Max 3:1 per rib | Rib freezes before cavity fills |
| 6 | Corner radius, internal | At least 0.5x wall thickness | Stress concentration, crack initiation |
| 7 | Corner radius, external | At least 1.0x wall thickness | Tool corner breaks down, sharp edge |
| 8 | Boss wall thickness | 60% of nominal wall | Sink ring around the boss |
| 9 | Boss stand-off | Gap to mating wall, 0.25 mm min | Boss becomes a sink, doubles wall |
| 10 | Undercuts | None in the parting direction | Slider or lifter, tool cost +30-60% |
| 11 | Gate location | Thickest section, hidden face | Weld lines in visible areas, jetting |
| 12 | Ejector pin placement | Flat, non-cosmetic surfaces | Visible pin marks on class A faces |
| 13 | Tolerances | ±0.05-0.1 mm process capability | Quote includes 100% inspection |
| 14 | Material shrink allowance | 0.4-0.8% unfilled, 0.2-0.5% filled | Dimensions off nominal, tool re-cut |
| 15 | Threads and inserts | Molded-in or post-installed, not both | Split responsibility, assembly failure |
The five that cause most rework
Wall thickness first. It sets cooling time, and cooling is 60-70% of the cycle. A 3.5 mm wall in ABS takes roughly three times as long to cool as a 2.5 mm wall, and it also produces a sink mark on the opposite face because the core shrinks away from the cavity. Most consumer electronics housings end up between 1.5 and 2.5 mm, not because that is strong enough, but because that is where the cycle time and the surface finish both work.
Draft angle second. Steel cannot slide against a vertical wall without scuffing it. One to two degrees per side is the normal specification, and 0.5° is the absolute floor for a textured or deeply ribbed wall. The cost of forgetting draft is not a failed part, it is a part with white stress marks and a tool that needs polishing every few thousand shots.
Rib-to-wall ratio third. A rib at full wall thickness creates a local mass twice the nominal section, which sinks the opposite face. At 50-60% of wall thickness the sink becomes invisible on most surfaces, and the rib still carries most of the bending stiffness the designer wanted. Ribs taller than three times their thickness tend to freeze before the cavity fills, producing short shots at the far end.
Undercuts fourth. Every undercut that cannot be released in the parting direction needs a slider, a lifter or a split cavity. Those add 30-60% to tool cost and add a wear item to the tool. Many undercuts disappear when the parting line is moved, which is a decision to make in CAD, not in the tool shop.
Tolerance fifth. Molding is not a precision process in the way machining is. Parts hold roughly ±0.05-0.1 mm on dimensions that are not affected by shrinkage across a flow path, and the tolerance band widens with distance from the gate and with glass-fibre content. A drawing calling ±0.02 mm on a molded feature will be quoted with a caveat, and the caveat is real.
Where molding ends and machining begins
A part that fails three or more of the geometry checks is usually cheaper as a machined prototype, at least for the first revision. CNC holds ±0.005 mm on critical features, needs no draft, and has no wall-thickness constraint — so the design can be tested before the geometry is frozen for tooling.
That is the practical sequence for most new products: machine 1-10 parts in 3-7 days, test, then cut aluminium tooling in 7-10 days with the geometry already validated. SkillsProto quotes both routes from the same STEP file so the comparison is on identical geometry.
The checks that only matter at volume
Three items on the list cost nothing at prototype quantity and everything at 100,000:
- Cooling channel layout. A conformal or baffled layout can cut cycle time 20-30%, but only pays after tens of thousands of shots.
- Hot runner versus cold runner. A hot runner adds €2,000-€8,000 to the tool and eliminates sprue regrind; it pays above roughly 10,000 parts or where the resin is expensive.
- Ejector and lifter wear. At prototype volume a lifter can be hand-fitted; at production volume it needs a hardened insert and a maintenance interval.
What to send for a DFM review
A STEP or IGES file at final geometry, the resin grade, the cosmetic requirement per surface, and the annual volume. That is enough to run all fifteen checks and to flag which ones affect tool cost rather than part function.
SkillsProto returns annotated DFM feedback within 24 hours, with the failing checks marked on the model and the cost consequence of each, then a priced quote for aluminium tooling at 7-10 days or steel at 15-25 days. MOQ is 1 on the machined prototype that usually comes first.
Upload the model at /quote/ and ask for the DFM report with the quote, not after it. The list above is the same one the review uses.
Frequently Asked Questions
What is the minimum draft angle for an injection molded part?
1-2° per side is standard, and 0.5° is the absolute floor for smooth walls. Textured surfaces need more: roughly 1.5° extra per 0.025 mm of texture depth, because the texture grips the part as it ejects. Zero draft is possible only on very shallow features with a polished tool, and it is not worth designing for.
How thick should walls be in an injection molded part?
1.5-2.5 mm covers most ABS, PP and PC/ABS parts. Below 1.2 mm the flow front can freeze before the cavity fills, especially with glass-filled resins; above 3 mm cooling time rises steeply and sink marks appear on the opposite face. The important rule is uniformity: hold every section within about 25% of the nominal wall.
Can injection molding hold ±0.005 mm tolerances?
No. Molding process capability is roughly ±0.05-0.1 mm on dimensions not affected by flow length, and the band widens with distance from the gate and with fibre content. ±0.005 mm belongs to CNC machining, which is why tight features on a molded part are often machined in a secondary operation rather than molded.
Do ribs cause sink marks?
Ribs at full wall thickness do. A rib at 50-60% of the nominal wall thickness usually stays invisible on the opposite face while still carrying the bending stiffness. Ribs also need draft and a rounded root; a square root concentrates stress and can crack under ejection.
What is the most expensive DFM mistake?
An undercut that needs a slider. It adds 30-60% to tool cost, adds a wear item, and often extends the tool build by a week. Most undercuts can be removed by moving the parting line or by adding a small side action in the part design instead of the tool, and both are free to change before the cavity is cut.
How fast can a DFM review and quote be delivered?
Within 24 hours of receiving a STEP file, the resin grade and the annual volume. The review covers the fifteen checks above with the failures annotated on the model. If the part also needs a machined prototype, SkillsProto ships those in 3-7 days while the tooling decision is being made.
Related capabilities
Related guides
Have parts to quote?
Upload your files — DFM-checked quotation within 24 hours.
