Free resource
Injection molding DFM checklist
Nine things worth checking on a plastic part before the STEP file leaves your computer, each one with the number it gets compared against. These are the thresholds the Fabdose analysis engine loads out of its own rule files, so the page also shows you where a geometry check stops being able to help.
One page. No email, no signup.
Six a geometry check can settle
Each of these can be decided from the shape alone, face by face, without knowing anything about your tool or your molder.
1. Draft angle on every face
Two degrees on a smooth surface, three on a textured one. Fabdose compares every face against the two degree figure by default, and skips the faces it has already classified as parting surfaces or undercuts, since neither is supposed to carry draft in the first place.
2. Undercuts, and how expensive each one is
Any face the mold cannot pull away from. The severity band comes from the angle. Under 5 degrees is usually ignorable, 5 to 15 is lifter territory, 15 to 30 normally needs a slide core, and past 30 degrees you are looking at a redesign or a mold technique that shows up on the quote.
3. Wall thickness against the resin you actually picked
Every resin has its own floor and ceiling. ABS bottoms out at 1.14mm, PP at 0.635mm, PEEK at 0.508mm. A 1.0mm wall is comfortable in polypropylene and too thin in ABS, so a check that does not know which resin you chose cannot answer this at all. Full table below.
4. Wall thickness uniformity
Every measured wall should sit within 30 percent of the part's dominant thickness. Dominant, not average: the mean gets dragged around by a handful of small rib and boss faces until the real wall starts looking like the outlier. Ribs deliberately built at 40 to 60 percent of nominal are excluded rather than counted as violations.
5. Flow length ratio
Flow length divided by wall thickness. Above 75 you are in thin wall molding, where filling gets difficult and short shots start appearing. Fabdose approximates flow length with the longest bounding box dimension, which is a rough stand-in for the real melt path and is labelled as an approximation in the report.
6. Shrinkage
Anything whose typical shrinkage runs above 1.5 percent gets a dimensional compensation note. In the resin data Fabdose ships, that is POM at 1.8 percent and PP, which reaches 2.0. ABS at 1.1 and PC/ABS at 0.35 stay quiet.
Three it cannot, so check them yourself
Fabdose carries the numbers below in its rule files and uses them where other checks need them, but on an injection molded part it does not flag ribs, bosses, holes or corner radii from the geometry today. These three are on you.
7. Ribs
40 to 60 percent of the nominal wall, spaced at least three wall thicknesses apart, no taller than three times the wall. Past 60 percent you are designing a sink mark into the visible face on the other side.
8. Bosses
Boss wall at 60 percent of nominal or under. Outside diameter between 2.0 and 2.5 times the inside diameter. Same sink mark logic as a rib, except a boss usually sits somewhere you can see.
9. Holes and internal corners
Hole depth no more than three times the diameter, minimum diameter 0.5mm. Internal corner radius at least 0.5mm, and ideally half the wall thickness. External at least 0.3mm. Sharp internal corners are where stress concentrates and where the melt front slows down.
Wall thickness and shrinkage, by resin
The wall thickness figures are what your part gets compared against. Shrinkage is carried as a note rather than a limit.
| Resin | Min wall | Max wall | Shrinkage |
|---|---|---|---|
| ABS | 1.14 mm | 3.56 mm | 0.7 to 1.6 % |
| PC | 1.016 mm | 3.81 mm | 0.5 to 0.7 % |
| PC/ABS | 1.14 mm | 3.56 mm | 0.2 to 0.5 % |
| PP | 0.635 mm | 3.81 mm | 1.0 to 2.0 % |
| PA | 0.76 mm | 2.92 mm | 0.3 to 1.2 % |
| POM | 0.76 mm | 3.05 mm | 0.4 to 2.0 % |
| PMMA | 0.64 mm | 3.0 mm | 0.2 to 0.5 % |
| PEEK | 0.508 mm | 3.0 mm | 1.0 to 1.7 % |
| TPU | 0.64 mm | 3.0 mm | 1.0 % |
| TPE | 0.64 mm | 3.0 mm | Not available |
Millimetre figures are unrounded because several of them were converted from imperial datasheet values. PC shrinkage is for unfilled grades; glass filled runs lower. TPE varies too much by type for a single number to mean anything.
Where these numbers come from
They are read straight out of the rule files that ship inside the Fabdose desktop app: the injection molding rule set for the process limits, and the materials file for the per-resin figures, which were compiled from resin supplier datasheets. None of it is an average of what other sites publish. If a number here disagrees with your molder, your molder is talking about your tool, your gate and your resin lot, and they win.
Run the first six on your own part
Fabdose reads a STEP file on your computer and names the faces that fail, by face number and by location in the model. The first five analyses are free and it does not ask for a card.