Design for injection molding is a set of rules that protect three physical events: the cavity fills, the part cools, and the part ejects. Every rule in this guide exists because a specific failure mode appears when the rule is broken, so each section states the failure, the design standard, and a counterexample. Review the geometry against these rules before the mold is approved, because a change on the CAD file costs hours, while a change in steel costs weeks and thousands of dollars.
Wall Thickness: The Rule Everything Else Depends On
Failure mode: molten plastic flows fastest through thick sections and cools slowest there, so a part with a 1 mm wall next to a 4 mm wall fills unevenly, shrinks unevenly, and warps. The visible results are sinks, short shots, and internal stress that appears after ejection.
Design standard: keep the wall uniform, within a range the material handles comfortably. For many engineering thermoplastics that range is roughly 1–4 mm, but the practical range depends on the material's flow length, the part size, and the gate strategy, so treat the number as a starting point for the DFM conversation, not a fixed limit. Where the geometry needs a transition between thicknesses, make it gradual instead of a step.
Counterexample: a boss and a flat wall sharing one surface with no transition. The thick boss cools last, sinks at its root, and pulls the adjacent wall out of flatness. The corrected design cores the boss out from the back or moves the material into a rib.
Wall thickness also sets the flow length and the gate strategy. A long, thin part needs a gate location that fills the cavity before the material freezes, and the injection molding supplier should confirm the material's flow length for your wall thickness during the DFM review.
Draft: The Angle That Lets the Part Leave the Mold
Failure mode: without a slight taper on vertical faces, the part sticks in the cavity, the ejector marks the surface, or the mold wears prematurely. The failure is not always immediate; it shows up as cosmetic drag marks or inconsistent ejection on later cycles.
Design standard: apply 1–2 degrees of draft on vertical faces as a general starting point. Deep ribs and bosses need more draft because they grip the mold over a longer distance, and textured surfaces need extra draft, roughly 1 degree per 0.025 mm of texture depth, so the texture does not lock the part in the cavity. The exact values depend on material, texture, and part depth, so confirm them with the supplier.
Counterexample: a cosmetic face with a fine texture and zero draft. The part releases with visible drag marks or requires increasing ejection force that risks cracking thin bosses. Mark which faces are cosmetic and which can carry draft on the drawing, because the supplier can suggest values, but the design team should approve the ones that affect appearance or fit.
Ribs, Bosses, and Strength Without Thick Sections
Failure mode: wherever the design wants a thick block, the block sinks, warps, and takes longer to cool. A solid, oversized boss around a screw hole looks strong but sinks at its root, and a thick rib junction creates a local hot spot that shrinks unevenly.
Design standard: use ribs to add stiffness at controlled thickness. A rib base should be about 50–80% of the wall thickness, with a radius at the root, so the junction does not become a thick section. Bosses for screws should keep the boss wall close to the nominal wall, and gussets can stiffen tall bosses without adding mass.
Counterexample: a rib that is 120% of the wall thickness with a sharp root. The junction is thicker than the surrounding wall, so it sinks visibly on the opposite surface. The corrected design reduces the rib base, adds a root radius, and keeps the thickness ratio inside the material's acceptable range.
Radii, Flow, and Internal Corners
Failure mode: sharp internal corners concentrate stress and restrict flow. In brittle materials they crack under load; in filling terms they make the flow front hesitate and can create visible knit lines or short shots at the corner.
Design standard: add an internal corner radius of at least 25–50% of the wall thickness. External corners can stay sharper, but every radius added to the internal side improves both strength and filling. Review holes, ribs, and bosses as flow obstacles, and choose the gate location against the full feature map, not as an afterthought.
Counterexample: a sharp internal corner at a load-bearing bracket root. The part survives first assembly but cracks under repeated load because the radius was omitted. The corrected geometry adds a root radius equal to about half the wall thickness.
Gates, Weld Lines, and Cosmetic Surfaces
Failure mode: the gate leaves a vestige where the part was separated from the runner, and weld lines form where flow fronts meet around holes or bosses. A gate on a visible surface leaves a permanent mark, and a weld line on a load-bearing section is a structural weak point.
Design standard: mark cosmetic surfaces on the drawing and agree where gates are acceptable in the tooling review. Place weld lines away from load-bearing sections or hide them with a design detail, and specify what gate vestige is acceptable on the final part. Plan for the trimming cost if the gate must be cut or sanded.
Counterexample: a gate placed on the front cosmetic face because it gave the shortest flow path. The vestige requires hand finishing on every part, and the cost appears in every batch. The corrected design moves the gate to a hidden face and accepts a slightly longer flow path.
Shrinkage, Tolerances, and Material Grade
Plastic shrinks as it cools, and the amount depends on the material family, the wall thickness, and the processing conditions. The mold is cut oversized by the expected shrink rate, so the tolerance scheme must be realistic for the chosen grade.
| Material family | Shrink behavior | Tolerance caution |
|---|---|---|
| Amorphous (ABS, PC) | Lower, more predictable shrink | Stable dimensions, but sensitive to packing pressure |
| Semi-crystalline (PA, POM) | Higher, grade-dependent shrink | Dimensional change after molding and moisture absorption |
| Filled or reinforced grades | Lower overall shrink, anisotropic | Directional behavior; gate and fill direction affect dimensions |
Confirm the material grade before the mold design is finalized, because shrinkage data and mechanical properties belong to the grade, not the family. Changing from one nylon to another after the mold is cut can move the parts out of tolerance. Mold temperature and packing pressure also shift the result: a part molded with high packing shrinks less, while a part molded at the edge of the process window can vary between batches, so the supplier's process control is part of the tolerance story.
Design Traps
- Thicker walls are stronger. Within the material's range, yes, but thick sections sink and warp. Ribs achieve stiffness without the defects.
- Draft is optional on small parts. Even small parts stick without draft. The angle is part of the geometry, not a mold trick.
- The mold fixes everything. A mold faithfully reproduces the design. Fill, cooling, and ejection problems start on the drawing.
- Any plastic will work. Shrinkage, flow, and warpage differ by grade, so the material decision belongs in the design phase, not after the mold is built.
DFM Review Checklist
Run this list on the drawing before requesting tooling quotes, and attach the answers to the DFM package so the supplier can focus on the remaining risks.
- Wall thickness uniform and within the material's practical range
- Thickness transitions gradual, not stepped
- Draft applied to all vertical faces, including ribs and bosses
- Textured surfaces have extra draft proportional to texture depth
- Rib bases at 50–80% of wall thickness with root radii
- Boss walls near nominal thickness, gussets for tall bosses
- Internal corner radii at least 25–50% of wall thickness
- Cosmetic surfaces marked and gate location agreed
- Weld lines placed away from load-bearing sections
- Material grade and shrink rate confirmed before mold design
- Tolerance scheme realistic for the material family
6CProto Engineering Team
Review the drawing as if you were watching the plastic fill it. Uniform walls fill evenly, draft releases cleanly, ribs add stiffness without sinks, and internal radii keep the flow moving. We run this checklist with customers before steel is cut, because the geometry that fills, cools, and ejects reliably on paper is the geometry that runs reliably in production.
Conclusion
The DFM rules protect fill, cooling, and ejection: uniform walls, draft on vertical faces, ribs instead of thick sections, radii at internal corners, and a gate strategy that respects cosmetic surfaces. Confirm the material grade and shrink rate before the mold is approved, then let the DFM review check the geometry against the material. The review checklist at the end of this guide is the fastest way to find the expensive mistakes while they are still free to fix.
FAQs
What wall thickness should I use for injection molded parts?
For many engineering thermoplastics, roughly 1–4 mm is a practical range, but the right value depends on the material's flow length, the part size, and the gate strategy. Keep the wall uniform and confirm the range with the supplier during DFM.
How much draft is needed on a molded part?
One to two degrees on vertical faces is a common starting point, with more on deep ribs and bosses and extra draft on textured surfaces. The exact values depend on material, depth, and texture, so confirm them for your geometry.
Why do thick sections cause sinks and warpage?
Thick sections cool and shrink more slowly than the surrounding material, so the surface sinks and the part bows as different areas shrink at different rates. Ribs, webs, and controlled-thickness bosses add stiffness without creating the thick section.
When should I confirm the material grade and shrinkage data?
Before the mold is cut. Shrinkage and mechanical properties belong to the specific grade, not the material family, and switching grades after the mold is cut can move parts out of tolerance. Confirm grade, shrink rate, and process window in the same conversation.
Sources
- 6CProto Injection Molding Services
- 6CProto Plastic Injection Molding
- 6CProto Standards and Tolerances
- ISO 2768-1:1989 – General tolerances for linear and angular dimensions
- ISO 9001:2015 – Quality management systems