Rules for applying draft to injection molded parts — by surface type, material, and texture depth.
Draft is the taper applied to surfaces parallel to the mold opening direction — typically vertical walls when the mold opens vertically. Without draft, the molded part grips the mold core and cavity as it shrinks during cooling. Ejection requires excessive force, causing surface drag marks, part deformation, or tool damage.
Draft is not a compromise — it is a fundamental requirement of the injection molding process.
The Basic Rule
The minimum draft angle is 1° per side for smooth, non-textured surfaces on most engineering thermoplastics. This means for every 1 mm of wall height, the wall narrows or widens by 0.017 mm on each side. For a 50 mm tall wall, 1° of draft means the base is 1.75 mm wider than the top.
In practice, more draft is always better than less. A draft angle of 2–3° is preferred for production molds where mold life and ease of ejection matter. Reserve 0.5° draft—the practical minimum—only for features where geometry prevents more.
Key Draft Guideline
Use at least 1° of draft per side for smooth, non-textured surfaces. Where the part geometry allows it, increasing the draft to 2–3° improves ejection, reduces surface damage, and supports longer mold life.
Draft by Surface Type
The required draft angle depends heavily on the surface finish, texture depth, and feature geometry. Textured surfaces generally require substantially more draft than smooth surfaces because the molded material must release cleanly from the texture pattern.
| Surface Type | Recommended Draft |
|---|---|
| Smooth, non-cosmetic | 1° minimum per side — the baseline for all draft calculations |
| Cosmetic / appearance | 1.5–2° — polished surfaces grip the mold more than textured surfaces; extra draft prevents drag marks |
| Lightly textured (< 15 μm) | 3° minimum — texture depth requires proportionally more draft to release without destroying the pattern |
| Standard texture (15–25 μm) | 3–4° — Mold-Tech standard leather patterns require 3° minimum |
| Heavy texture (25–50 μm) | 5° minimum — coarse grain and embossed patterns require aggressive draft to release |
| Very coarse (> 50 μm) | 6–8° — deep texture patterns may require negotiation with the mold builder |
| Inside rib walls | 0.5–1° per side — ribs have short depth relative to width, so less draft is acceptable |
| Deep core features | 2–3° — long, slender core pins require more draft to prevent galling and sticking |
Draft by Material
Some materials require more draft than others due to their shrinkage and surface characteristics:
| Material | Recommended Draft and Considerations |
|---|---|
| Polypropylene (PP) | High crystalline shrinkage of 1.5–2.0% grips cores aggressively — 2° minimum recommended for tall walls |
| ABS | 1° draft is generally adequate — low shrinkage and good release |
| Polycarbonate | 1–1.5° — moderate shrinkage, but polished PC surfaces tend to stick more than matte surfaces |
| Nylon (PA 6/6) | 1.5° minimum — moderate-to-high shrinkage and semi-crystalline surfaces can grip smooth cores |
| POM (Delrin) | 2° minimum — high crystalline shrinkage and a semi-crystalline surface make draft especially important |
| PEEK / PEI | 1–2° — high mold-temperature processing requires careful draft for clean release |
| TPE / TPU | 0.5° minimum — flexible materials strip from low-draft features more easily than rigid resins |
Common Draft Design Errors
- Zero draft on side walls: This typically occurs when engineers design in CAD without considering the mold opening direction. All walls must be reviewed from the pull direction.
- Insufficient draft on textured surfaces: This is the most common source of texture damage during ejection. Always obtain the specified texture depth before finalizing draft angles.
- Inconsistent draft direction: Walls drafted in the wrong direction, narrowing toward the core, create locked features that cannot eject. Every drafted surface must taper to allow release.
- Draft on shutoff surfaces: Surfaces that contact the opposite mold half must seal flush. Applying draft to these shutoff surfaces can create flash.
Texture Design Warning
Do not finalize draft angles before the surface texture has been specified. The deeper the texture, the more draft the surface requires to release without drag marks or damage to the pattern.
How to Apply Draft in CAD
Draft should be applied after the nominal geometry is defined, as the final step before checking the part for moldability. Best practices include:
- Establish the parting direction first: The parting direction determines which surfaces require draft.
- Apply draft from the parting surface outward: Walls should taper from the parting line toward the core and cavity.
- Use the CAD draft-analysis tool: Verify draft across all surfaces before sending the design to the injection molder.
- Flag restricted features: Identify any features where 1° of draft cannot be achieved so they can be reviewed with the mold builder.
Frequently Asked Questions
What happens if there is no draft on an injection molded part?
Without draft, the part grips the mold core during ejection. At minimum, this causes surface drag marks on the part—scratches parallel to the ejection direction. In more severe cases, ejector pins push through the part, the part deforms during ejection, or the mold surface is damaged. For production tooling, zero-draft features cause tooling-maintenance problems and shorten tool life.
Can injection molded parts have zero draft?
Theoretically, zero draft may be possible for very short features under 2 mm tall on polished molds using rigid, low-shrinkage materials. In practice, even short features benefit from 0.5° of draft. Features over 5 mm tall should always have at least 1°. Consult the injection molder about any feature where draft cannot be achieved. In some cases, the mold design can compensate through polished shutoffs or stripper plates.
