Injection Molding Draft Angle: Rules by Material, Depth and Texture
Last Updated: October 31, 2026
Answer Capsule: Injection molding draft angle is the taper on every wall parallel to the mold’s pull direction so the part releases cleanly. Start at 1 degree per side on smooth walls, use at least 0.5 degree on ribs and bosses, add about 1 degree per inch of depth, and give textured surfaces 3 degrees or more.
Your CAD model has perfectly vertical walls, because that is how you drew it. The mold builder will not cut it that way. If they do, the first parts come out scuffed, bent, or stuck on the core. Every one of those outcomes is a draft angle problem, and every one is cheaper to fix in CAD than in steel.
Missing draft is the single most common DFM comment Legacy Molding writes. It shows up on ribs, bosses, molded text and shut-offs far more often than on the main walls. Adding it late means re-quoting the tool and sometimes re-dimensioning the part.
This guide gives you the injection molding draft angle rules by feature, depth, surface finish and material, with the numbers a mold builder will use. It also covers where draft hides, what zero draft costs, and how a DFM review from Brent Hanke’s team catches it before tooling starts.
What is draft angle in injection molding?
Draft angle is the small taper added to any part surface that runs parallel to the direction the mold opens, so the part can slide off the core and out of the cavity. It is measured in degrees from that pull direction. A 1 degree draft on a 1 in tall wall moves the top of that wall about 0.017 in relative to the bottom.
Draft goes in both directions. Outside walls taper inward toward the top of the part so the cavity can pull away. Inside walls and holes taper outward so the core can withdraw. If you draft one and forget the other, the part will hang on the core.
Think of a bucket. The sides lean in slightly, which is why one bucket pulls out of another. A part with no draft is two straight-sided buckets, and the plastic has shrunk onto the inner one.
Why does a molded part need draft?
A molded part needs draft because plastic shrinks as it cools and grips the core, and the ejector pins then have to push the part off that grip. Without taper, the ejection force rises, the surface drags along the steel, and the part or the tool pays for it.
The failure modes, in the order you will see them:
- Drag marks and scuffing. Lines parallel to the pull direction on cosmetic walls. On a textured surface, the texture is wiped off.
- Ejector pin push-through. The pins leave deep witness marks or punch into the part because the part will not let go.
- Warp and distortion. The part is pulled off while still soft and bends at the ribs.
- Stuck parts and damaged steel. The cycle stops, someone pries the part off, and the cavity gets scratched.
- Longer cycles. The molder cools the part longer so it is stiff enough to survive ejection, which raises your part price.
Draft is not a cosmetic nicety. It sets the ejection force, which sets the cooling time, which sets the cycle, which sets the per-part cost.
How much draft angle do you need?
Most parts need 1 degree per side on smooth walls, 0.5 to 1 degree on ribs and bosses, and 3 degrees or more on textured surfaces. Add about 1 degree per inch of depth on tall features. These are starting points, and the mold builder or the texture house may ask for more.
| Feature or surface | Minimum draft per side | Preferred draft | Notes |
|---|---|---|---|
| Smooth outside wall, polished | 0.5 degree | 1 to 2 degrees | Deeper walls need more |
| Smooth inside wall or core | 1 degree | 1 to 2 degrees | Plastic shrinks onto cores, so err high |
| Rib | 0.5 degree | 1 degree | Taper thins the rib tip, see wall thickness rules |
| Boss (inside and outside) | 0.5 degree | 1 degree | Deep screw bosses need more |
| Molded text or logo | 0.5 degree | 1 degree or more | Raised text drafts easier than recessed |
| Shut-off face (bypass core) | 3 degrees | 5 degrees | Ask your mold builder |
| Light texture (about 0.001 in deep) | 1.5 degrees | 3 degrees | Texture house will specify |
| Heavy texture (0.002 to 0.003 in deep) | 3 degrees | 5 degrees or more | Add about 1.5 degrees per 0.001 in of depth |
The depth rule. A common rule of thumb is 1 degree per inch of draw. A 3 in deep housing wall that starts at 1 degree should end up closer to 3 degrees on the cosmetic outside surface. On the inside, where the core grips, give it at least as much.
The texture rule. Texture is cut into the steel as tiny pits, and the part has to clear those pits before it can slide. Texture houses commonly ask for about 1.5 degrees of draft for every 0.001 in of texture depth. Get the pattern number and its draft requirement before you freeze the walls.
The injection molding design guide puts these draft numbers next to the wall, rib and boss rules so you can check a part in one pass.
Does draft angle change by material?
Yes. Rigid, low-shrink amorphous resins release with the least draft, high-heat and soft materials need more, and semi-crystalline resins grip cores harder because they shrink more. Material changes the minimum, not the rules above.
Covestro’s part and mold design guide gives material-specific numbers for its own resins. Its polycarbonate and PC/ABS blends need at least 1 degree of draft for easy ejection. Its high-heat polycarbonate ejects best with 3 degrees or more. Its TPU grades need at least 5 degrees plus a slightly roughened mold surface, and those figures are a fair guide for the same families from any supplier.
Rules of thumb by family:
- ABS, PC, PC/ABS, acrylic. 1 degree works on most walls. These amorphous resins shrink little and release well.
- Polypropylene, HDPE, acetal, nylon. Semi-crystalline, higher shrink, grip cores harder. Keep 1 degree minimum and go higher on deep cores.
- Glass-filled grades. Stiffer and lower shrink in the flow direction, but abrasive. Draft reduces wear on the steel as well as on the part.
- TPE and TPU. Soft materials drag and stretch during ejection. Plan on 3 to 5 degrees and talk to the molder about the mold surface.
Ask your molder for the resin’s published shrink rate before you lock the draft. Legacy Molding runs 50 or more resins and knows which ones fight deep cores.
Where is draft most often missed?
Draft is most often missed on ribs, bosses, molded text, shut-off faces and the inside of deep pockets. Designers draft the big walls and forget the small features that are just as parallel to the pull direction. Each of those features is a tiny core or cavity of its own.
Here is a DFM review Legacy Molding runs most weeks. A battery housing arrives with clean 1.5 degree draft on the outer walls. Inside, eight screw bosses and a grid of stiffening ribs are perfectly vertical, and the model number is recessed into a flat face with square walls.
Every boss and rib would hang on the core, and the recessed text would chip at the edges. The fix is a few minutes in CAD: 1 degree on each boss and rib, and raised text with 1 degree on the letter walls. The tool quote does not change, and the parts eject at a normal cycle.
The checklist Legacy Molding uses:
- Ribs. Draft both sides. Keep the base at 50 to 60 percent of the wall and let the taper thin the tip. The wall thickness, rib and boss rules show how draft and rib thickness interact.
- Bosses. Draft the outside and the hole. Core the boss so the wall stays thin, then draft that core.
- Text and logos. Raised text, 1 degree or more on the letter walls, and a rounded letter face.
- Shut-offs. Any face where the core and cavity steel meet to form a window or a snap-fit needs 3 to 5 degrees, or the steel wears and the part flashes.
- Deep pockets and cores. Inside surfaces need as much draft as outside.
- Textured faces. Confirm the texture depth and add the draft the texture house asks for.
- Parting line. Draft runs away from the parting line in both directions. A wall that crosses the parting line needs draft on each side of it.
How a DFM review catches draft before tooling
A DFM review catches missing draft by checking every surface against the pull direction, not by eyeballing the model. Legacy Molding reviews every part for manufacturability before a tool is designed, and draft is the first item on the list.
You send a STEP, IGES or SolidWorks file, the material, the annual volume, the tolerances, the surface finish, and any texture pattern. In 24 to 48 business hours you get a quote with DFM notes. Those notes list each feature that needs draft, the degrees suggested, and any toleranced dimension the draft would change.
Draft and tolerance meet on tall features. A 1 degree draft moves a wall about 0.0175 in over 1 in of height. If a toleranced dimension sits at the top of a drafted wall, say where it should be measured. Legacy Molding measures first articles with calipers and height gauges, so a clear datum avoids an argument later.
Frequently Asked Questions
Can you injection mold a part with zero draft?
Only on very short features, usually under about 2 mm tall, on polished steel with a rigid low-shrink resin. Even then the tool wears faster and the parts may scuff. Anything taller needs at least 0.5 degree. If a function truly requires a zero-draft face, the mold builder may need a slide or a lifter, which adds cost, so ask before you commit.
Which way does draft angle go on inside and outside walls?
Outside walls taper inward as they rise from the parting line so the cavity can pull away. Inside walls, holes and pockets taper outward so the core can withdraw. Both tapers open toward the direction the part leaves the steel. A part with draft on only one side still sticks.
How much draft angle does a textured surface need?
Plan on 3 degrees for a light texture and 5 degrees or more for a heavy one. The usual rule is about 1.5 degrees of draft for every 0.001 in of texture depth. Get the pattern number from the texture house and ask for its draft requirement before you freeze the walls.
Does draft angle affect part tolerances?
Yes. Draft changes a dimension along the height of the wall, so a 1 degree taper shifts a 1 in wall by about 0.0175 in from bottom to top. Dimension the part where it will be measured, usually at the parting line or a flat datum face. Call out the draft on the drawing so the mold builder and the inspector read it the same way.
Conclusion
Three takeaways. Start every wall at 1 degree of injection molding draft angle per side, add about 1 degree per inch of depth, and give textured surfaces 3 degrees or more. Ribs, bosses, text and shut-offs are where draft gets missed, so check the small features, not just the big walls. Material shifts the minimum, with soft and high-shrink resins needing more.
Draft added in CAD costs minutes. Draft added in steel costs a re-quote. Legacy Molding reviews every part for draft before a tool is designed, and ships a first article with every new tool so you can see the result measured.
Send your CAD and annual volume for a quote with DFM notes, or call Brent at 480-256-9773.
Sources
- Covestro, Engineering Polymers Part and Mold Design: A Design Guide (PDF): https://solutions.covestro.com/-/media/covestro/solution-center/brands/downloads/imported/1557214249.pdf
Brent Hanke | Legacy Molding | 480-256-9773 | b.hanke@legacy-molding.com
Brent Hanke is the owner of Legacy Molding, a custom plastic injection molder in Phoenix, Arizona, producing parts for OEMs across the Southwest and the country.
Have a part like this to quote?
Send the CAD and annual volume. A Phoenix engineer replies within one business day with pricing and DFM notes.
