Zero-draft walls are technically possible. They also guarantee ejection problems, surface damage, and production headaches that dwarf the appearance benefit of perfectly vertical walls. Draft is the slight angle added to surfaces parallel to the mold opening direction, allowing parts to release cleanly from cores and cavities. Understanding why draft is necessary and how much specific applications require prevents design conflicts that delay projects and compromise part quality.
Why Parts Need Draft
Three physical phenomena make draft essential: shrinkage grip, vacuum adhesion, and ejection force mechanics.
Shrinkage onto cores is the primary driver of draft requirements. As plastic cools and solidifies, it contracts. This shrinkage pulls the part tightly against any male features (cores) it surrounds. Without draft, the part grips the core with friction proportional to the contact area and shrinkage force. Ejection must overcome this friction, requiring either excessive force (risking part damage) or extended cooling (wasting cycle time).
With draft, the part begins releasing from the core as soon as it moves. The angled surface creates clearance immediately, dramatically reducing the ejection force required. Even small draft angles create significant clearance over the length of a feature.
Vacuum effects occur between flat surfaces and polished mold faces. When the part contacts the cavity surface over its entire area, opening the mold creates a vacuum. Air cannot enter between the surfaces to equalize pressure. This vacuum resists part release. Draft and surface texture break up the vacuum, allowing air infiltration during mold opening.
Ejection force mechanics concentrate stress when draft is insufficient. Ejector pins pushing against a part that won’t release create localized stress concentrations. The part may distort, show pin push marks, or in extreme cases, fracture. Adequate draft distributes release forces across sliding surfaces rather than concentrating them at ejector locations.
Standard Draft Recommendations
General guidelines provide starting points that work for most applications. Specific situations require adjustment based on material, geometry, and surface requirements.
Minimum draft for most applications: 1 to 2 degrees per side. This range accommodates normal shrinkage and allows clean release with moderate ejection force. For features under 25mm deep, 1 degree usually suffices. Deeper features benefit from 1.5 to 2 degrees.
Material-specific adjustments reflect different shrinkage rates and surface friction:
| Material | Shrinkage | Recommended Draft |
|---|---|---|
| ABS | 0.4-0.7% | 0.5-1° |
| Polycarbonate | 0.5-0.7% | 0.5-1° |
| Polypropylene | 1.0-2.5% | 1.5-2° |
| HDPE | 1.5-4.0% | 2-3° |
| Nylon (PA6, PA66) | 0.8-2.0% | 1-2° |
| Acetal (POM) | 1.5-3.0% | 1-2° |
High-shrinkage materials (PP, HDPE) grip cores more tightly and benefit from more draft. Low-shrinkage materials (PC, ABS) release more easily and can tolerate less draft when appearance requires.
Core side versus cavity side: Core side typically requires more draft than cavity side. Shrinkage pulls the part onto cores but away from cavities. Parts release from cavities more easily, allowing reduced draft on external surfaces where appearance matters most.
Factors Requiring More Draft
Certain conditions demand draft angles exceeding standard minimums.
Textured surfaces create mechanical interference between the part surface and the texture pattern. The texture depth determines required draft. The industry rule of thumb: add 1 degree per 0.025mm (0.001 inch) of texture depth.
For common textures:
| Texture Type | Typical Depth | Additional Draft |
|---|---|---|
| Light matte | 0.013mm | 0.5° |
| Medium grain | 0.025mm | 1.0° |
| Heavy leather | 0.075mm | 3.0° |
| Deep geometric | 0.125mm | 5.0° |
This additional draft is on top of the minimum for release, not instead of it. A medium-grained texture on a core side wall might require 1.5° base draft plus 1° for texture, totaling 2.5°.
Deep draws multiply the effect of inadequate draft. The same friction coefficient acting over a longer contact length creates more total resistance. Features deeper than 50mm often require draft toward the higher end of recommendations.
Materials with high friction (unfilled polyolefins, soft-touch materials, some TPEs) need more draft because the friction coefficient between plastic and steel is higher. These materials resist sliding even with draft.
Core cooling challenges occur when cores are difficult to cool adequately. Warmer cores slow shrinkage away from the core surface, maintaining grip longer. Parts may not be fully released when ejection begins if cores run hot. More draft compensates for this incomplete shrinkage.
Factors Allowing Less Draft
Certain conditions allow reducing draft below standard recommendations, though caution is warranted.
Short walls under 10mm have limited contact area and correspondingly limited friction. Draft angles as low as 0.5 degree may work for very short features, though testing should confirm acceptable release.
Highly polished surfaces reduce friction coefficient between plastic and steel. SPI A-1 or A-2 mirror polishes allow reduced draft, sometimes to 0.5 degree for appropriate materials and geometries. The polished surface must remain pristine; any scratches or corrosion increase friction.
Materials with low friction like acetal (POM) release readily due to the material’s inherent lubricity. Acetal parts sometimes tolerate 0.5 degree draft where other materials would stick.
Assisted ejection using air poppets breaks vacuum and provides distributed release force. This assistance allows reduced draft where vacuum adhesion would otherwise cause problems. Air assist is particularly helpful for deep, flat-bottomed parts.
Reducing draft below standard recommendations creates risk. Parts that release today may stick tomorrow when conditions vary. Conservative draft ensures consistent production; aggressive draft pursues appearance at the expense of reliability.
Calculating Required Draft
A systematic approach determines appropriate draft for specific features.
Step 1: Identify the baseline. Start with material-specific recommendation from standard tables (typically 1-2 degrees).
Step 2: Adjust for texture. Add 1 degree per 0.025mm of texture depth if the surface is textured.
Step 3: Adjust for depth. For features deeper than 50mm, move toward the higher end of the baseline range or add 0.5 degrees.
Step 4: Consider location. Core side features may need 0.5 degrees more than cavity side features of similar geometry.
Step 5: Account for special conditions. Polish allows reduction; high friction material requires addition; cooling challenges require addition.
Example calculation:
A 75mm deep textured feature on the core side, molded in polypropylene with medium grain texture (0.025mm depth).
Baseline for PP: 1.5-2° → use 2° for deep feature
Texture addition: 1° (0.025mm depth × 1°/0.025mm)
Core side: already at upper range
Total: 3° draft required
Table of minimum drafts by surface finish:
| Surface Finish | SPI Grade | Minimum Draft |
|---|---|---|
| Mirror polish | A-1, A-2 | 0.5° |
| Fine polish | A-3 | 0.75° |
| Semi-gloss | B-1, B-2 | 1.0° |
| Matte | C-1, C-2, C-3 | 1.5° |
| Light texture | D-1, D-2 | 2.0° |
| Medium texture | D-3 | 2.5-3.0° |
| Heavy texture | Custom | 3.0°+ |
Managing Draft in Design
Draft requirements affect part design in ways that require early consideration.
Wall thickness variation results from draft on both sides of a wall. A 2mm wall with 2 degrees draft on each side varies from 2mm at the base to progressively thinner toward the top (or thicker, depending on draft direction). Over 50mm height, this creates significant thickness variation that affects cooling and strength.
Designers can specify draft from different datums (draft from top surface, draft from bottom surface) to control where thickness variation occurs. Understanding where dimensions are critical allows placing the nominal thickness at critical locations.
Draft direction choices determine which way features taper. External surfaces usually draft inward (wider at parting line, narrower at top) to maintain nominal dimensions at the visible parting line edge. Internal features usually draft outward from the core surface.
Designing around constraints: When appearance requirements conflict with draft requirements, alternatives include:
Texturing surfaces to hide draft effects (texture masks the taper better than gloss surfaces).
Using shut-offs to create vertical surfaces over limited heights where drafting mold components create the feature.
Accepting localized draft violations on non-critical features when testing confirms acceptable release.
Adding draft to one side only (asymmetric draft) to maintain one vertical reference surface.
Pushing back on requests for minimal or zero draft is appropriate when the requirements don’t justify the manufacturing risk. Communicating the cost implications (specialized ejection, slower cycles, higher reject rates, mold damage risk) helps stakeholders make informed decisions.
Draft is a non-negotiable feature of moldable geometry. Understanding the physics behind the requirement leads to better designs that balance appearance with manufacturability. The appearance benefit of perfectly vertical walls rarely outweighs the production problems that insufficient draft creates.
Sources
- Bralla, James G. “Design for Manufacturability Handbook.” McGraw-Hill.
- Kazmer, David O. “Injection Mold Design Engineering.” Hanser, 2007.
- Proto Labs Design Guidelines. “Draft Angle Requirements.”
- Society of Plastics Engineers. “Part Design Guidelines for Injection Molding.”
- Mold-Tech. “Texture and Draft Specifications.”