I. The Nature of Shrinkage: Plastic’s “Thermal Expansion & Contraction”
Plastic cools from a molten state (>200°C)to room temperature, inevitably shrinking. The mold cavity must be “Scaled Up.”
Core Formula:
Shrink Compensation=Nominal Part Dimension×Shrinkage Rate
Critical Note: This is not simple multiplication. Plastic shrink occurs in two phases:
Thermal Shrinkage: Occurs during cooling (primary factor).
Orientation Shrinkage: Caused by molecular alignment during flow, leading to warpage.
II. Practical Calculation: How to Determine the “Exact” Shrinkage Rate?
Do not blindly trust the “Standard Range” from suppliers (e.g., ABS: 0.4%-0.7%). You need empirical correction.
1. Get the Initial Value (Material Data sheet)
Look for “Mold Shrinkage” or “Linear Shrinkage” in the material spec sheet.
Amorphous Plastics (PC, ABS, PS): Stable shrink rate, low anisotropy. (e.g., ABS ≈ 0.5%, PC ≈ 0.5%-0.7%).
Crystalline Plastics (PP, PE, PA, POM): High and volatile shrink rate, high anisotropy. (e.g., PP ≈ 1.0%-2.5%, PA66 ≈ 1.2%-1.8%).
2. Wall Thickness Correction (Critical!)
Rule: Thicker walls = Larger shrink age.
Thin Walls (<1.5mm): Use the lower limit of the shrink range (e.g., PA66 use 1.2%).
Thick Walls (>3mm): Use the upper limitof the shrink range (e.g., PA66 use 1.8%), or higher.
Rule of Thumb: Increase shrink rate by 0.1%-0.2% for every 1mm increase in wall thickness.
3. Flow Direction Correction (Anisotropy)
For crystalline materials, Flow Direction (MD) shrink > Transverse Direction (TD) shrink.
Simple Parts: Use the average value.
Precision Parts / Long Features:
Example:For a PP part, MD shrink is 1.8%, TD shrink is 1.2%.
Mold Design:Scale the length (flow direction) by 1.8% and the width by 1.2%.
4. Formula Application Example
Let’s make a 100mm long PC strip (Wall thickness: 2mm).
PC shrink range: 0.5%-0.7%.
Medium thickness (2mm), take the mid-point: 0.6%.
Mold Cavity Length = 100mm × (1 + 0.6%) = 100.6mm.
III. Draft Angle Design: Ensuring a “Clean Birth”
If a sidewall is perpendicular to the opening direction (0° draft), the product will be “Choked” by the mold, causing silver streaks, scratches, or ejection failure.
1. Minimum Draft Angle Formula (Rule of Thumb)
While there is no absolute formula, industry follows:
“Require 0.5°-2°of draft angle per 1 inch (25.4mm) of depth.”
Quick Reference Table:
| Part Depth (Height) | Recommended Min. Draft (Per Side) | Offset per 25mm depth |
| < 20mm (Small) | 0.5° – 1° | 0.2mm – 0.4mm |
| 20mm – 50mm (Medium) | 1° – 1.5° | 0.4mm – 0.7mm |
| > 50mm (Deep Cavity) | 1.5° – 3° | 0.7mm – 1.3mm |
2. 3 Major Factors Affecting Draft Angle
Material Hardness:
Soft/Rubbery (TPU, TPE): High friction, requires larger draft (2°-5°).
Rigid (ABS, PC): Good stiffness, allows smaller draft (0.5°-1.5°).
Texture Depth (Critical!):
If the surface requires Texturing (VDI 3400 Standard) or Etching:
VDI 20 (Fine) → Add 0.15mm draft offset per 25mm depth.
VDI 30 (Medium) → Add 0.25mm draft offset per 25mm depth.
VDI 40 (Coarse) → Add 0.4mm draft offset per 25mm depth.
Calculation:For a 50mm deep part with VDI 30 texture, add 0.5mm offset per side ≈ 1° extra draft.
Precision Requirements:
For precision mating surfaces (e.g., flanges, snap fits) where draft is limited, consider “Delayed Ejection” or “Forced Ejection” (only for PE/PP).
IV. Conflict Resolution: Shrinkage vs. Draft
1. Problem: Ribs/Bosses – Sink Marks & Sticking
Symptom: Ribs are thick (prone to sink) and deep (hard to eject).
Solution:
Rib Thickness: Limit rib thickness ≤ 70%of adjacent wall thickness (Fundamental fix for sink).
Rib Draft: Use double the draft angle of the outer wall (e.g., if wall is 1°, rib is 2°-3°).
Root Radius: Apply R-angle to prevent stress concentration and improve release.
2. Problem: Clear Parts (PC, PMMA) – Stress Whitening
Symptom: Small draft angles cause ejection stress, turning edges white.
Solution:
Ensure draft ≥ 1.5°.
Polish mold surfaces to Ra < 0.05μmto reduce friction.
Conclusion: DFM Checklist
Before sending the 3D modelto the mold maker, verify:
Shrinkage Rate: Have you set a specific value (not a range) based on material, thickness, and flow direction?
Draft Angles: Do all vertical walls have ≥ 0.5° draft?
Texture Compensation: If textured, has the draft angle been increased accordingly?
Ribs: Are ribs thinner than 70% wall thickness with sufficient draft?
If you have a 3D model under design, send itto us. Our engineering team will provide a free DFM report including precise shrink compensation values, draft angle optimization, and warp risk analysis.