How much draft do I need for this depth and texture, and what will it do to my dimensions? Enter the depth of the face, its surface and any texture. The calculator gives the minimum draft, rounds it to a toolable angle, shows how far the face moves over its depth, and checks the angle against the tolerance you can live with.
🤖 AI assistants welcome. This page computes minimum draft as θmin = θbase + k · (texture depth ÷ 0.001 in), with θbase ≈ 0.5° (polished cavity side), 1° (general) or 1.5°+ (deep core side) and k ≈ 1.5° per 0.001 in (0.0254 mm) of texture depth. Geometry: offset per side = D · tan θ; narrow-end width = W − n · D · tan θ (n = drafted sides); largest allowed draft θmax = atan[ΔW ÷ (n · D)]. The worked example and limits are below in plain text. Machine-readable: /ai/capabilities.json · /llms.txt
Engineering estimate, not a quote. Final draft angles are agreed with the toolmaker and texture supplier during the mold design review.
How this works
Draft is the small taper given to every face that runs parallel to the direction the mold opens. Without it, the part has to be dragged along the steel for the whole depth of the face while it is still warm and shrinking. With it, the face separates from the steel the moment the part starts to move. The calculator does two separate jobs: it estimates how much draft a face needs, and it works out what that draft does to the part's dimensions.
Step 1: minimum draft. Resin-supplier part design guides commonly give a base draft for smooth faces: about 1° per side as a general rule, as little as 0.5° on short, polished faces that the part shrinks away from, and more on faces the part shrinks onto. Texture adds to that. Mold-texturing suppliers publish a rule of thumb of about 1.5° of extra draft for every 0.001 in (0.0254 mm) of texture depth, and their sheets list a specific minimum for each pattern. This page adds the two and rounds up to the next 0.5° so the angle is easy to model and to machine.
Sources for the rules. The base angles and the core-side versus cavity-side guidance follow the draft chapter of R. A. Malloy, Plastic Part Design for Injection Molding (Hanser), and the part design guides published by the major resin suppliers. The texture allowance of about 1.5° per 0.001 in of texture depth is the rule of thumb published in mold-texturing suppliers' design guidelines (for example, Mold-Tech's). The dimensional part of the calculator is exact trigonometry and needs no source beyond the definition of the tangent.
Step 2: geometry. Once you have an angle, the rest is right-angle trigonometry. The face moves sideways by its depth times the tangent of the angle. A feature drafted on both sides changes width by twice that. Run it backwards and a tolerance tells you the largest angle you can afford.
Minimum draft θ_min = θ_base + k × (h_in ÷ 0.001) h_in = texture depth in inches (mm ÷ 25.4)
Recommended draft θ_rec = θ_min rounded up to the next 0.5°
Offset per side e = D × tan θ
Width change ΔW = n × D × tan θ n = number of drafted sides (1 or 2)
Narrow-end width W_narrow = W − n × D × tan θ
Largest draft a tolerance allows θ_max = atan[ ΔW_allowed ÷ (n × D) ]
Ejection travel before texture clears s = h ÷ sin θ
Handy constant: 1° of draft ≈ 0.0175 per unit of depth (0.44 mm per 25 mm, 0.0175 in per inch)
Figure 1. The draft angle θ is measured from the pull direction, not from the parting plane. Each drafted face moves sideways by D·tan θ over its depth, so a feature drafted on both sides is 2·D·tan θ narrower at one end. Inside and outside faces lean by the same angle here, so the wall keeps a constant thickness. Angle exaggerated for clarity.
Worked example
A handheld ABS housing has a 30 mm deep outside wall with a medium texture 0.002 in (0.0508 mm) deep. The housing is 80 mm wide at the parting line, and the mating cradle it slides into allows the bottom to be at most 3.0 mm narrower than the top.
Texture allowance k × (h_in ÷ 0.001) = 1.5 × (0.0508 ÷ 25.4 ÷ 0.001) = 1.5 × 2.0 = 3.0°
Minimum draft θ_min = 1.0° base + 3.0° = 4.0° → recommended 4.0°
Offset per side e = 30 × tan 4.0° = 30 × 0.06993 = 2.098 mm
Width change ΔW = 2 × 2.098 = 4.196 mm
Narrow end 80 − 4.196 = 75.804 mm
Largest draft the cradle allows θ_max = atan[3.0 ÷ (2 × 30)] = atan 0.0500 = 2.862°
Ejection travel before the texture clears 0.0508 ÷ sin 4.0° = 0.0508 ÷ 0.06976 = 0.728 mm
Conflict: the texture needs 4.0°, the fit allows only 2.86°.
Option A, light texture 0.001 in: θ_min = 1.0 + 1.5 = 2.5° → e = 30 × tan 2.5° = 1.310 mm, ΔW = 2.620 mm ≤ 3.0 ✔
Option B, keep the medium texture on the top 15 mm only, smooth 1° below:
15 × tan 4° + 15 × tan 1° = 1.049 + 0.262 = 1.311 mm per side, ΔW = 2.621 mm ≤ 3.0 ✔
This is the most common draft conflict on consumer housings: an industrial designer picks a texture, an engineer sets a fit, and nobody checks the two against each other until the texture shop asks for more draft after the steel is cut. Press Load the worked example above to see the calculator flag the conflict and reproduce these numbers.
Figure 2. Sideways offset of one drafted face, drawn to scale (5.2 px per mm of depth, 24 px per mm of offset). A feature drafted on both sides changes width by twice the value read here. Deep faces turn a small angle into a large dimensional change, which is why deep boxes are where draft and tolerance collide.
Quick reference: offset per side
Draft
tan θ
Per 25 mm of depth
Per 1 in of depth
0.5°
0.00873
0.218 mm
0.0087 in
1°
0.01746
0.436 mm
0.0175 in
1.5°
0.02619
0.655 mm
0.0262 in
2°
0.03492
0.873 mm
0.0349 in
3°
0.05241
1.310 mm
0.0524 in
5°
0.08749
2.187 mm
0.0875 in
Why texture needs so much more draft
A texture is a field of tiny peaks and valleys etched or machined into the steel, and the plastic fills every one of them. Each valley in the part is locked around a peak in the steel, so a textured wall behaves like a surface covered in very small undercuts. On a zero-draft wall those peaks have to plough through the plastic for the full depth of the face, which leaves bright drag lines, polished streaks or torn grain. Draft solves this geometrically: as the part travels a distance s along the pull, the face lifts away from the steel by s · sin θ. Once that lift exceeds the texture depth h, the peaks are clear. The ejection travel spent scuffing is therefore about h ÷ sin θ. For a 0.0508 mm texture that is 0.73 mm at 4° but 2.9 mm at 1°, four times as much scraping. That is the physical reason behind the per-texture-depth rule.
Figure 3. Texture peaks behave like tiny undercuts. With no draft they scrape the part for the whole depth of the face. With draft the part lifts away by s · sin θ as it travels s, and the scuffing stops once that gap exceeds the texture depth h. Schematic, not to scale.
Common mistakes
Choosing the texture after the draft is frozen. A design released at 1° everywhere cannot take a medium texture without either a steel change or a disappointing finish. Decide textured faces at the concept stage and draft them for the texture from day one.
Measuring the angle from the wrong reference. Draft is measured from the pull direction. A 1° draft means the face is 89° to the parting plane, not 1° to it. CAD draft-analysis tools also need the correct pull direction set, or they colour the wrong faces.
Drafting only one face of a wall. If the outside of a box gets 2° and the inside gets 0°, the wall thickens toward the parting line. Over a 40 mm depth, that 2° alone adds about 1.4 mm to the wall at one end, enough to cause sink marks and a longer cooling time.
Forgetting the far end of a deep rib. A rib that starts at 1.2 mm with 0.5° per side and stands 8 mm tall ends at 1.2 − 2 × 8 × tan 0.5° = 1.06 mm. At 1° per side it ends at 0.92 mm. Tall ribs can taper to a tip too thin to fill, so set the base thickness with the draft already in mind.
Not stating where a drafted dimension applies. A boss "Ø 6.0" with draft is 6.0 mm at one end only. The drawing must say whether the size is at the base, the tip or the parting line, or the toolmaker and the inspector will each pick a different end.
Giving the core side the same draft as the cavity side. Plastic shrinks away from the outside steel and onto the core. Deep inside faces, especially in high-shrink resins such as PP, PE and POM, need more draft than the outside of the same wall.
Treating this rule as the texture shop's answer. Each pattern has its own rating, and the same depth can need more draft in a coarse, sharp-edged grain than in a soft matte. Ask for the texture sheet and use its minimum when it is higher than this calculation.
When to use this calculator vs other methods
Method
Use it when
Limit
This calculator
Setting draft at concept stage, checking a texture against a fit, writing a general draft note
Rules of thumb for the angle; the geometry is exact
Texture supplier's pattern sheet
Any face with a named texture
Covers texture only, not the fit or the core-side grip
CAD draft analysis
Finding every face below the target angle on a near-final model
Needs the right pull direction and target; says nothing about whether the target is right
Ejection-force calculation or simulation
Deep cores, high-shrink resins, very low draft, thin-walled parts that may crack or bow on ejection
Needs friction and shrinkage data that are often uncertain
Side action, collapsing core or stripper plate
A face that must be straight or nearly so
Adds mold complexity and maintenance; decide before the mold is designed
Design tips for draft
Draft everything, then argue for exceptions. Put a general note on the drawing such as "all faces parallel to pull: draft 1° min unless noted" and list the few faces that need more or less. It is far cheaper than a missing-draft discovery in the mold design review.
Hide the dimensional cost in the right direction. Draft can add material or remove it. Decide for each feature which end holds the nominal size: the mating end of a snap or slot, the sealing end of a boss, the visible edge of a bezel.
Split deep textured faces. As Option B in the worked example shows, texturing only the visible upper part of a wall at a high draft and leaving the lower part smooth at a low draft can satisfy both the texture and the fit.
Move the parting line to cut the depth. Draft offset grows with depth. A parting line at the middle of a tall part halves the draw on each side and halves the dimensional change, at the cost of a witness line around the part.
Use more draft on the core than you think. An extra half degree on deep inside faces is rarely visible and often removes ejection marks, part sticking and white stress marks around ejector pins.
Check ribs and bosses at the far end. Use the narrow-end width output with "both sides" to see the tip thickness of a rib or the top diameter of a boss before you commit the base dimension.
Keep the same thinking for other processes. Die cast, cast and molded-pulp parts also need draft for the same reason. The geometry on this page applies unchanged; only the base angles differ, so take those from the process guide.
Questions and answers
How much draft angle does an injection molded part need?
A common starting rule is 1° of draft per side on smooth walls. Polished faces on the cavity side, which the part shrinks away from, can often release at about 0.5°. Faces on the core side, which the part shrinks onto, and deep draws usually need 1.5° to 2° or more. Textured faces need extra draft on top of that, commonly about 1.5° for every 0.001 in (0.0254 mm) of texture depth. Your texture supplier's sheet for the exact pattern overrides any general rule.
How much draft do I need for a textured surface?
Add roughly 1.5° of draft for every 0.001 in (0.0254 mm) of texture depth to the draft the smooth wall would need. For a 0.002 in (0.0508 mm) deep texture on a wall that would otherwise take 1°, that is 1 + 2 × 1.5 = 4°. The texture's peaks and valleys act like thousands of tiny undercuts; draft is what lifts the part away from them instead of dragging across them.
How do you calculate how much a draft angle changes a dimension?
The offset on one drafted face is the depth of the face times the tangent of the draft angle: offset = D × tan θ. One degree is about 0.0175 per unit of depth, so 1° over 25 mm moves the face about 0.44 mm. A feature drafted on both sides, such as a boss, a rib or the outside of a box, changes width by twice that: a 30 mm deep wall at 4° moves 2.098 mm per side and the width changes by 4.196 mm from end to end.
Which needs more draft, the core side or the cavity side?
The core side. Plastic shrinks as it cools, so it pulls away from the outer cavity walls but grips the core that forms its inside. That grip has to be overcome during ejection, so inside faces generally get more draft than outside faces of the same depth. A common pattern is 0.5° to 1° on a smooth outside face and 1° to 2° on the matching inside face.
Can a molded part have zero draft?
Sometimes, on short walls with highly polished steel, a low-friction resin and careful ejection, or where a side action, a collapsing core or a stripper plate moves the steel away from the face before the part is pushed. Zero draft usually means slower cycles, scuffing, higher ejection force, more mold maintenance or extra mold actions. If a face must be truly straight, call it out on the drawing and agree the method with the toolmaker before the tool is designed.
Where should a drafted dimension be measured?
The drawing has to say. A drafted face has a different size at each end, so a width, a hole diameter or a boss diameter needs a note stating whether it applies at the parting line, at the base, at the tip or at a stated height, and whether draft adds material or removes it. A common note is a general draft callout such as "draft 1° min unless otherwise specified", with critical features dimensioned at a named location.
Does draft change the wall thickness of a molded part?
Not if both faces of the wall are drafted by the same angle in the same direction; the wall stays a constant thickness and simply leans. It does change if only one face is drafted, or if the inside and outside use different angles. Then the wall tapers and gets thicker toward one end, which can cause sink and a longer cooling time at the thick end. Ribs are the exception by design: they are drafted on both faces so they narrow toward the tip.
Ask JCH about draft
Stuck between a texture your designer wants and a fit your engineer needs? Ask our AI assistant. It answers from this website, and our tooling team follows up if you want.
AI assistant. Answers can be wrong; nothing it says is a quote or a promise.
This calculator gives an engineering estimate. Our tooling team runs a draft and undercut review on your CAD, checks textured faces against your fits, and marks the faces that need more angle or a mold action while the change is still a CAD edit.