Injection Molding Design Rules: Draft, Walls, Ribs

Injection molding design rules are the geometry limits a plastic part has to respect so it fills, freezes, and ejects cleanly out of a steel mold. The core numbers are short to state. Draft every wall 1 to 2 degrees per side. Hold walls uniform, about 1 to 3mm for most thermoplastics. Size ribs and bosses at 50 to 60 percent of the nominal wall. Radius inside corners at 25 to 60 percent of it. Published resin-manufacturer design guides converge on these values, and a molder applies them to the cavity, the core, and the ejection system long before any steel is cut.

The rules exist because a molded part is never cut from solid stock. It forms inside a closed mold, shrinks as it freezes, and has to push clear of the very steel that shaped it. Every rule on this page traces back to one of three facts: shrink, ejection, or cooling. The injection molding hub carries the process story, the cycle stages, mold types, and gate and runner systems. This page is the rulebook a designer applies at the CAD screen, with the per-resin wall ranges, the draft-by-texture arithmetic, and the rib, boss, and gusset ratios that a summary cannot carry. For the cross-process framing of design reviews, start with design for manufacturing.

The sections below cover why a molded part obeys different rules than a machined one, then draft angles, wall thickness, ribs and bosses, radii and holes, gate and ejection decisions, and the tolerance territory that ISO 20457 governs. A checklist at the end compresses the rule set into a single review pass.

From the model to the tool quote

The rules on this page live in geometry, so what leaves the desk is a solid model exported as STEP, with units stated explicitly in millimeters on both the model and the drawing, because a unit mismatch rescales every wall and rib value above at once. CAD file formats covers the exchange formats molders and tool shops actually open and how to package native files alongside the neutral export, so this page does not restate that list. The 2D drawing still carries the intent the model cannot: the draft callout per surface, the texture specification, the tolerance tier per dimension, and the datum scheme the closing checklist ends on. Send the drawing with the model rather than after it, since the molder reads both together when quoting the tool.

Why a molded part obeys different rules than a machined one

A machined part starts as solid stock and gives up material to a cutter, so its limits are tool access, workholding, and how little wall survives cutting force. A molded part starts as melt. Two blocks of steel, the cavity and the core, close on that melt and form every surface at once, inside and out. From that single difference come the three constraints that shape every rule below.

First, shrink. Thermoplastics contract as they solidify. Amorphous resins such as ABS, polycarbonate, and polystyrene shrink under about 1 percent. Semi-crystalline resins such as polypropylene, polyethylene, nylon, and acetal shrink more, up to about 3.5 percent, and unevenly around thick sections and fibers. The mold is cut oversize to compensate, which ties part dimensions to the resin grade, so the resin is locked before mold design begins. The shrink table in the wall section lists published rates by resin.

Second, ejection. The finished part sits wrapped around the core and inside the cavity, and it must come out along one straight line, the draw direction. Surfaces parallel to that line need taper so they release instead of dragging. Features that point sideways, such as side holes, snap fits, and internal threads, are undercuts, and each one forces a mechanism into the mold: a slide for external undercuts, a lifter or a collapsible core for internal ones, an unscrewing device for threads. Shallow undercuts in flexible resins such as PE and PP can sometimes bump off. Every deliberate side action adds moving steel, wear surfaces, and maintenance, and it repeats in every cavity of a multi-cavity mold.

Third, cooling. The part cannot leave the mold until it is stiff enough to eject, and cooling time scales with the square of wall thickness: double the wall and the cooling-dominated portion of the cycle roughly quadruples. That arithmetic, more than any other, is why thin uniform walls are the economic heart of molded-part design. The thickest section on the part sets the cycle for the whole cavity set.

Mold construction hands the designer one more decision, the parting line, the seam where the two halves meet. Dimensions that stay within one mold half hold tighter than dimensions that cross the parting line or pass through moving mold sections, so critical features belong on one side of it. A stepped parting line needs a shut-off angle of about 7 degrees, with 5 degrees as the absolute minimum, to limit drag wear and flash on the shut-off steel. Die casting works the same way in metal, shrink and release, which is why its design guides read like a close cousin of this page.

Draft angles by surface condition

Draft is the taper built into a wall, rib, or boss so the part clears the steel during ejection. It is specified per side, and both the cavity and the core faces of a feature need it. The floor, on the most favorable geometry, is 0.5 degrees per side. The working range is 1 to 2 degrees per side, with deep parts taking proportionally more taper.

Getting the number right is a chain of four decisions: resin class, surface finish, texture depth, and feature type.

Resin class. Amorphous resins (ABS, PC, PMMA, PS) release readily and can run 0.5 degrees per side on shallow polished walls under about 1in of draw. Semi-crystalline resins (PP, PE, acetal, nylon) start near 1 degree per side, and PP and POM often take 2 degrees on smooth walls. Published per-material tables add roughly 0.25 degrees for each additional inch of draw depth.

Surface finish. Mold finishes fall into SPI classes: A1 to A3 diamond-polish gloss, B1 to B3 paper semi-gloss, C1 to C3 stone matte, and D1 to D3 dry-blast texture, spanning about Ra 0.012 to Ra 18µm from the finest polish to the coarsest blast. The surface finishing guide puts those classes in context. Draft follows finish: matte and textured surfaces need more taper than a polish, and the D-class textures drive the adder below.

Texture depth. The commonly cited rule adds 1 degree of draft for each 0.001in (0.025mm) of texture depth, on top of the base draft the finish already needs. Stated by depth band, published tables put light texture under 15µm at 3 degrees minimum, standard texture at 15 to 25µm at 3 to 4 degrees, heavy texture at 25 to 50µm at 5 degrees, and coarse grain above 50µm at 6 to 8 degrees. Some suppliers call for 1 to 1.5 degrees per 0.001in rather than 1 degree, so confirm the adder with the shop finishing the tool.

Feature type. Ribs carry 1 to 1.5 degrees per side as typical practice, with 0.5 degrees as the minimum, and rib draft thins the rib toward the top, so keep the top width at least 0.6mm or the rib may not fill. Bosses take 0.5 degrees minimum on the outside diameter and 0.25 degrees minimum on the cored inside diameter. Shut-off faces on stepped parting lines take the 7-degree figure from the section above.

Skimp on draft and the wall slides in full contact with the steel on every shot. The results are drag marks and scuffing on the show surface, texture tearing off the part, parts stuck on the core, distortion or breakage at the ejector pins, and galling on polished mold steel. One degree of taper prevents all of it; nothing on that list repairs cheaply in production.

One geometry check closes the section: draft changes the wall from top to bottom. A round part 4in deep drafted 3 degrees per side grows roughly 0.42in from top to bottom, so on deep drafted walls, verify the nominal wall at both ends rather than only at the height the drawing states.

Wall thickness by resin

Uniform walls come before everything else. A thick section freezes last: the skin stiffens while the molten core keeps shrinking, and the core pulls the surface inward into a sink mark or closes into an internal void. Non-uniform thickness is the primary driver of sink, warp, residual stress, and dimensional drift, and semi-crystalline resins show it worse than amorphous ones because they shrink more in the first place.

Most thermoplastic work lands at 1 to 3mm of wall. Around 1mm is the practical floor for flow, and about 5mm the practical ceiling for cycle time; most consumer parts sit between 1.5 and 3mm. Published resin-manufacturer design guides give each resin a range, and the table below collects those ranges next to the matching molding shrink rates. Confirm the range for the specific grade with the resin supplier, because filled and lubricated grades shift both columns.

Three patterns read straight out of the table. Amorphous resins (ABS, PC, PS, PMMA, PEI) shrink between roughly 0.2 and 0.8 percent and sink less. Semi-crystalline resins (PP, PE, PA, POM, PET) shrink from roughly 1.0 to 3.5 percent, so their walls trend thinner and their ribs trend thinner still. The ranges are wide because they span the variety of grades and part sizes each resin serves; pick a nominal inside the range and hold it uniform.

The thin end of the range is limited by flow. Thin walls need higher injection pressure and risk short shots, and published flow length-to-thickness ratios run about 100:1 to 300:1 depending on the material, so a long thin part may need a flow analysis or an extra gate. Lay the gate out so melt flows from thick sections into thin ones, which avoids restricted flow, trapped stress, and uneven packing.

Where thickness must change, make the transition gradual, about 3:1 in taper length to thickness change, and keep adjacent walls within about 40 to 60 percent of each other. Core out bulky sections instead of thickening walls: coring keeps shrink uniform, removes the sink risk, and shortens the cycle. Settle the resin before freezing the wall values, since the two columns of the table move together; the materials guide covers resin selection by property.

Ribs and bosses

Ribs buy stiffness without buying wall thickness, and the price of a rib is sink. Rib material sits on top of a solid wall, so the junction behaves as a local thick section, and the rib must be thinner than the wall it stands on. The standard rule sizes ribs at 50 to 60 percent of the nominal wall, and published design guides refine it to 0.6 times the wall on walls under 1/8in (3.2mm) and 0.4 times the wall on thicker walls. Amorphous resins tolerate the upper end of that band, semi-crystalline resins the lower end. Across published sources the rule spreads between 40 and 60 percent, and above roughly 65 percent, sink on the face opposite the rib becomes near-certain.

The rest of rib geometry follows from the same mechanics. Keep rib height at or under 3 wall thicknesses; deeper ribs fill poorly, build mass at the base, and stick on ejection. Space parallel ribs at least 2 wall thicknesses apart so the steel blade between them stays sound and cools the part evenly. Root the rib with a radius of 25 to 50 percent of the wall, minimum 0.015in (0.38mm). Prefer melt flow running down the length of a rib; flow striking a rib across its width branches, hesitates, and can trap gas. And prefer several thin ribs to one thick one: a lattice of light ribs stiffens a panel with less mass, less sink, and a shorter cycle than a single heavy rib.

Bosses follow rib logic. Keep boss wall thickness at the base under 60 percent of the nominal wall, or sink and voids appear at the junction. A common proportion sets the outside diameter at about twice the inside diameter, with height under 3 outside diameters. Radius the boss base at 25 to 50 percent of the wall, minimum 0.015in, and radius the end of the cored hole at 0.010in (0.25mm) minimum. Hold the boss at least 0.125in (3.2mm) inboard of a wall and tie the two together with a rib rather than merging them into a solid mass, and keep at least 2 wall thicknesses between neighboring bosses. Core tall or thick bosses hollow. For self-tapping screws, published guides set the cored inside diameter near 0.8 times the nominal screw diameter, engagement of at least 2.5 screw diameters, and a cored hole about 0.032in (0.813mm) deeper than the fully engaged screw, with a chamfer at the boss top as a lead-in.

Gussets brace free-standing bosses and follow rib rules: 50 percent of nominal wall in thickness, height up to about 95 percent of the boss it supports and generally under 4 wall thicknesses with 2 preferred, length 30 to 100 percent of gusset height, and a fillet near 25 percent of the wall at the intersections.

Radii, corners, and holes

A sharp inside corner does two jobs badly: it concentrates stress in the finished part and it forces the melt to turn hard as it fills. Published guides call for a fillet of 25 to 60 percent of the nominal wall at inside corners, toward the high end where the corner carries load, with a suggested minimum of 0.020in (0.51mm), and sharp edges broken by at least 0.005in (0.13mm). Keep the corner at uniform thickness by setting the outside radius equal to the inside radius plus the wall, R = r + t, which also evens out shrink around the corner. Edges of depressions take a minimum radius of 0.015in (0.38mm), with about half the nominal wall preferred.

Holes are cored by pins, and a pin standing in moving melt works like a cantilever. A blind hole, pinned from one end, is reliable to a length-to-diameter ratio under 2, stretching to about 3 once the diameter passes 3/16in (4.8mm). A through hole, pinned from both ends, reaches a ratio of 4, and about 6 at those larger diameters. Space holes at least 2 wall thicknesses, or 2 hole diameters, from each other and from edges, whichever is larger, so the pins and the material around them survive injection pressure. Keep hole axes parallel to the draw direction; an angled or side-facing hole is an undercut, with everything that brings.

Gates, ejection, and undercuts

Gate placement is a part-design decision with mold consequences. The gate sets where melt enters, and with it the flow path, the weld-line positions, and the packing pattern. Gate so the melt runs from thick sections into thin ones, keep gates off cosmetic faces because every gate leaves a witness, and walk the weld lines: two flow fronts meeting around a hole or a boss leave a visible and weaker seam, so place that seam where appearance and strength can live with it. Published molder guidance sizes the gate land at roughly 50 to 80 percent of the wall thickness at the gate.

Ejection needs the same care. Ejector pins push the part off the core, and every pin leaves a mark, so land the pins on non-cosmetic, non-functional surfaces and give the part enough flat area for them to push against. Draft and ejection compound: more taper means less ejection force, which means smaller pins and less witness.

Undercuts deserve their own pass. Before accepting a side action, try the three design moves that delete it: relocate the feature to the parting line so the mold halves form it, pass a core pin through the part and shut it off on the far side, or split the part into two pieces that each mold plainly. When the undercut is functionally required, the slide or lifter is the honest answer, and it belongs in the tooling conversation early, while the parting line is still negotiable. For undercut-heavy prototype geometry, printing the part settles the form before any tool is cut; see 3D printing and the injection molding versus 3D printing comparison.

Tolerances and the design decisions that move them

ISO 20457 specifies manufacturing tolerances and acceptance conditions for moulded plastic parts, covering parts made by injection, injection-compression, transfer, compression, and rotational molding. The standard draws one line worth knowing: it does not address surface imperfections such as sink marks. The practical reading for a designer is that tolerance standards assign dimensional windows, while sink, warp, and read-through stay geometry problems, solved with the ratio rules above rather than bought with a tighter callout. German practice runs parallel through DIN 16742, which classifies molded dimensions as mold-fixed or non-mold-fixed and widens the window for the non-mold-fixed ones.

Three design decisions move molded tolerances more than any others.

Where the dimension lives. A dimension formed within one mold half holds tighter than one that crosses the parting line or spans moving mold sections, because mold closure and core shift add variation. Put critical relationships on one side of the parting line.

Which resin and fill. The shrink table above shows the spread, from roughly 0.2 percent on acrylic to 3.5 percent on polyethylene. Glass or mineral fill cuts shrinkage about in half in published materials data and softens sink, but fiber-filled grades shrink directionally, which trades a dimensional problem for a flatness problem on wide flat parts.

How much draft. A drafted face is a tapered face, so a drawing that sizes a drafted wall without stating the measuring height is ambiguous at inspection. State where the nominal applies, top, middle, or bottom, and check both ends on deep walls.

When a feature must hold tighter than the mold alone will hold, the standard move is to mold it close and machine it after: a drilled and reamed hole or a machined face holds machining tolerance regardless of the resin. The CNC machining guide covers that post-mold route. Whatever window is chosen, put it on the drawing together with the resin grade and its shrink value; technical drawing requirements covers the callouts that make a molded-part drawing readable to a molder.

The draft-angle table on this page, minimum draft by surface condition, is the review baseline for the first of those decisions. Use it as written, then adjust per the resin class and finish decisions in the draft section.

Injection molding design checklist

Run this pass over the model before the file leaves the desk. Each line exists because its failure mode costs more to fix in steel than in CAD.

Resin and shrink:

• Resin grade selected and locked, with its published shrink range noted on the drawing.
• Filled grade weighed where sink or shrink must come down, with directional shrink checked on flat parts.

Walls:

• Nominal wall inside the published range for the resin, 1 to 3mm for most work.
• Adjacent walls within about 40 to 60 percent of each other, with transitions gradual at about 3:1.
• Bulky sections cored out rather than left solid.

Draft:

• 1 to 2 degrees per side on vertical walls, with 0.5 degrees only on shallow polished amorphous work.
• Texture accounted for: base draft plus about 1 degree per 0.001in (0.025mm) of texture depth.
• Ribs at 1 to 1.5 degrees, and bosses 0.5 degrees outside and 0.25 degrees inside.
• Stepped parting-line shutoffs at about 7 degrees.

Ribs and bosses:

• Rib thickness 50 to 60 percent of the wall, 0.6 times on thin walls and 0.4 times on thick ones.
• Rib height at or under 3 wall thicknesses, spacing at least 2 wall thicknesses, root radius 25 to 50 percent of the wall.
• Boss wall under 60 percent of the wall, OD near twice the ID, height under 3 diameters, bosses tied in with ribs or gussets and cored when tall.

Radii and holes:

• Inside fillets 25 to 60 percent of the wall, and outside radius set to inside radius plus wall.
• Blind holes under 2 diameters deep and through holes under 4, with holes spaced at least 2 wall thicknesses or 2 diameters from edges and each other.
• Hole axes parallel to the draw direction.

Gates, ejection, undercuts:

• Gate positioned thick-to-thin, off cosmetic faces, with weld lines placed deliberately.
• Ejector witness marks on non-functional surfaces, with enough flat area to push against.
• Every undercut listed, and each one justified, moved to the parting line, cored through, or designed out.

Tolerances and file prep:

• Critical dimensions kept within one mold half, with across-parting-line callouts given the wider window.
• Drafted dimensions measured at a stated height.
• Tight features flagged for post-mold machining where the mold alone will not hold them.
• File exported with explicit units, and the resin grade, finish class, and texture depth stated alongside it; CAD file formats covers the formats molders read.

A part that clears this review fills, freezes, and ejects the way the rules intend. For the road from prototype iterations to production tooling, see rapid prototyping and low-volume manufacturing. The shared vocabulary of the molding floor is collected in the manufacturing glossary.