How to Design Ribs and Bosses: Wall Ratios, Draft and Sink Control

A connector housing failed final inspection over a defect that no dimension caught. The stiffening rib under the gloss face had a base drawn at 0.8x the 2.0 mm nominal wall. The extra material made a 3.6 mm local section under a 2.0 mm skin, and that mass pulled the face inward by 0.04 mm as it cooled. A raking light showed the dip on every shot, and the fix meant recutting the cavity.

Ribs stiffen walls and bosses carry screws, yet both are local thick sections that decide whether a mold fills, ejects, and stays sink-free. This guide is the dedicated geometry pillar for those two features, read from the mold side. It states the ratios the drawing must carry so the tool maker can cut draft, vent the deep slots, and eject without scuffing. The nine-rule overview, How to Design for Moldability: 9 Geometry Rules, gives ribs and bosses one rule each. This article gives both features the full ratio treatment with tables and example numbers.

The Snapshot

• Rib base thickness: 0.4 to 0.6x the adjoining wall, with 0.5x as the common working figure. Thicker bases sink before the press runs.
• Rib height: hold at 2 to 3x base thickness for stability. Draft ribs over 5 mm tall at 0.5 to 1.5 degrees per side and taper tips toward 0.8 to 1.2 mm.
• Boss walls: 0.4 to 0.6x nominal wall with the outside diameter near 2x the bore. An M3 boss runs a 3.0 to 3.4 mm bore at a 6 to 7 mm OD.
• Sink visibility: dips read on gloss surfaces from about 0.025 mm up. Rib bases above 0.5 to 0.6x wall sink first.
• Filling: ribs crossing the flow create knit lines, while ribs parallel to the flow fill best. Rib tips are last-fill traps that need vents or ejector pins at the ends.

Why Ribs and Bosses Fail Parts

Ribs and bosses exist to buy stiffness without wall thickness. Bending stiffness grows with the cube of section depth, which is why a ribbed 2.0 mm wall beats a flat wall on stiffness per gram. A rib is a blade of material standing on the wall, and a boss is a hollow cylinder that seats a screw or aligns a mating part. Both work until the geometry crosses a ratio, and then they fail the mold in predictable ways.

The failures show up at trial, not in CAD. A rib base at 0.8x wall sinks the opposite face from about 0.025 mm on gloss. A rib with no draft over 5 mm of height scuffs or sticks during ejection. A sharp root corner below 0.25 mm radius cracks the steel at the slot base after thermal cycling. Each failure maps to a number the drawing never stated.

Five failure modes trace directly to rib and boss geometry:

• Sink marks above the rib base or boss wall, visible from 0.025 mm on gloss faces.
• Short shots at rib tips and boss tops where air traps at the end of the slot.
• Ejection scuffing or sticking on ribs drafted under 0.5 degrees per side.
• Weld lines where ribs run across the flow and the melt rejoins around them.
• Cracked ribs at the root where the fillet radius sits under 0.25 mm.

Every one of these is cheaper before steel. A DFM pass that checks the rib ratio, draft, root radius, and venting plan costs hours in CAD. Found at T1 instead, the same problem becomes EDM work, a welded repair, or a new cavity insert. The geometry rules below are what keep that rework off the mold schedule.

Rib Geometry: The 0.5-0.6x Wall Rule

The rib base is the single number that decides most rib failures. Hold it at 0.4 to 0.6x the adjoining nominal wall, with 0.5x as the common working figure. On a 2.0 mm wall that means a 1.0 mm base at 0.5x, inside an allowed band from 0.8 to 1.2 mm. Above 0.6x, the material behind the opposite face is thick enough to sink before any process setting can help.

The ratio does the same job on every wall thickness. A 2.5 mm wall takes a 1.0 to 1.5 mm rib base, and a 3.0 mm wall takes 1.2 to 1.8 mm. Shrinkage class adjusts the working point. Semicrystalline resins that shrink 1.5 to 2.5 percent should stay at or below 0.5x. Amorphous resins at 0.5 to 0.7 percent shrinkage can run 0.6x on hidden faces.

Height follows the base. A rib fills and ejects stably up to about 2 to 3x its base thickness. A 1.0 mm base rib therefore runs 2 to 3 mm tall before it needs a taper, gussets, or a tooling review. Above 3x base, the tip fills late, the melt hesitates at the root, and the steel can grip the blade hard enough to buckle the rib during ejection.

Draw the full rib definition on the part. State the base thickness, height, draft per side, tip thickness, and root radius. Spacing matters too: keep parallel ribs about 2 to 3x the wall apart so melt flows between them without hesitation, which is 4 to 6 mm on a 2.0 mm wall. A drawing that states all six numbers gives the tool maker a cavity slot to cut, vent, and polish without guessing.

Rib Draft, Tip and Root Radii

Draft releases the rib from its steel slot. Ribs need 0.5 to 1.5 degrees per side, with 0.5 degrees as the floor on ribs over 5 mm tall. Deep ribs above 10 mm run 1.0 to 1.5 degrees per side so the steel does not grip the blade. Draft failures at scale have their own guide in 9 Draft Angle Mistakes That Kill Moldability, and this section fixes the numbers for ribs.

Texture changes the draft requirement. The typical rule is about 1 degree of draft per 0.025 mm of etch depth. A shallow VDI finish around 0.025 mm deep takes about 1 degree per side, and a 0.05 mm grain takes 2 degrees. Specify the SPI or VDI class before the draft is locked, because texture added after steel is cut removes draft for free.

Draft grows the root. At 1 degree per side, a 10 mm rib gains about 0.35 mm across its base, since tan 1 degree is 0.0175 mm per mm of height. A 1.0 mm tip on a 10 mm rib at 1 degree per side lands near 1.35 mm at the root, which can cross the 0.6x limit on a 2.0 mm wall. Dimension the rib from the tip, then confirm the root stays inside the wall ratio.

Tip thickness controls filling and packing at the end of the slot. Draw the free end at 0.8 to 1.2 mm. Unfilled resins will fill thinner slots, but tips under 0.8 mm starve in practice, and glass-filled grades need 1.0 to 1.2 mm so fibers do not bridge at the tip. A fat tip above 1.5 mm overpacks at the last point to freeze and adds mass to the very zone that sinks.

Root radius keeps both the part and the steel alive. A fillet of 0.25 to 0.5 mm spreads the bending stress where the rib meets the wall and removes the crack starter that a sharp corner creates. The same radius protects the mold, because the slot corner is a thin blade of steel that sees cavity pressure of 30 to 80 MPa on every shot. A zero-radius corner will chip during polishing or crack in service.

Boss Geometry: Wall, Height and Core Pins

A boss is a hollow cylinder standing off the wall to seat a screw, pin, or mating feature. Its wall thickness should run 0.4 to 0.6x the nominal wall, with the outside diameter near 2x the bore diameter. A molded M3 boss typically shows a 3.0 to 3.4 mm bore at a 6 to 7 mm OD. At a 3.2 mm bore and 6.2 mm OD, the wall works out to 1.5 mm per side, which is 0.6x on a 2.5 mm wall.

Height is capped before gussets. A boss stands freely up to about 2.5x its outside diameter. A 6 mm OD boss runs to 15 mm tall unsupported, and above that, side loads from insertion or screw torque crack the root. The fix is gussets, a cored base, or a shorter boss, never a thicker wall.

Draft on a boss comes from two surfaces. The outside wall needs 0.5 to 1 degree per side so the part releases from the cavity. The bore is formed by a core pin, and the pin must pull out of the hole on ejection. Deep bores bend the pin under injection pressure, so hold unsupported pin length near 5x diameter or less and support the rest with a guide bushing.

Blind bosses trap air. A boss with a closed top is a dead end for the melt, and the air at the pin tip compresses as the cavity fills. Vent the core pin with a small flat of 0.02 to 0.05 mm, or place an ejector pin under the boss so it both vents and pushes the part off. Without one of those, the boss top shows a short shot or a burn mark on the first trial shots.

Gate near the boss. A boss packs through the gate, so place the gate under or beside the boss where the part allows. Gate depth at 50 to 80% of the wall keeps the feed open while the boss base packs, which is the same window that keeps sinks off the face behind the boss.

Gussets: Supporting Tall Bosses

Gussets turn a tall boss into a braced structure. Add three to four gussets radiating from the boss at 90 or 120 degree spacing, each 0.4 to 0.6x the nominal wall thick. A 1.0 mm gusset on a 2.0 mm wall is typical. The gusset web runs from the boss down the wall and tapers from about 0.5 to 0.75x the boss height down to zero at its outer tip.

Each gusset is a small rib and obeys rib rules. Keep the gusset base inside 0.5 to 0.6x wall, give it 0.5 to 1 degree of draft per side, and fillet its root at 0.25 to 0.5 mm. Gussets under a gloss face sink exactly like ribs, so core them out or move them off the cosmetic surface. Four thin gussets beat one fat one on both stiffness and sink risk.

Gussets earn their cost on load, not looks. A tall boss carrying screw torque of 0.4 to 0.6 N·m, typical for an M3 thread-forming screw into plastic, will crack at the root on vibration or re-assembly cycles without support. The gusset band that fixes it adds a few grams of material and one cavity detail. Any boss past 2.5x OD, or any boss hit by a side load at assembly, gets gussets by default in a DFM pass.

Sink Marks and the Cosmetic Surface Problem

Sinks are the most common rib and boss rejection, and the visibility threshold is tiny. A dip of about 0.025 mm reads on a gloss surface, and piano finishes catch dips near 0.01 mm. Sink risk starts the moment the rib base passes 0.5 to 0.6x wall. The full defect story with all eight mold-side root causes lives in How to Prevent Sink Marks, and this section keeps the geometry view.

The table below maps wall ratio to sink risk on a typical 2.0 mm wall. Local section means the wall plus the rib base behind the visible face. Values are typical published guidance, and the acceptance number belongs in the mold specification.

← swipe to scroll →

Table note: Typical published guidance for sink risk by rib base ratio on a 2.0 mm wall. Local section is the wall plus the rib base behind the visible skin. Verify against your material grade and surface finish before setting acceptance values.

Three geometry-led countermeasures fix most sink-prone ribs and bosses. First, core out the rib under the cosmetic surface, leaving a 0.5 to 1.0 mm gap between the rib end and the visible wall so the face stays at nominal thickness. Second, gate under or beside the feature so packing reaches the base before the gate freezes. Third, watch the pack step itself: overpacking swells the base, and the swell relaxes inward when pressure drops, so cut pack pressure in 10 percent steps while you measure the dip.

Measure the result, do not eyeball it. A profilometer or optical scanner reads sink depth across the feature, and a raking light finds the line before the gauge does. Set acceptance at 0.025 mm on gloss surfaces and 0.05 to 0.1 mm on textured ones at the T1 trial. Texture hides sinks two to four times deeper than gloss, which is a finish decision made before the cavity is polished.

Filling, Knit Lines and Venting Traps

Flow direction decides whether a rib helps or hurts the fill. A rib running parallel to the main flow fills cleanly along its slot. A rib crossing the flow splits the melt front, and the two fronts rejoin past the rib into a knit line. The same thing happens behind a boss, where the melt wraps around the cylinder and meets on the far side.

Knit lines cost strength, and the loss scales with material. At a good knit, unfilled amorphous resins keep 80 to 95 percent of tensile strength, glass-filled grades keep 40 to 70 percent, and LCP keeps 40 to 60 percent. A rib that must cross the flow deserves a mold flow analysis before steel. Our guide How to Reduce Weld Lines covers the gate moves, overflow wells, and temperature levers, while this article only flags the geometry that creates the knit.

Rib tips are last-fill traps. The deepest slot fills last, and air at the blind end has nowhere to go as the melt front arrives. Trapped air compresses, the tip short-shots, or the surface burns at the slot end. Vent at the rib ends with steel vents 0.01 to 0.06 mm deep on a 0.5 to 1.5 mm land, sized by material, or run ejector pins at the rib ends and let the pin clearance vent the slot.

Bosses create the same trap at their tops, and a boss fed from one side hesitates on the far side where the weld wraps around it. Ribs fill best along their long axis, so orient long ribs with the flow. If a knit must land behind a loaded boss, add an overflow well at the downstream side so the fronts meet inside the well instead of on the boss wall.

Mold-Side Machining of Thin Rib Slots

Every rib on the part is a slot in the steel. A 0.6 mm rib means a 0.6 mm wide slot, often 5 to 10 mm deep, cut into a hardened cavity block. That geometry decides the machining method before the tool is quoted. A slot deeper than about 4 to 5x its width stops being end-mill territory and moves to EDM.

Small end mills have a depth limit. A 0.5 mm carbide end mill is practical to about 3 mm of depth before deflection and tool breakage take over. For deeper slots, sinker EDM burns the shape with a graphite or copper electrode at typical tolerances of ±0.005 to 0.01 mm. Wire EDM cuts through-features and slot ends where a wire can pass, holding ±0.002 to 0.005 mm. Our article on wire EDM for mold making covers the process limits and finish in detail.

EDM leaves a recast layer on the slot walls. Typical recast runs 0.005 to 0.025 mm thick, with micro-cracks that collect at sharp corners. Polishing removes the recast, which is another reason the rib root carries a 0.25 to 0.5 mm radius. A zero-radius slot corner keeps those recast cracks in a loaded corner, and the blade cracks in service.

Steel choice buys strength, not stiffness. Tool steels all sit near 200 GPa modulus, so blade flexure is set by geometry: web thickness, slot depth, and the support behind the slot. What the grade and hardness buy is yield strength and wear. A cavity block at HRC 52 resists web flexure and erosion from glass-filled melt far better than the same block at HRC 30, which is why rib-dense cavities run hardened.

Cooling decides where the slots can go. Waterlines need about 2 to 2.5x their diameter of steel between the channel and the cavity surface, so a 10 mm channel needs 20 to 25 mm of cover. Deep rib clusters block straight drilling, and that is when the slot layout and the cooling layout must be resolved together, before the block is ordered.

Design Ratios Quick-Reference Table

This table is the drawing checklist for a DFM pass. Read it against the nominal wall, write the numbers on the part, and send it with the RFQ.

← swipe to scroll →

Table note: Typical published design ratios for ribs, bosses, and gussets in injection molded parts. All values scale from the nominal wall thickness and assume standard unfilled or lightly filled engineering resins.

Check an example end to end. A 2.5 mm wall with a 3.2 mm bore takes an OD near 6.2 mm, because 6.2 minus 3.2 divided by 2 is 1.5 mm per side, exactly 0.6x wall. The same boss at 8 mm tall sits inside the 2.5x OD limit of 15.5 mm, so it needs no gussets. At 18 mm tall it does, and the drawing should say so before the cavity is cut.

The table is a starting point, not a substitute for a fill and cooling review. Material shrinkage, gate position, and surface finish move the working point inside the bands. A mold design and DFM review flags the outliers before steel is ordered, and that review is the cheapest hour in the whole program.

FAQ: Rib and Boss Geometry

Q1. What happens if a rib base sits at 0.8x wall?

The local section behind the face is roughly 1.8x the nominal wall, and that mass sinks. On a 2.0 mm wall with a 1.6 mm base, expect dips from 0.05 mm up on gloss, clearly visible next to parts molded at 0.5x. The process cannot remove that dip, so the fix is geometry: thin the rib to 1.0 mm, add a second rib, or core out the base behind the cosmetic face.

Q2. How much draft does a 10 mm tall rib need?

At least 0.5 degree per side, and 1.0 to 1.5 degrees is the practical band for deep ribs. Draft adds width at the root, about 0.35 mm total at 1 degree per side over 10 mm. Textured surfaces need more, roughly 1 degree per 0.025 mm of etch depth, so lock the SPI or VDI class before the draft is dimensioned.

Q3. When does a boss need gussets?

Past about 2.5x its outside diameter, or whenever assembly loads it sideways. A 6 mm OD boss is fine to 15 mm, and above that add three to four gussets at 0.4 to 0.6x wall. Screw torque of 0.4 to 0.6 N·m into a tall unsupported boss cracks the root on re-assembly.

Q4. Why do sinks show on one rib and not the one next to it?

Sinks follow local mass, distance from the gate, and cooling. A rib at 0.55x wall near the gate packs well and stays clean, while a 0.7x rib at the far end of the same part sinks on every shot. Measure both at trial, and set acceptance at 0.025 mm on gloss before the first shots are taken.

Q5. Do snap-fit beams follow the same rib rules?

Snap beams are cantilever ribs with the same root logic at 0.5 to 0.6x wall, but the root radius matters more because bending strain concentrates there. Draft rules differ because the beam needs a sharp engagement face, not pure release. Our guide How to Design Snap Fits for Injection Molded Parts covers the allowable strain by resin and the beam math.

The Bottom Line

Ribs and bosses are thick sections wearing a useful name. Keep rib bases and boss walls at 0.4 to 0.6x nominal wall, draft every feature 0.5 to 1.5 degrees per side, fillet the roots at 0.25 to 0.5 mm, and vent the rib tips. State every number on the drawing, because the mold cuts what the drawing says.

The mold side then does its part: slots that EDM can reach, vents at the last-fill rib ends, gates that pack the boss bases, and cooling that keeps the thick zones from running hot. Geometry approved at the DFM stage fills, ejects, and stays sink-free at trial. Geometry that skips the ratio review pays for the omission in steel.

DieStrike is an IATF 16949 certified precision mold manufacturer running 120+ machines, with mold geometry held to ±0.005 mm standard and ±0.002 mm precision, cavity steel hardened to HRC 62, and injection molds delivered in 2 to 5 weeks. Standard mold parts ship in 3 to 7 days, DFM feedback returns within 24 hours, and connector OEMs including TE Connectivity, Amphenol, and Luxshare run geometry-critical programs on this tooling discipline. Send your rib and boss layout with the RFQ, and get the ratio check back with the quote by contacting DieStrike.