Injection Molding Design Guide

What the process imposes on your design

An injection mold has two halves. The cavity forms the outer surface of the part, the core forms the inner surface, and they close along a parting line. Molten polymer is injected under pressure, held while it cools and shrinks, then the halves separate and ejector pins push the part off the core.

Three consequences follow, and between them they explain almost every rule in this guide. The part must release from steel, so every vertical face needs taper. The polymer shrinks as it cools, and it shrinks unevenly wherever the section is uneven, so wall thickness must be controlled. And the tool has to be cut, so geometry that is expensive to machine is expensive to mold.

Choose the material first

Resin selection is not a late decision to be made once the geometry is fixed. Shrinkage rate, melt flow, and stiffness all differ between polymers, and they determine the wall thickness you can use, the draft you need, and the tolerance you can hold. Designing the part and then choosing the resin means redoing the part.

Resin	Characteristics
Acetal (POM)	Rigid and dimensionally stable, low moisture absorption, good chemical resistance. The default for gears and bearing surfaces.
Acrylic (PMMA)	Optically clear, weather and UV resistant, shatter resistant relative to glass. Brittle and notch sensitive.
ABS	Tough and impact resistant, including at low temperature. Easy to mold, paint, and plate. Poor outdoors without capping.
Nylon (PA)	High heat, abrasion, and fatigue resistance. Absorbs moisture, which moves dimensions after molding.
PBT	Creep resistant and dimensionally stable in thin sections. Common in electrical and connector parts.
Polycarbonate (PC)	Strong, light, naturally transparent, stable across a wide temperature range. Notch sensitive, so avoid sharp internal corners.
PEEK	Outstanding mechanical properties with chemical and thermal resistance. Cost per kilo decides most inquiries.
PEI (Ultem)	Stiff and stable with inherently low flammability and low smoke, without additives.
Polyethylene (PE)	Chemically resistant, available in high and low density grades. Difficult to bond or paint.
PPSU	High toughness, high flexural and tensile strength, resists repeated steam autoclaving.
Polypropylene (PP)	Good chemical resistance, unaffected by moisture, and the material of choice for living hinges. High shrinkage.
Polystyrene (PS)	Light, inexpensive, moisture and bacteria resistant. Brittle.
TPE	Processed like a plastic, behaves like a rubber. The usual overmolded grip material.
TPU	Rubber-like elasticity with good load bearing. Tougher and more abrasion resistant than most TPEs.

Filled grades change the calculation again. Adding glass or carbon fiber raises stiffness substantially but makes shrinkage directional, which means a filled part warps in ways an unfilled one does not, and the filler abrades the tool. Specify the exact grade, not the family.

Wall thickness

Uniform walls cool and shrink evenly. Where a section is thicker, it stays molten longer and continues contracting after the surface has frozen, pulling the surface inward as a sink mark.

Wall thickness is the single most consequential dimension on a molded part. It sets strength, cycle time, material cost, and cosmetic quality all at once.

Keep it uniform

A part with uniform walls cools evenly and therefore shrinks evenly. Where thickness varies, the thick sections stay molten longer, continue shrinking after the thin sections have frozen, and pull the surface in with them. That is the mechanism behind sink marks, voids, warp, and internal stress. Uniform walls are not an aesthetic preference; they are how you avoid four separate defect modes at once.

Keep it in range for the resin

Walls that are too thick waste material and lengthen cycle time, and both are paid on every part for the life of the tool. Walls that are too thin may not fill, producing short shots and trapped air. Each resin has a practical window. Treat these as the comfortable band rather than a hard limit: a thin-wall packaging part in PP runs below the bottom figure on a dedicated high-speed press, and a structural glass-filled part sits above the top one.

Resin	Recommended wall thickness
Acetal (POM)	0.75 – 3.0 mm
Acrylic (PMMA)	0.65 – 3.8 mm
ABS	1.1 – 3.5 mm
Nylon (PA)	0.75 – 3.0 mm
PBT	1.5 – 3.0 mm
Polycarbonate (PC)	1.0 – 3.8 mm
PEEK	0.5 – 5.0 mm
PEI (Ultem)	0.5 – 5.0 mm, by grade
Polyethylene (PE)	0.75 – 5.0 mm
PPSU	0.75 – 6.0 mm
Polypropylene (PP)	0.5 – 3.8 mm
Polystyrene (PS)	0.65 – 3.2 mm
TPE	0.65 – 3.2 mm
TPU	0.65 – 3.2 mm

Blend the transitions you cannot avoid

Where a change in thickness is genuinely required, do not step it. Blend it with a chamfer or, better, a fillet across a length of at least three times the thickness difference. An abrupt step is a stress concentration and a flow disturbance; a gradual transition is neither.

Corners and radii

Strike the internal and external radii from the same center point so the wall thickness stays constant around the corner. This is the detail most often missed.

Sharp internal corners concentrate stress, restrict flow, and force uneven shrinkage. They also raise tooling cost, because a sharp internal corner in the part is a sharp external corner in the steel that usually has to be produced by EDM rather than milling.

Make the internal radius at least half the nominal wall thickness.
Make the external radius equal to the internal radius plus the wall thickness.
Strike both radii from the same center point, so the wall thickness stays constant around the corner. This is the detail most often missed, and getting it wrong reintroduces the thick section you were trying to avoid.

Sharp corners are not always wrong. They are the right place for a parting line, because a parting line on a sharp edge is easier to seal and less visible. Use them deliberately rather than by default.

Draft

Without draft the part shrinks onto the core and grips it. One to two degrees is a working minimum on a smooth surface, and more on a texture.

Draft is the taper applied to faces parallel to the direction the tool opens, so the part can release. Without it, the part shrinks onto the core, grips it, and either scuffs or refuses to eject. Draft also reduces tool wear and shortens cooling time, so it pays for itself beyond simply making ejection possible.

Surface finish	Minimum draft
Smooth, unpolished	1 to 2 degrees
Light texture	3 degrees
Heavy texture	5 degrees or more

For textured surfaces the working rule is to add roughly 1.5 degrees of draft for every 0.025 mm of texture depth, on top of the base requirement. The finish standards published by SPI and VDI, and by texture houses such as Mold-Tech, each carry their own recommended draft tables, and the specific texture you choose should be selected before the tool is cut rather than after.

Draft direction matters as much as draft angle. The part must stay on the half of the tool that carries the ejector system, normally the core. If features are drafted toward the cavity instead, the part can stick in the wrong half and be damaged on every cycle. A rectangular part with through-holes, for instance, should have those holes drafted toward the core, not the cavity.

Ribs and bosses

Rib thickness at 50 to 60 percent of the nominal wall, height no more than 2.5 times the wall. Thicker ribs telegraph a sink mark onto the visible face opposite.

Molded parts have thin walls for good reasons, and thin walls are not stiff. Ribs and bosses restore strength without adding the mass that thick walls would.

Ribs

Thickness: 50 to 60 percent of the nominal wall. Thicker than that and a sink mark appears on the opposite face, directly in the visible surface.
Height: no more than 2.5 times the nominal wall. If you need more stiffness than one rib provides, use several shorter ribs rather than one tall one.
Base fillet: roughly 0.25 to 0.5 times the nominal wall, and not more than about 0.25 mm. Enough to relieve stress and help flow; not so much that it recreates a thick section.
Draft: at least half a degree per side, and more if the surface is textured.
Orientation: run ribs in the direction of expected load and, where possible, in the direction of flow.

Bosses

Keep boss wall thickness to no more than 60 percent of the nominal wall, for the same sink reason as ribs.
Support bosses with gussets or ribs rather than thickening them. A thick solid boss is a guaranteed sink mark.
Do not attach a boss directly to a side wall, which creates a thick junction. Stand it off and connect it with a rib.
Remember that the hole shrinks as it cools, so size the cored hole for the fastener or insert it will actually receive.
Where a boss takes a threaded insert or a self-tapping screw, check the hoop stress the insert will impose. A boss that is right for a screw is often wrong for an ultrasonic insert.

Tolerances

Every process varies, so the designer’s job is to state which variation is acceptable. In molding, tolerance is normally quoted in one of two bands: commercial tolerances, which most tools hold without special measures, and fine tolerances, which need a more precise tool, tighter process control, and more inspection, and which cost accordingly.

The cavity is cut larger than the drawing by the expected shrinkage of the resin, typically half a percent for an amorphous material and one and a half to two percent for a semi-crystalline one. Shrinkage is not uniform: it differs along and across the flow, and it changes with wall thickness, pack pressure and mold temperature. That is why the first tool is cut steel-safe and adjusted after the first samples.

A boss made solid is a thick section joined to a thin wall, and it will pull a sink mark onto the opposite face. Core it out so the wall of the boss is around six tenths of the nominal wall, then restore the stiffness with gussets running into the floor. The screw sees the same thread engagement and the show face stays flat.

Tolerance type	What it governs
Dimensional	Overall size of the part. Scales with the dimension, since shrinkage accumulates over length.
Straightness and flatness	Warp across large flat areas. Usually a symptom of uneven cooling rather than of tool accuracy.
Hole diameter	Larger holes need larger tolerances, because more shrinkage acts across them.
Concentricity and ovality	Large thin-walled cylindrical parts shrink unevenly and go out of round.

Tolerance also varies by resin, because shrinkage does. A dimension routine in POM may be unachievable in PP on identical geometry. And on any assembly, the individual tolerances are only half the question: the stack-up across mating parts is what determines whether a screw actually passes through three aligned holes. Analyse the stack before tightening any single dimension.

Parting lines, gates, and ejector pins

These three are decided in the tool, not the part, but they all leave marks on the part, and where those marks fall is a design decision you should make rather than inherit.

Parting lines

The parting line is where the two halves meet, and it leaves a faint witness line on the finished part. It does not have to run around the visual center of the part. Consider a molded brick with studs on top: the parting line sits along the bottom edges, where you have to turn the part over to see it. Place yours on a sharp edge, which simplifies the tool and seals well, and avoid running it across a filleted surface, which needs a tighter-tolerance tool and raises the risk of flash.

Anything that stops the two halves drawing straight apart is an undercut, and it is freed by a slide or a lifter that moves as the tool opens. Slides work, but they add cost, cycle time, maintenance and a witness line. Where a hole can be opened through to a surface so one half shuts off against the other, the feature is made by the tool closing and costs nothing.

Gates

The gate is where melt enters the cavity. Its size governs fill rate, so larger parts need larger gates. Its position governs where the flow fronts meet and therefore where weld lines form, where warp appears, and where sink and voids are most likely. It also leaves a vestige after trimming, so it belongs on a non-cosmetic surface, frequently along the parting line.

Gate	Trimming	Best suited to
Edge or standard	Manual	Flat parts. Rectangular cross-section, optionally tapered.
Fan	Manual	Large or fragile parts needing rapid, even filling.
Tab	Manual	Thin flat parts where shear stress must be confined away from the part.
Direct or sprue	Manual	Large cylindrical parts fed rapidly through a single sprue.
Disc or diaphragm	Manual	Round parts requiring concentricity. Difficult and costly to trim.
Ring	Manual	Tube-like parts, allowing material to flow freely before entering the cavity.
Spoke	Manual	Tube-shaped parts. Perfect concentricity is hard to achieve.
Hot tip	Automatic	Round or conical parts needing uniform flow. Requires a hot runner.
Submarine or tunnel	Automatic	Shears off on ejection and hides the blemish below the visible surface.
Pin	Automatic	Fast-flowing resins and cosmetic parts that cannot carry a vestige at the parting line.

Ejector pins

Ejector pins leave small circular witness marks, and those marks have to go somewhere. Plan for them rather than discovering them on the first samples.

Put pins on surfaces that will not be seen in use.
Distribute ejection force as evenly as the geometry allows, or the part deforms as it comes off.
Apply force where the part is strongest and stiffest, typically against ribs and bosses rather than open panels.
Avoid thin sections and sloped surfaces. A pin pushing on a slope tends to skid and mark.
Keep pins clear of the travel of any slides or lifters in the tool.

From design to production

Get DFM feedback before the tool is cut

The economics here are stark and worth stating plainly. While the part is still a model, a change costs minutes. Once steel has been cut, the same change costs days and real money, and if the correction requires adding material back into the cavity it may mean welding or a replacement insert. The DFM review is the cheapest engineering hour in the whole program.

A useful review answers specific questions rather than offering general reassurance: will the gate position leave a cosmetic defect, will the parting line be visible where it matters, will the ejector pins mar or damage the part, where will the flow fronts meet and form a weld line, and which specified tolerances are going to be difficult to hold.

Start with a single cavity

For a new product, a single-cavity tool is cheaper, quicker to cut, and easier to modify. Since a design commonly changes after the first samples, committing to a multi-cavity or family tool before the design is proven risks paying for cavitation you then have to re-cut. Once the design is genuinely frozen, multi-cavity and family tooling is the right way to bring unit cost down.

Review the samples properly

First samples exist to be measured, not admired. Perform functional testing and dimensional measurement against the drawing, and check the texture against the physical reference rather than a photograph, since light, medium, and heavy versions of the same pattern look very different in the hand. Where a change is needed, raise it as a formal engineering change so that what was altered and why is recorded against the tool.

Injection molding guide