How should I design plastic injection molded parts to reduce production costs?
- Share
- Issue Time
- Jul 10,2026
The short answer
Cut injection molding cost by fixing the part design before the tool is cut. Keep walls uniform at 1.5 to 3 mm, pull 1 to 3 degrees of draft, radius every corner at half the wall, and remove undercuts needing side actions. These changes typically cut tooling 20 to 40 percent and cycle time 15 to 25 percent.
Where injection molding cost is actually decided
Most of the cost of a moulded part is committed long before a machine runs, because tooling structure, cycle time and scrap rate are all consequences of geometry. A wall that is thicker than it needs to be adds cooling time to every cycle for the life of the program; an undercut adds a slide that has to be built, maintained and replaced; a mirror finish adds hours of hand polishing to the tool. Buyers who treat design as free and tooling as the cost get the arithmetic backwards, since the design decisions are what the tooling and the cycle price is built from.
The levers are few and well understood. Wall thickness and uniformity set cooling time and therefore machine cost per part. Draft, radii and the parting line decide whether the part ejects cleanly or is dragged out of the cavity. Undercuts decide how many moving components the tool needs. Ribs and bosses decide how much material the part uses and whether it sinks. And tolerance, texture and mold class decide how much precision is paid for that the part may never use. Worked in that order, they compound; worked in the wrong order, each one re-opens the last.
Wall thickness: the rule that sets cooling time
Uniform wall thickness is the single highest-value design rule in injection molding. Recommended thickness is 1.5 to 3 mm for most thermoplastics, held uniform within roughly 10 to 25 percent, because plastic shrinks as it cools and a thick section shrinks more than a thin one. The result of an uneven wall is a sink mark on the cosmetic face, a warp that closes a flatness callout, or an internal void that only shows up in a pressure test. Where a thickness change cannot be avoided, the transition should be gradual — a taper over at least three times the thickness change — rather than a step.
The cooling arithmetic explains why this matters so much. Cooling time scales with the square of wall thickness, so doubling a wall roughly quadruples the time that section needs in the mold, and the whole cycle waits for the thickest point. Studies of cycle time put uniform-wall designs 15 to 22 percent faster than non-uniform ones, with material savings around 18 percent and scrap falling from roughly 8 percent to about 2.5 percent on a part that was previously sink-marked. Thinning a wall from 3.5 mm to 2.2 mm and adding ribs, in one published case, cut cooling time from 28 seconds to 21 seconds and material use by 21 percent.
Draft, radii and the parting line
A vertical wall with no draft is a wall that has to be dragged out of the mold, and the damage shows as scuffing, drag marks and a tool that wears faster than it should. The working rule is at least 1 degree of draft on textured surfaces and 0.5 to 1 degree on polished ones, with roughly 1 degree added for every 0.025 mm of texture depth, because a texture that is deep enough to look like leather will hold the part unless it is drafted out. Draft costs nothing at the design stage and is expensive to add after the steel is cut, since it usually means welding and re-cutting a cavity surface.
Radii go with draft. Every internal corner should carry a radius of at least half the local wall thickness, because a sharp internal corner is a stress concentration and a flow restriction at the same time. A radiused corner fills more evenly, cools more evenly and carries load into the surrounding wall rather than cracking at the point where the two walls meet. The parting line then has to be placed where it lands on a non-cosmetic surface if possible, because it is the one artifact that a simple set of polishing stones cannot remove.
Undercuts and side actions: the biggest single lever
An undercut is a feature that cannot be released in the direction the mold opens, so it needs a slide, a lifter or a collapsing core. Each of those adds a moving component to the tool, and each moving component adds cost at three points: it has to be built, it has to be maintained, and it lengthens the cycle every time it strokes. Published planning figures put the tooling premium for an undercut at 30 to 100 percent, with each additional side action, lifter or threaded core adding roughly 2,000 to 15,000 US dollars and 5 to 20 seconds to the cycle. A simple two-plate tool with straight-pull geometry might cost 8,000 dollars and run a 15 second cycle; the same part with two side cores and a threaded feature could cost 28,000 dollars and need 35 seconds.
Removing them is worth real money. In one documented redesign, deleting two side undercuts took a tool from 28,500 to 18,200 dollars, a 36 percent reduction, and cut the cycle from 42 seconds to 34. Redesigning four lifters down to one cut tool cost by about 45 percent and made production 22 percent faster. If an undercut is genuinely required, put it on the outside wall, where an external slide is cheaper and simpler than an internal lifter, and keep it off the cosmetic face.
Ribs and bosses: strength without sink marks
A rib adds stiffness far more cheaply than a thicker wall, provided the rib itself is proportioned so it does not simply create the sink mark it was meant to avoid. The working proportions are a rib thickness of 0.5 to 0.6 times the base wall, a rib height of 2.5 to 3 times the base wall, and spacing of at least twice the base wall between ribs. The corresponding rule for bosses is a wall of 0.5 to 0.6 times the base wall, with a radius at the base and gussets to the nearest wall rather than an increase in the boss diameter. Every one of these is a local thickness decision, and local thickness is what drives sink.
The material saving is the second benefit and it is not small. Converting a solid section to a ribbed one commonly removes 15 percent of the part weight, which comes straight off the material cost, and it reduces the thick region that would otherwise dominate the cooling time. On a part made in millions the material line is a large share of unit cost, which is why a ribbed design that looks more complex on the drawing is often the cheaper part to run.
Tolerances, texture, mold class: what to stop over-specifying
Tolerance is the most commonly over-ordered feature on a moulded part. Plastic moves with shrinkage, moisture and temperature, so calling a tight tolerance on a non-functional dimension buys nothing except rework; a realistic target for feature position on a commodity resin is in the region of plus or minus 0.1 mm, with a formal tolerancing scheme such as an ISO 20457 grade agreed where the drawing needs one. The engineering habit worth building is to tolerance only what mates with something else, and to let everything else sit at the general tolerance block.
Finish and mold class follow the same logic. A mirror polish requires several hours of hand work per cavity and adds roughly 1,000 to 5,000 US dollars to a tool, while a fine matte finish off a standard spark-eroded surface costs nothing extra — and a moulded-plastic matte can be indistinguishable from a polished surface on a part nobody touches. Mold class matters as much: a tool built for a million-plus shots can cost three to five times a class intended for under 100,000, so a program below that volume is usually better served by the lighter class. Specifying to the volume, rather than to the ambition, is the last and often the largest saving available.
Five numbers then capture most of the available saving on a typical part. Wall thickness: 1.5 to 3 mm and uniform within about a quarter of the nominal. Draft: at least 1 degree on textured walls, 0.5 to 1 degree on polished ones. Corner radius: at least half the local wall thickness at every internal corner. Rib proportion: 0.5 to 0.6 of the base wall in thickness, 2.5 to 3 times in height. And tolerance: a realistic general tolerance with tight values reserved for mating features, plus a finish and mold class chosen against the actual annual volume rather than the worst case.
Worked in sequence, those five decisions typically remove 20 to 40 percent of tooling cost and 15 to 25 percent of cycle time, and well-run DFM programs report defect rates below 1 percent and far fewer mold modifications after the first sample. The order matters. Fix the wall before the draft, because changing the wall changes everything downstream; fix the undercuts before the tolerance, because removing a side action can release a dimension that no longer needs a tight callout. A DFM review that runs after the steel is cut is not a review, it is a change order.
Where design-for-cost is the wrong conversation
Optimising cost can go too far in five places. A part that will be sterilised, chemically cleaned or used outdoors may need a thicker or a different wall, and thinning it for cycle time is a false saving. A cosmetic face may genuinely need a specific texture or a mirror grade, in which case the polishing cost is a product requirement rather than an over-specification. A ribbed design can be cheaper in material and dearer in tooling if the ribs add side actions, so the two levers have to be costed together rather than separately. A wall thin enough to need high injection pressure can force the tool into a larger machine, which costs more per hour than the material it saved. And a tolerance loosened to save rework is a bad trade if the part then fails to assemble, because the assembly line is a more expensive place to discover a dimension.
Three limits are worth stating on any brief. Material is only part of the unit cost — machine time, tool amortisation, scrap and secondary operations usually matter more, so a design decision should be evaluated on the total rather than on the resin line. Cycle time improvements from thinner walls flatten out once the part is thin enough that pack and hold dominate the cycle, so the last millimetre is rarely the one that pays. And every cost decision interacts with quality: the cheapest geometry that meets the requirement is the goal, not the cheapest geometry that can be moulded at all.
See injection molding for the process family these rules apply to, plastic injection molding for the service that builds the tool, and FDM 3D printing for validating a geometry before the tool investment is committed.
Scope and sources. The cycle time and tooling saving table — simple geometry 20 percent cycle and 15 percent cost, uniform wall thickness 15 percent cycle and 10 percent cost, draft angles 25 percent cycle and 5 percent cost, parting line 10 percent and 8 percent, ribs and supports 5 percent and 12 percent, minimising undercuts 30 percent cycle and 20 percent cost, material selection 10 percent and 15 percent, cooling efficiency 20 percent and 25 percent, venting 15 percent and 10 percent, and simulation 5 percent and 5 percent — the draft angle of 1 to 2 degrees, the plus or minus 0.1 mm tolerance note and the observation that up to 30 percent of project time goes on revisions come from a design efficiency study. The wall thickness band of 1.5 to 3 mm with cooling time scaling as the square of thickness, the 4x cooling penalty of a 3 mm wall against a 2 mm wall, the 1.5 to 3 mm design range, the draft minimums of 1 degree on textured and 0.5 to 1 degree on polished surfaces, the undercut tooling premium of 30 to 100 percent and the 20 to 40 percent tooling and 15 to 25 percent cycle-time savings come from the same DFM design guide, which also documents the 3:1 gradual transition rule for a wall change. These replace the unsourced illustration and market claim that appeared in an earlier version of this answer. The worked redesigns — two undercuts removed for a 36 percent tool cost cut and a cycle from 42 to 34 seconds, four lifters reduced to one for 45 percent and 22 percent, and uniform 2.2 mm walls giving 21 percent less material and a cooling time from 28 to 21 seconds — together with the figure that up to 70 percent of moulding cost is fixed at the design stage, the side-action premium and the second-operation and scrap figures come from a design optimisation study. The cost per side action of 2,000 to 15,000 US dollars and 5 to 20 seconds of cycle, the two-plate versus two-side-core comparison of 8,000 dollars at 15 seconds against 28,000 at 35 seconds, the mirror polish premium of 1,000 to 5,000 US dollars for 8 to 16 hours of hand work, the class 101 to class 104 cost ratio of three to five times and the volume table from cycle optimisation to material substitution come from an injection molding cost breakdown. The DFM targets of wall fluctuation within plus or minus 10 percent, draft increments of 1 degree per 0.025 mm of texture, a rib thickness of 40 to 60 percent of the base wall, an internal radius of 0.5 times the local wall, a 30 percent or better weld-line strength gain from gate placement, an ISO 20457 grade 7 tolerance reference, the conformal cooling distance of 1.5 to 2.0 times the channel diameter and the defect rate below 0.8 percent come from a DFM design guide. All cost figures are planning ranges for a quotation discussion, and the savings are cumulative guidance rather than guarantees on any particular part.