Answers › Die casting vs molding

Die casting or injection molding: which process fits my part?

Reviewed by the JCH tooling team · Updated

Choose die casting when the part has to be metal: for heat conduction, stiffness at temperature, or shielding. Choose injection molding when plastic will do the job, because production plastic molds typically outlast aluminum die casting dies many times over and molded parts usually need no machining or coating. Volume and post-processing usually settle the close calls.

The quick sort

Most parts sort themselves on three questions before any detailed comparison is needed.

  1. Does the part have to be metal? If it must carry heat away, shield electronics, take high load at temperature, or meet a flame or creep requirement no plastic grade can, die casting is the starting point. If it needs to insulate, flex, come in color, or be clear, it's plastic.
  2. How many will you make over the life of the program? Die casting tools wear out much faster than plastic molds because they run molten metal at several hundred degrees. Low totals favor whichever tool is cheaper to build; high totals favor the tool that lasts.
  3. How much work happens after the part leaves the tool? Die castings commonly need trimming, machining of sealing faces and threads, and a coating. Molded plastic parts often need nothing.

Side by side

Die casting (aluminum, zinc, magnesium)Injection molding (thermoplastics)
Melt temperature in the toolZinc about 430 °C, magnesium about 650 °C, aluminum about 700 °C (ASSAB)Far lower; the tool runs well below metal-casting heat
Typical wall1.0 to 5.1 mm, depending on alloy and size; down to 0.5 mm on small castings with the caster's input (NADCA)Depends on resin, e.g. ABS 1.14 to 3.56 mm, polycarbonate 1.02 to 3.81 mm (Protolabs)
DraftCalculated by depth, alloy and feature; inside walls get about twice the draft of outside walls (NADCA)About 2° covers most situations; 0.5° is a common minimum on vertical faces (Protolabs)
Tool lifeAluminum dies about 60,000 to 200,000 shots; zinc about 0.5 to 2 million (ASSAB)SPI Class 101 molds are built for a million cycles or more; Class 103 for up to 500,000
What wears the toolHeat checking, cracking, erosion near the gateAbrasion from fillers, corrosion from some resins, ordinary wear
Usual secondary workTrim gates and overflows, machine critical faces and threads, coat or plateOften none; sometimes decoration, inserts or assembly
StrengthsStiffness, heat conduction, shielding, high-temperature strengthColor, low weight, insulation, snap fits, living hinges, clear parts

Why the draft rules look different

Both processes put a cooling material into a closed steel tool, and both need taper on faces parallel to the opening direction. The physics behind it is the same: as the part cools it shrinks, gripping any core it surrounds and pulling away from the walls around it. NADCA's draft method makes that explicit. Draft is calculated from the feature's depth, the alloy and whether it's an inside wall, an outside wall or a hole, with holes needing the most and outside walls the least. Plastic design guides usually give a simpler blanket figure and adjust for texture; the logic of draft angle carries over directly.

Why inside walls need more draft than outside walls: the part shrinks onto the core and away from the cavity cavity half (outside surfaces) core part wall outlined in blue; mold opens straight down Cooling metal or plastic shrinks. Inside walls and holes: the part grips the core, so they need the most draft. Outside walls: the part pulls away from the cavity, so they need less. NADCA standard draft, aluminum, feature 25 mm deep: inside wall about 1.9 deg, outside wall about half that.

Wall rules diverge more. Die-cast aluminum tolerates thicker sections than most plastics before it gets into trouble, and plastic parts generally want thinner, more uniform walls to avoid sink and warp; wall thickness for molded parts covers the plastic side. When a part is converted from one process to the other, the wall plan usually has to be redrawn, not just re-specified.

A closed injection mold mounted between the platens of a press, held by blue clamp blocks, with tie bars running past it.
A plastic injection mold clamped in its press. Die casting uses a similar press-and-tool arrangement, but the tool takes molten metal at several hundred degrees every shot, which is why an aluminum die's life is counted in far fewer shots than a production plastic mold's.

Worked example: a 40 mm deep electronics housing

Take a hypothetical housing, 150 by 100 mm and 40 mm deep, with 2.5 mm walls, planned at 150,000 parts over the life of the product.

As an aluminum die casting. A 2.5 mm wall sits comfortably inside NADCA's 1.0 to 5.1 mm typical range. Using NADCA's standard-tolerance draft formula for aluminum, a 40 mm deep inside wall needs about 1.06 mm of draft distance, which works out to roughly 1.5°; the outside walls need about half that, near 0.8°. Tool life is the catch. ASSAB gives 60,000 to 200,000 shots as the normal life of an aluminum die, so 150,000 parts may land inside one die's life or may need repair, replacement inserts or a second die, depending on the alloy, the part and how the die is run. The cost model should include that. Then add the post-cast work: trim the gates and overflows, machine the gasket face flat and tap the screw holes, and coat the outside; powder coating and metal finishing covers the last step.

As a molded plastic part. A 2.5 mm wall is inside the range Protolabs lists for ABS and polycarbonate. Draft of 1 to 2° on the 40 mm walls is normal. A steel production mold built to SPI Class 102 or 101 covers 150,000 shots with room to spare. Screw bosses, snap fits and the gasket groove can all be molded in, so the part may come off the press finished. What you give up is stiffness, heat spreading and shielding, which may mean ribs, a conductive coating or a metal shield inside.

So the choice for this housing turns on function. If the electronics inside dump heat into the walls, aluminum earns its extra tooling and machining. If they don't, plastic is usually simpler and cheaper per part at this volume.

When each one wins

When the answer is a third process

Small, intricate metal parts often fit neither well. For pieces of a few grams with fine features, metal injection molding may beat both. At low volumes, machining from bar avoids tooling altogether. And many products end up as a mix, a cast or machined metal core with a molded plastic shell; combining plastic and metal parts covers how those are coordinated. Whatever the process, run the drawing past a draft check early; the draft angle calculator is a quick first pass for the plastic side.

Common questions

Is die casting stronger than injection molding?

Die-cast aluminum and zinc are generally stiffer and stronger than unfilled plastics, and they keep that strength at higher temperatures. Glass-filled engineering resins narrow the gap for many brackets and covers. The right comparison is the specific alloy against the specific resin grade at the part's working temperature, not metal against plastic in general.

Why does a die casting die wear out faster than a plastic mold?

Every shot hits the die surface with molten metal hundreds of degrees hotter than the steel, then the surface is cooled again. That cycling causes heat checking, cracking and erosion near the gate. Aluminum dies wear faster than zinc dies because aluminum is cast much hotter.

Can a die-cast part be converted to plastic?

Often, if the part isn't relied on for heat conduction, shielding or high-temperature strength. The geometry usually needs redesigning: thinner, more uniform walls, ribs instead of solid sections, and features like snaps or bosses molded in. Prototype the plastic version and test it under real load and temperature before cutting a production mold.

Which process holds tighter tolerances?

Both can hold tight tolerances on well-designed features, but die castings usually have critical faces, bores and threads machined afterwards, which is how the tightest metal tolerances are reached. Molded plastic parts are usually used as molded, so their tolerances depend on resin shrinkage, wall design and process control.

Is zinc or aluminum better for die casting?

Zinc casts at a lower temperature, allows thinner walls and finer detail, and gives much longer die life, which suits small, detailed parts. Aluminum is far lighter for its size and is the common choice for larger housings and structural parts. The part's size, weight limit and volume usually decide it.

Sources

Send the part file and the quantity you expect to run, and we'll review it before you commit to tooling. NDA first if you want one.

Send a part for reviewBook a 30-minute call