← Journal Design · · 6 min

Designing for injection moulding before you have a mould budget

How we prototype enclosures with SLS and CNC while keeping walls, ribs and bosses ready for injection moulding when the tooling budget arrives.

Milo Perović
Founder & lead engineer

  • DFM
  • Enclosures
  • Manufacturing
  • SLS
Designing for injection moulding before you have a mould budget

Most hardware start-ups reach the enclosure question at an awkward moment: the electronics work, a pilot customer wants units, and nobody has budgeted for steel tooling. This post is for founders and engineers who will eventually go to injection moulding but need to build the first ten, fifty or two hundred enclosures some other way.

The trap is designing for whatever process makes the prototype. A housing drawn for SLS or CNC usually has to be redrawn for a mould, and the redraw tends to move bosses, change wall thickness and break the PCB fit you spent months validating. We prefer one geometry that is mould-ready from the first print.

Why prototype processes hide moulding problems

SLS and CNC are forgiving in exactly the places a mould is not. A printed nylon part has no draft, no ejector pins, no parting line and no sink marks. It does not care whether a wall is 1.2 mm or 4 mm thick. Everything looks fine until a toolmaker reviews the files and returns a list of changes.

CNC fails in the opposite direction. It cannot cut sharp internal corners, struggles with deep, thin ribs and charges heavily for every pocket. Designers then simplify the part to suit the cutter, and the simplified part is often worse for moulding too. Neither process will warn you, so the discipline has to sit in the CAD model rather than in the prototype.

What injection moulding needs from the geometry

A handful of rules cover most of what a toolmaker will ask about. The figures below are typical starting points for common enclosure plastics such as ABS, PC and PC/ABS. Your moulder and resin datasheet have the final word.

  • Uniform nominal wall. Around 1.5–3 mm suits most handheld and wall-mounted enclosures. Pick one value and hold it; where thickness must change, blend it gradually rather than stepping it.
  • Draft on every face parallel to the opening direction. 1–2° is a comfortable default, with 0.5° as a practical minimum on smooth surfaces. Textured faces need considerably more, roughly an extra degree for every 0.025 mm of texture depth; the texture supplier will quote exact values.
  • Ribs thinner than the wall. Keep rib thickness to roughly 50–60% of the nominal wall to avoid sink marks on the cosmetic side, with height up to about three times the wall.
  • Cored-out bosses. Screw bosses should be hollow, tied to the nearest wall with ribs, with their own wall at around 60% of nominal.
  • Radii on internal corners. At least half the wall thickness inside, with the outside radius equal to inside radius plus wall. This helps flow and removes stress concentrations.
  • No accidental undercuts. Every hook, side hole or latch that cannot pull straight out of the mould needs a side action or lifter, and each one adds cost and lead time.

None of this makes the part harder to print or machine. Draft and radii cost nothing in SLS, and a uniform wall usually makes a CNC part cheaper. That is why we apply the rules from the first sketch rather than at handover.

Keeping the CAD model mould-ready

We treat the enclosure as a single master model with a few derived variants, not as separate prototype and production designs.

Model draft from the start

Draft is far easier to add while features are simple than after fillets, ribs and bosses are layered on. We set a pull direction and a parting line early, then build every feature with draft applied. A draft analysis colour map before each print run catches faces that slipped through.

Drive the wall from one parameter

Nominal wall, rib ratio and boss dimensions all reference a single parameter. If the moulder later asks for 2.2 mm instead of 2.0 mm, the change propagates without hand-editing dozens of features, and the PCB clearances update with it.

Derive prototype variants, do not fork them

Some changes are genuinely process-specific: thicker snap hooks for printed nylon, or heat-set insert holes in place of thread-forming screw bosses. We keep these as configurations of the master rather than as edits to it, so the production geometry stays intact and the differences are documented.

Choosing the right bridge process

Before steel tooling, there are several ways to make parts. Each one teaches you something different about the design.

ProcessTypical quantityGood forWatch out for
SLS (PA12)1–200Fit checks, internal layout, field pilotsPorous, grainy surface; snap fits behave differently from moulded parts
CNC (ABS, PC, POM)1–50Cosmetic samples, real material propertiesTool radii in corners; cost rises fast with pockets and ribs
Vacuum casting10–100 (around 20 per silicone mould)Near-production look, colour and texturePolyurethane resins only approximate the final plastic
Aluminium soft toolingHundreds to thousandsReal moulded parts in the production resinTool life and design-change cost; still a commitment

Quantities vary with part size, tolerance and supplier. The useful question is not which process is cheapest per part, but what each batch needs to prove. A field pilot proves the layout and sealing concept; a cast batch proves colour and finish; soft tooling proves the part actually moulds.

What a printed prototype cannot tell you

Founders often read a successful SLS pilot as proof the enclosure is finished. Several properties only appear once real resin is in a real mould:

  1. Shrinkage and warp. ABS and PC typically shrink around 0.4–0.7%, while semi-crystalline resins such as PP can shrink well over 1%. Long, flat lids are the usual victims.
  2. Cosmetic defects. Sink, weld lines, gate marks and ejector witness marks depend on gate position and wall uniformity.
  3. Snap-fit behaviour. A hook tuned in printed nylon may crack or feel loose in PC/ABS because stiffness and elongation differ.
  4. Gasket compression. If the enclosure targets an IP rating, compression across a moulded, slightly warped lid is not the same as across a printed one.

We record these as open risks in the bench notes rather than pretending the prototype closed them. They are cheap to discuss now and expensive to discover at first shots.

Talking to a moulder before you can pay one

A DFM review from a toolmaker is often free or cheap when you share a quotation package, and it is the best single check on a mould-ready design. Send them a STEP file, the intended resin and colour, the cosmetic faces marked, target quantities and any texture specification. Ask for gate and ejector locations, a list of undercuts, and a tool quote with and without side actions.

Material and finish choices belong in the same conversation. Our post on CMF design decisions that survive manufacturing covers which colour and texture decisions to lock early and which to leave open.

What we would do

If you are starting an enclosure with no mould budget yet, this is the short version of our approach:

  • Choose the production resin family and pull direction before drawing features.
  • Set one nominal wall parameter and drive ribs and bosses from it.
  • Apply draft and radii everywhere, even though the printer does not need them.
  • Keep prototype-only changes as documented configurations, never edits to the master.
  • Pick each bridge batch for what it proves, not for unit price.
  • Get a moulder’s DFM review before the design freezes, not after.

Done this way, the jump to steel is a tooling order rather than a redesign. If you want to see how enclosure work fits alongside PCB, firmware and testing, our services page sets out the full scope.

Working on something similar?Free scoping call →