AN-044 Build guides · cluster
Design for Manufacturing (DFM): The Working Guide
Design for manufacturing with real numbers: wall thickness, draft, ribs, tolerances and bend rules for molding, CNC and sheet metal, plus DFMA examples.
by the HardwareMap editors6 min read
Contents
Design for manufacturing (DFM) is shaping each part so its process can make it repeatably at your target cost: uniform walls and draft for molding, reachable corners for machining, bend-safe holes for sheet metal, and fewer parts overall. It is stage four of how to start a hardware company, and it decides unit cost and yield before a factory sees the files.
The rules below are numbers, not principles. Where a number comes from a process vendor's published guide, the guide is linked. Treat every number as a starting point: your factory's capability page and its DFM feedback on your actual part outrank any table.
Design for manufacturing rules by process
Sources: Protolabs design guidelines for injection molding, CNC milling and sheet metal, and the Protolabs Network SLS design guide. Printing gets its own note: design for additive manufacturing.
Injection molding DFM: walls, draft, ribs, bosses
Molding is where DFM pays most, because the mold is the most expensive thing you will buy and the hardest to change. The injection molding cost note covers the price side.
Uniform walls. Plastic shrinks as it cools. A thick section cools last and pulls the surface in, leaving a sink mark, or warps the part. Protolabs lists recommended wall ranges by resin: ABS 1.14 to 3.56 mm, polycarbonate 1.02 to 3.81 mm, nylon 0.76 to 2.92 mm, polypropylene 0.89 to 3.81 mm. Pick one nominal wall and hold it. Where the part must be thicker, core it out and add ribs.
Draft. Faces parallel to the mold's pull direction need a taper to release. Protolabs accepts 0.5° on vertical faces but recommends 2° for most situations, 3° for light texture and 5° or more for medium texture. The Protolabs Network injection molding guide adds a rule of thumb: on features taller than 50 mm, add one degree per 25 mm of height.
Ribs. Rib thickness at 0.5 times the main wall, height under three times the rib thickness, with a fillet at the base. A thicker rib prints its own sink mark on the cosmetic face opposite.
Bosses. Treat a boss as a rib closed into a circle. Tie it to a wall with ribs instead of merging it into one. For threaded inserts, make the boss outer diameter twice the insert size.
Undercuts. A straight-pull mold has two halves. A snap hook or side hole needs a side action, which adds cost and lead time. Move the parting line, use a pass-through core, or redesign the feature to face the pull.
Thinner is faster. The same guide notes that cutting a wall from 3 mm to 2 mm can cut cycle time by 50 to 75%. Cycle time is most of the per-part price on a running mold.
CNC machining and sheet metal DFM
CNC. A cutter is round, so internal corners take its radius. Design internal radii a little larger than the tool you expect, and avoid deep narrow pockets: Protolabs' automated milling reaches 50.8 mm from each side. Keep features above 0.51 mm and the nominal thickness above 1.02 mm. Hold the whole part to ISO 2768 medium and call out tighter tolerances only on mating features. Each tight callout adds a gauge, an inspection step and sometimes a second setup.
Sheet metal. A sheet metal part is one thickness throughout. Protolabs stocks 0.61 to 6.35 mm. Tolerance gets looser with every bend: ±0.13 mm between features on one face, ±0.38 mm across two bends, ±0.76 mm across three or more on thin stock. Put precision features on a single face, keep holes clear of bend lines so they do not stretch into ovals, and expect brake lines on cosmetic faces unless you specify a finish that hides them.
Boards. For printed circuit boards, DFM means designing to the fabricator's standard capabilities, not its extreme ones. Most fabs publish both, as JLCPCB does. Standard trace widths, via sizes and stack-ups cost less and yield better. The PCB assembly guide covers the assembly side: fiducials, panelization and component spacing for pick-and-place.
Design for manufacturing and assembly (DFMA)
Optimizing each part is half the job. Design for manufacturing and assembly asks how many parts there are and how they go together. Removing a part removes its tooling, its inventory line, its inspection and its assembly step.
A working DFMA checklist:
- Challenge every part. Does it move relative to its neighbor? Is it a different material for a reason? Must it come apart for service? If none apply, merge it with a neighbor.
- Cut fastener count and variety. Snap fits, bosses with heat-set inserts or one screw size across the product. A line that stocks one driver bit runs faster.
- Assemble from one direction. Top-down, with gravity, so the unit never flips on the fixture.
- Make wrong assembly impossible. Asymmetric keys, offset pins and connectors that only fit one way.
- Design the test in. Test points on the board, a programming header reachable through the housing, a fixture location on the enclosure.
Score the result with two numbers: total part count and total assembly operations, counted from the manufacturing bill of materials. Both should fall with every design pass. If a change adds a part, it should remove a step somewhere else, or buy a function a customer pays for.
How to run a DFM review
A DFM review is a meeting with a document, not a conversation. Run it in this order:
- Freeze the process per part. Write the process, material and finish next to each line of the BOM before the review. A part without a process cannot be reviewed.
- Send the factory native CAD plus drawings. STEP for geometry, a PDF drawing for tolerances, finishes and critical-to-function dimensions. A drawing that marks five critical dimensions gets a better review than one that tolerances all two hundred.
- Get written feedback per part. Most molders and machine shops return a DFM report with the quote: draft warnings, thick sections, undercuts, unreachable corners. Online services generate one automatically on upload.
- Log each finding with an owner and a decision. Accept, reject with reason, or change. Rejected findings come back as defects at EVT, so a written reason saves an argument later.
- Re-review after every change that touches tooling. A moved boss changes the mold flow. A new hole changes the bend sequence.
Expect two or three loops on a molded part. Each loop costs a few days in CAD. Skipping one costs a mold change, which the prototype to production note places at DVT, where it hurts most.
Design for manufacturing examples from the index
One part redesigned. A 4 mm-thick ABS enclosure lid, flat, with 0° side walls and four molded screw threads. DFM pass: wall to 2 mm with ribs at 1 mm under the flat face, 2° draft on the side walls, threads replaced by bosses with brass heat-set inserts. The mold loses its side actions, cycle time drops with the thinner wall, and the cosmetic face stops showing sink. The injection molding tooling cost note shows what side actions add to a quote.
A process chosen for change. Prusa Research prints the plastic parts for its own printers on an in-house print farm. Prusa says the farm runs around 700 printers and that a part improvement can reach shipping printers within hours of a new G-code upload. That is a DFM decision: at its volumes, Prusa traded molding's lower unit cost for zero tooling and same-day design changes.
An interface designed to outlive the board. Framework designed its laptop chassis so that several generations of mainboards drop into older units. The mechanical interface, mounting points and connector positions were fixed as a product constraint, so every new board is a DFM problem with fixed outer boundaries.
Frequently asked questions
What is design for manufacturing (DFM)?
Design for manufacturing is the practice of shaping a part so a chosen process can make it repeatably at target cost. It means designing to the process limits: wall thickness and draft for molding, tool access and corner radii for machining, bend radii and hole spacing for sheet metal. A DFM review is the check a factory runs on your files before it quotes or cuts tooling.
What is the difference between DFM and DFMA?
DFM looks at each part and asks whether its process can make it well. DFMA, design for manufacturing and assembly, adds the assembly line: how many parts there are, how many fasteners, which direction each part goes in, and whether an operator can install it wrong. DFMA often removes parts entirely, which saves more than optimizing any single part.
When should a hardware startup do a DFM review?
Run an informal review against the process rules while designing, then a formal review with the factory before EVT parts are ordered and again before production tooling is cut. Most molders and machine shops return automated or engineer-written DFM feedback with a quote. Changes are nearly free in CAD, cheap at EVT, and expensive once a steel mold exists.
What are common design for manufacturing examples?
Replacing a sharp internal corner with a radius so a cutter can reach it. Adding 2 degrees of draft so a molded part ejects without drag marks. Coring out a thick section to a uniform wall to stop sink marks. Swapping four screws for snap fits. Moving a hole away from a bend in sheet metal so it does not distort. Each one trades a little design freedom for yield.
What tolerance should I put on my drawings?
Use a general tolerance block such as ISO 2768 medium for non-critical dimensions, and call out tighter tolerances only where function needs them. Protolabs quotes plus or minus 0.13 mm as typical for machined parts and plus or minus 0.08 mm plus material shrink for molds. Every tighter tolerance adds inspection time and cost, so justify each one.
HardwareMap catalogues the companies that turned prototypes into parts a factory can make. Building one? Submit it and get a part number.
Building one?
Submit it to the index and get a part number. Every entry is reviewed by hand.