Fused Deposition Modeling (FDM)
Fused deposition modeling extrudes molten thermoplastic filament along programmed paths so each layer welds to the one beneath it.
- Part
- Forming
- Revised
- 2026-08-11
At a glance
- Family
- Additive Manufacturing
- Typical tolerances
- ±0.020 in (±0.5 mm) or ±0.5% of nominal, whichever is greater, on desktop-class machines. Industrial systems hold ±0.008 in (±0.2 mm) or ±0.002 in/in. Drilled and reamed features are far tighter.
- Surface finish
- Ra 200–1,000 µin (5–25 µm), with visible layer lines whose spacing equals the layer height. Sanding, vapor smoothing (ABS in acetone), or filler primer are needed for a cosmetic finish.
- Typical volumes
- 1–500 parts
- Lead time
- 1–5 business days; small parts print in 1–4 hours and a full plate in 10–30 hours. No tooling, so the first part ships as fast as the last.
- Materials
- Plastic, Composite
What it is
Fused deposition modeling (FDM), also called fused filament fabrication, extrudes molten thermoplastic filament through a heated nozzle — 0.4 mm is the standard size — and lays it down path by path so each 0.002–0.016 in (0.05–0.4 mm) layer welds to the one beneath. It is the cheapest and most widely available additive process, and the only common one that uses genuine engineering thermoplastics: PLA, PETG, ABS, ASA, nylon, polycarbonate, and on industrial machines PEI (ULTEM) and PEEK.
The trade-off is anisotropy. Bonds between deposited roads are weaker than the filament itself, so Z-axis tensile strength typically runs 30–70% of the XY value. Accuracy is the loosest of the mainstream processes at roughly ±0.020 in (±0.5 mm) or ±0.5% of nominal, whichever is greater, on desktop machines; industrial systems reach ±0.008 in (±0.2 mm).
FDM suits jigs, fixtures, housings, ducting, and functional prototypes from 1 to a few hundred parts, with build volumes from 200 mm cubes to 36 × 24 × 36 in (914 × 610 × 914 mm).
How it works
- Slice and plan tool paths. The model is sliced at 0.002–0.016 in (0.05–0.4 mm) — 0.008 in (0.2 mm) is the usual default — and each layer is decomposed into perimeters (typically 2–4), solid top and bottom skins, and a sparse infill of 15–40%.
- Heat and prime. The nozzle reaches material temperature and the bed is heated to control first-layer adhesion and warp: roughly 190–220 °C (375–430 °F) nozzle with a 50–60 °C bed for PLA, 230–250 °C (445–480 °F) with a 100–110 °C bed for ABS and PETG, and 260–310 °C for polycarbonate. High-temperature materials such as PEI 9085 need a heated chamber above 160 °C (320 °F).
- Extrude the first layer. The first layer is deliberately squashed against the bed. Get this wrong and nothing else matters — first-layer squish also produces the "elephant foot" flare of 0.1–0.2 mm that shows up on close-fitting bases.
- Build up layers. The head traces perimeters and infill; the platform or gantry indexes one layer height. Extrusion width is normally 100–120% of nozzle diameter, so a 0.4 mm nozzle lays roads about 0.42–0.48 mm wide.
- Print supports. Overhangs beyond about 45° from vertical need support, either the same material (breakaway) or a dissolvable one such as HIPS or PVA on dual-extruder machines.
- Cool and remove. Amorphous materials such as ABS and PC shrink 0.4–0.8% on cooling and warp when cooled unevenly, which is why they need an enclosed chamber. Semi-crystalline nylons need dry filament — nylon absorbs moisture from air within hours and prints with visible bubbles.
- Post-process. Remove supports, drill and ream critical holes, tap threads or install heat-set inserts, and sand or vapor-smooth cosmetic surfaces.
Design guidelines
Wall thickness
Design walls as a multiple of extrusion width. With a 0.4 mm nozzle, 0.032 in (0.8 mm) equals two perimeters and is the practical minimum; 0.048–0.063 in (1.2–1.6 mm) gives three or four perimeters and is where structural walls should sit. A wall specified at 1.0 mm forces the slicer to fill an awkward 0.2 mm gap with a weak thin extrusion.
Overhangs and bridges
Anything overhanging more than about 45° from vertical needs support. Unsupported bridges span up to roughly 0.4 in (10 mm) reliably if both ends are anchored. Chamfer or fillet overhanging edges to 45° and you can often delete supports entirely.
Holes
Printed holes come out 0.004–0.016 in (0.1–0.4 mm) undersize because of extrusion width compensation and corner cutting. Drill and ream any hole that locates something. Horizontal holes should be drawn as teardrops or hexagons so the top does not need support.
Orientation and anisotropy
Orient the part so the principal tensile and bending loads act in the XY plane. Layer-to-layer bonds carry 30–70% of the in-plane strength, so a printed hook loaded along Z will fail at a layer boundary. Where load direction cannot be controlled, increase perimeter count rather than infill.
Threads and inserts
Do not print threads below M6. Use heat-set brass inserts (the cleanest option in FDM), or drill and tap — see the tap drill chart for pilot sizes and the thread size chart for the corresponding major diameters.
Fits and clearances
Allow 0.008–0.012 in (0.2–0.3 mm) per side for a slip fit and 0.016 in (0.4 mm) for a free-running fit. Add a 0.02 in (0.5 mm) chamfer at the base of mating features to clear the elephant-foot flare.
Minimum features
The nozzle diameter sets the floor: 0.016 in (0.4 mm) for a standalone rib or pin, embossed text at 0.02 in (0.5 mm) line width and 0.12 in (3 mm) cap height. Engraved text reads better than embossed at small sizes.
| Feature | Recommended | Limit | Why |
|---|---|---|---|
| Wall thickness | 0.048 in (1.2 mm) | 0.032 in (0.8 mm) | Multiples of a 0.4 mm extrusion width |
| Overhang angle | 45° from vertical | 60° with cooling | Each road needs the one below for support |
| Unsupported bridge | 0.2 in (5 mm) | 0.4 in (10 mm) | Molten road sags between anchors |
| Hole diameter | 0.12 in (3 mm), then ream | 0.08 in (2 mm) | Printed holes run 0.1–0.4 mm undersize |
| Layer height | 0.008 in (0.2 mm) | 0.004 in (0.1 mm) cosmetic | Time scales inversely with layer height |
| Clearance, moving | 0.016 in (0.4 mm) | 0.008 in (0.2 mm) | Extrusion overshoot closes tight gaps |
| Pin or rib | 0.08 in (2 mm) | 0.032 in (0.8 mm) | Two-perimeter minimum for stiffness |
Cost drivers
FDM cost is almost entirely machine hours. Print time scales with the number of layers times path length, so height and solid volume both matter, but layer height is the strongest single lever: doubling from 0.004 in (0.1 mm) to 0.008 in (0.2 mm) roughly halves the build.
Material is secondary on desktop-class work — PLA, PETG, and ABS filament are commodity-priced by the kilogram — but rises sharply for polycarbonate, nylon composites, and especially PEI and PEEK, which also demand a high-temperature machine. Support material and the labor to remove it are a real line item on parts with deep internal overhangs; dissolvable support trades that labor for tank time.
Volume breakpoints: FDM is normally the cheapest route for 1–50 parts. Between 50 and 500, look at SLS or MJF, which produce better parts at similar unit cost once the build is packed. Above about 1,000 parts, injection molding wins.
- Increase layer height on non-cosmetic parts — the single biggest time saver.
- Reduce infill to 15–20% and add perimeters instead; perimeters carry most of the bending stiffness.
- Orient the part to eliminate supports before adding them.
- Split large parts at natural seams and bond them, rather than paying for a tall build.
- Stay on commodity materials unless a specific thermal or chemical requirement forces PC, nylon, or PEI.
Questions
6 questionsWhat tolerance can FDM hold?
Desktop-class FDM holds about ±0.020 in (±0.5 mm) or ±0.5% of the dimension, whichever is greater. Industrial systems with heated chambers reach ±0.008 in (±0.2 mm) or ±0.002 in/in. If a hole or shaft needs to be tighter, print it undersize and drill or ream it.
Why are FDM parts weaker in the Z direction?
Each deposited road bonds to the layer below by partial remelting, and that weld is smaller than the road's own cross-section. Z-axis tensile strength typically lands at 30–70% of the XY value, so parts should be oriented with the main load in the print plane.
What is the minimum wall thickness for FDM?
0.032 in (0.8 mm), which is two perimeters at a standard 0.4 mm nozzle. Use 0.048–0.063 in (1.2–1.6 mm) for structural walls. Always specify wall thickness as a multiple of extrusion width so the slicer does not leave a weak partial gap.
What overhang angle can FDM print without support?
About 45° from vertical is the reliable limit; good part cooling stretches it toward 60° on small features. Horizontal bridges span up to roughly 0.4 in (10 mm) when both ends are anchored. Chamfering overhanging edges to 45° often removes the need for support entirely.
How do you get threads into an FDM part?
Heat-set brass inserts are the most reliable option: print a straight pilot hole and melt the insert in with a soldering iron. Tapping directly into the plastic works down to about M6 but strips more easily. Printed threads below M6 are not worth attempting.
Why does my ABS part warp or crack at the corners?
ABS shrinks roughly 0.4–0.8% as it cools, and uneven cooling puts the lower layers in tension. Print it in an enclosed, heated chamber with a bed at 100–110 °C (212–230 °F), add generous corner fillets, and avoid large flat first layers. PETG or ASA warp less if the chamber is not available.