Design for 3D printing comes down to five things: walls thick enough for the process, overhangs the process can build, holes and gaps it can resolve, clearances that let parts fit, and an orientation that balances strength, surface and print time. Each process has different limits, so a part that prints perfectly in SLS can fail in FDM. The table below gives typical starting values for FDM, SLA, SLS and MJF.
Key points
- Every limit depends on the process, the machine and the material. Use the table as a starting point, then confirm with your supplier.
- FDM and resin need support under overhangs; SLS and MJF do not, because the powder holds the part.
- Hollow parts need escape holes for resin or powder, or the trapped material is paid for and stays inside.
- Holes and clearances print tighter than drawn on most processes. Design the gap, then test it.
- Orientation sets height, support, surface and strength at once. It is a cost decision, not a detail.
Why does design for 3D printing matter?
Design for manufacturing is cheapest before the file is sent. A wall too thin to print, a cavity that traps powder or an overhang with no support is visible in the geometry, and catching it then costs a minute. Catching it after a failed build costs the machine time, the material and the delivery date.
Printing has fewer constraints than moulding or machining. There is no tool to release and no cutter to reach into a corner. But it has its own rules, and they differ by process. If you are still choosing a process, the FDM vs SLA vs SLS comparison is the place to start.
Typical design limits by process
These are typical starting points drawn from common practice, not guarantees. Machines, materials and layer heights move them, and your supplier’s own limits always take precedence.
| Rule | FDM | SLA and other resin | SLS | MJF |
|---|---|---|---|---|
| Minimum wall | About 0.8-1.2 mm, ideally a multiple of the extrusion width | About 0.5 mm supported, about 1 mm free-standing | About 0.7-1 mm | About 0.5-1 mm |
| Overhangs | Up to about 45° from vertical without support | Supported; low angles and islands need supports | No supports needed | No supports needed |
| Smallest hole | About 2 mm; small vertical holes print undersize | About 0.5-1 mm | About 1.5 mm | About 1-1.5 mm |
| Clearance between moving parts | About 0.3-0.5 mm | About 0.1-0.3 mm | About 0.3-0.5 mm | About 0.4-0.6 mm |
| Hollow parts | Usually printed with infill instead | Drain holes needed to empty resin | Escape holes needed to remove powder | Escape holes needed to remove powder |
| Main orientation concern | Strength across layers, support, bed contact | Support marks, peel forces, suction cups | Packing, thermal distortion of large flat areas | Packing, thermal distortion of large flat areas |
For a closer look at walls alone, including metal printing, machining and moulding, see the minimum wall thickness guide.
Walls: how thin is too thin?
A wall below the process minimum may not print at all, may print with holes, or may print and then break in handling. On FDM, walls are built from perimeters, so the useful wall thicknesses are multiples of the extrusion width. A wall slightly thicker than two lines but thinner than three leaves a gap the slicer either fills with a thin wiggle or leaves empty.
On resin, thin walls warp as they peel off the film and cure unevenly. On SLS and MJF, thin walls are fragile when the part is dug out of the powder and blasted clean. Thin is also a question of height: a thin wall that is tall and unsupported is weaker than the same wall that is short or braced by ribs.
Overhangs and supports
An overhang is any surface that faces downwards with nothing beneath it. FDM can lay filament out at an angle up to roughly 45° from vertical, because each layer is supported by the one below it. Beyond that, or for a flat ceiling, it needs support structures, which cost material and time to print and labour to remove, and leave marks.
Resin printing supports nearly everything that is not standing on the plate, including small islands that start in mid-air. SLS and MJF need no supports because the unfused powder carries the part, which is one reason they suit complex shapes.
Ways to reduce support: chamfer instead of a flat ledge, use a 45° roof or a teardrop shape for horizontal holes, split a part into two pieces that each print flat, and orient so the cosmetic face is not supported.
Holes, gaps and fine detail
Most processes print holes slightly smaller than drawn. On FDM, small vertical holes shrink because the nozzle rounds the inside corner, and horizontal holes droop at the top. Drill or ream holes that need a precise diameter, or design them slightly oversize and test.
A gap that is too narrow fuses shut: resin bleeds across, powder sinters into it, filament bridges it. If two surfaces must stay apart, keep the gap above the clearance in the table, and remember that any coating or finish adds thickness on both sides.
Hollow parts, drain holes and trapped material
A hollow part saves material and weight, but the inside must be emptied. In resin printing, liquid resin trapped in a sealed cavity is a trapped volume: it can crack the part later and you have paid for it. Add at least one drain hole, ideally two so air can enter as resin leaves, near the lowest point in the print orientation.
SLS and MJF have the same problem with powder. A sealed cavity stays full of unfused powder, so the part weighs as much as a solid one and still costs build volume. Escape holes need to be large enough to get powder out, typically several millimetres across, and more than one helps.
Orientation: strength, surface, support and time
Orientation is the decision that affects everything at once:
- Strength. FDM parts show strong anisotropy: the bond between layers is weaker than the filament, so orient load paths along the layers.
- Surface. Curved and sloped faces show stair-stepping; faces touching supports show marks. Put the cosmetic face upwards or vertical.
- Distortion. Large flat areas tend to warp on FDM and on powder bed processes. Tilting a large flat part, or adding ribs, reduces it.
- Time and cost. Height sets the number of layers. On resin machines that cure a whole layer at once, layer time barely depends on how much of the plate is used, so height is close to time.
Worked example: how orientation changes layer count on a resin printer. The layer time is an example figure.
A bar 120 × 20 × 10 mm, printed at 0.05 mm layers, with an example layer time of 8 s.
| Orientation | Height | Layers | Print time |
|---|---|---|---|
| Lying flat | 10 mm | 10 ÷ 0.05 = 200 | 200 × 8 s = 1,600 s, about 27 min |
| Standing upright | 120 mm | 120 ÷ 0.05 = 2,400 | 2,400 × 8 s = 19,200 s, 5 h 20 min |
Flat is 12 times faster here. It may still be the wrong choice if it puts supports on a cosmetic face or makes a large flat area peel badly, which is why a shop compares orientations rather than always picking the lowest one.
Files and units
Send a file that carries its units and a clean, closed mesh. An STL has no units, so a part drawn in inches can arrive 25.4 times too small; see how file units cost you money. The STL vs STEP vs 3MF guide explains which format to send and why.
Checking a design before you order
A good supplier checks walls, gaps, overhangs and trapped volumes against the actual machine and material before printing, and tells you what failed and why. Quotometry runs these checks on upload, decides them against the limits of the material and machine the buyer picks, and shows the result next to the price; the DFM checks page lists what it looks for. The FDM and SLA technology pages go further into each process.
Questions people ask
What is the most common reason a 3D print fails a design check?
Walls that are too thin for the process and material, closely followed by unsupported overhangs on FDM and resin, and sealed hollow sections that trap resin or powder. All three are visible in the file before printing, which is why bureaus check for them on upload rather than discovering them on the build plate.
How much clearance should moving parts have in a 3D print?
It depends on the process. As a starting point, resin printing often works with a few tenths of a millimetre between surfaces, while FDM, SLS and MJF usually need more, around half a millimetre or so for parts that must move freely. Print a small test piece on the actual machine and material before committing a full assembly.
Does orientation change the price of a 3D print?
Often, yes. Orientation changes the part's height, which sets layer count and print time, and it changes how much support material is needed and where support marks land. On powder bed processes it also changes how parts pack into the build. A good quote either picks the cheapest valid orientation or lets the buyer choose one.
Why does my FDM part break along the layer lines?
FDM parts are anisotropic: the bond between layers is weaker than the extruded filament itself, so a part is usually weakest when it is pulled in the build direction. Orient the part so the main load runs along the layers rather than across them, and add fillets where stress concentrates.
Quotometry prices every part from your own machines and rates, on your website, in seconds.