3D printing design guidelines

Printed parts typically need walls of at least 0.030 in (0.8 mm) in SLS and MJF, 0.020 in (0.5 mm) in SLA and 0.016 in (0.4 mm) in metal, overhangs of 45° or steeper from horizontal in FDM, SLA and metal, two or more escape holes in hollow parts, and 0.020 in (0.5 mm) clearance between printed-in-place parts. SLS and MJF hold about ±0.3%.

Try the interactive lab Check a part in the builder

Self-supporting angle: 45° from horizontal
SLS/MJF minimum wall: 0.030 in (0.8 mm)
Assembly clearance: 0.020 in (0.5 mm)
SLS/MJF tolerance: ±0.3%, ±0.012 in min

SSG MFG · design guideDG-14 · 11 rules

What are the 3d printing design rules?

11 rules, in the order you meet them on a model. Every value is typical; the principal quoting your part confirms its own limits.

Design rules and typical values
#	Rule	Typical value
01	Meet the process minimum wallSLS/MJF about 0.030 in (0.8 mm); SLA about 0.020 in (0.5 mm); FDM about 0.040 in (1.0 mm); metal about 0.016 in (0.4 mm)	SLS/MJF about 0.030 in (0.8 mm); SLA about 0.020 in (0.5 mm); FDM about 0.040 in (1.0 mm); metal about 0.016 in (0.4 mm)
02	Design self-supporting overhangsAt least 45° from horizontal for FDM, SLA and metal LPBF; no limit for SLS and MJF	At least 45° from horizontal for FDM, SLA and metal LPBF; no limit for SLS and MJF
03	Keep bridges and horizontal holes shortFDM bridges up to about 0.4 in (10 mm); horizontal holes in metal self-support to about 0.3 in (8 mm), teardrop above that	FDM bridges up to about 0.4 in (10 mm); horizontal holes in metal self-support to about 0.3 in (8 mm), teardrop above that
04	Add escape holes to hollow partsAt least two holes, about 0.2 in (5 mm) for powder or 0.14 in (3.5 mm) for resin, at opposite ends	At least two holes, about 0.2 in (5 mm) for powder or 0.14 in (3.5 mm) for resin, at opposite ends
05	Leave clearance between mating partsAbout 0.020 in (0.5 mm) for printed-in-place SLS/MJF assemblies; 0.010–0.020 in (0.25–0.5 mm) for separately printed fits	About 0.020 in (0.5 mm) for printed-in-place SLS/MJF assemblies; 0.010–0.020 in (0.25–0.5 mm) for separately printed fits
06	Size holes and pinsHoles and pins at least 0.060 in (1.5 mm) diameter; ream or drill holes that need a fit	Holes and pins at least 0.060 in (1.5 mm) diameter; ream or drill holes that need a fit
07	Orient for loadLoad FDM parts in the X–Y plane; put cosmetic faces up in SLA and away from supports	Load FDM parts in the X–Y plane; put cosmetic faces up in SLA and away from supports
08	Hollow or lattice thick sectionsHollow polymer sections over about 0.5 in (13 mm) thick; add ribs or lattice inside	Hollow polymer sections over about 0.5 in (13 mm) thick; add ribs or lattice inside
09	Radius internal corners in metal and resinInside radius at least 0.020 in (0.5 mm)	Inside radius at least 0.020 in (0.5 mm)
10	Leave stock on critical metal featuresAbout 0.010–0.020 in (0.25–0.5 mm) for finish machining	About 0.010–0.020 in (0.25–0.5 mm) for finish machining
11	Put critical features on a drawingSLS/MJF ±0.3% (±0.012 in / ±0.3 mm minimum); SLA about ±0.005 in (±0.13 mm) over the first inch; flag tighter features for machining	SLS/MJF ±0.3% (±0.012 in / ±0.3 mm minimum); SLA about ±0.005 in (±0.13 mm) over the first inch; flag tighter features for machining

These build on the short list on the 3d printing process page, with the failure each rule prevents and a drawing for each.

When does a 3D print need supports?

Tilt a face from vertical toward horizontal to see where FDM, SLA and metal powder bed fusion start needing supports, typically below about 45°. SLS and MJF print the same face with no supports because the unfused powder holds it up.

OVERHANG 50° FROM HORIZONTAL · FDM

Self-supporting from: 45°
Supports: none

Works: self-supporting

At 50° each layer rests mostly on the one below. No supports, no witness marks on this face.

Typical limits. Short bridges and small horizontal holes can print unsupported; the printer's own guidance governs.

Why does each rule matter?

Each rule with its typical value, the reason behind it and what happens on the floor when it's ignored. Switch any drawing between Do and Avoid; point at a callout to pick it out.

Rule 01

Meet the process minimum wall

SLS/MJF about 0.030 in (0.8 mm); SLA about 0.020 in (0.5 mm); FDM about 0.040 in (1.0 mm); metal about 0.016 in (0.4 mm)

Why: Below these thicknesses the process cannot form a closed, solid wall reliably.
If you ignore it: Thin walls warp, print with holes, or break during depowdering, support removal or bead blast.

Fig. 1Minimum machined wall

Do. Walls at least 0.030 in (0.8 mm) in metal and 0.060 in (1.5 mm) in plastic, kept short relative to their thickness, stay flat and hold size.

Avoid. A tall, thin wall rings under the cutter, springs away from it and comes out wavy, thin at the top or cracked.

Rule 02

Design self-supporting overhangs

At least 45° from horizontal for FDM, SLA and metal LPBF; no limit for SLS and MJF

Why: Each layer needs something underneath it. Powder-bed polymer processes use the loose powder as support.
If you ignore it: Shallow overhangs sag or curl, and the supports that fix them add cost, leave witness marks and must be cut off, by hand or EDM in metal.

Fig. 2Overhang angle

Do. Overhangs at 45° or steeper from horizontal build on the layer below and need no support in FDM, SLA or metal.

Avoid. Shallow overhangs need support structures that scar the surface and cost removal time; unsupported, they droop and curl.

Rule 03

Keep bridges and horizontal holes short

FDM bridges up to about 0.4 in (10 mm); horizontal holes in metal self-support to about 0.3 in (8 mm), teardrop above that

Why: A bridge or hole top prints over air. Short spans hold; long spans droop.
If you ignore it: Bridges droop, hole tops print flat or rough, and pins that should fit come out tight.

Rule 04

Add escape holes to hollow parts

At least two holes, about 0.2 in (5 mm) for powder or 0.14 in (3.5 mm) for resin, at opposite ends

Why: Powder and resin inside a closed cavity cannot drain. Two holes let air in while material flows out.
If you ignore it: Trapped powder adds weight, and trapped resin keeps curing and cracks the part from the inside.

Fig. 3Escape holes

Do. Two or more escape holes, about 0.2 in (5 mm) for powder or 0.14 in (3.5 mm) for resin, let the inside be cleaned out.

Avoid. A sealed hollow keeps its powder or liquid resin: extra weight, and in SLA a cavity that can crack the part as it cures or heats.

Rule 05

Leave clearance between mating parts

About 0.020 in (0.5 mm) for printed-in-place SLS/MJF assemblies; 0.010–0.020 in (0.25–0.5 mm) for separately printed fits

Why: Heat from fusing spreads into neighboring powder, and resin and filament processes spread slightly at each layer.
If you ignore it: Moving parts fuse together, and snap and slip fits need sanding or reprinting.

Fig. 4Clearance between printed parts

Do. Leave about 0.020 in (0.5 mm) between parts printed in place in SLS or MJF so they come out free.

Avoid. A tight gap fills with partly fused powder and the parts come out as one piece.

Rule 06

Size holes and pins

Holes and pins at least 0.060 in (1.5 mm) diameter; ream or drill holes that need a fit

Why: Small holes fill with partly fused powder, and small pins break during cleanup.
If you ignore it: Holes close up or print undersize, and pins snap off during depowdering or support removal.

Rule 07

Orient for load

Load FDM parts in the X–Y plane; put cosmetic faces up in SLA and away from supports

Why: FDM parts are weakest between layers, and supports leave witness marks on the faces they touch.
If you ignore it: FDM parts split along a layer line under load, and support marks land on the face the customer sees.

Rule 08

Hollow or lattice thick sections

Hollow polymer sections over about 0.5 in (13 mm) thick; add ribs or lattice inside

Why: Powder-bed and resin parts price by volume, and thick polymer sections hold heat and warp.
If you ignore it: Parts cost more than they need to, and thick SLS and MJF sections warp and sink as they cool.

Fig. 5Core out thick sections

Do. Hollow the section from the back into walls and ribs at T: same stiffness at the face, a fraction of the cooling time.

Avoid. A solid thick section takes several times longer to cool and still sinks at the surface and voids in the middle.

Rule 09

Radius internal corners in metal and resin

Inside radius at least 0.020 in (0.5 mm)

Why: Residual stress from printing and brittle cured resin both crack from sharp corners.
If you ignore it: Metal parts crack at corners during stress relief or plate removal, and SLA parts crack on assembly.

Fig. 6Inside and outside radii

Do. Inside radius at least half the wall and outside radius equal to inside plus T: the corner stays at thickness T and flow turns smoothly.

Avoid. A sharp inside corner concentrates stress about 3× and the corner runs thick: cracks start there, and it cools last.

Rule 10

Leave stock on critical metal features

About 0.010–0.020 in (0.25–0.5 mm) for finish machining

Why: As-printed metal is rough and can move during stress relief and plate removal.
If you ignore it: Bores, sealing faces and datums come out undersize or rough with no stock left to clean them up.

Fig. 7Machining stock

Do. A thin, even allowance on the faces that need it; the datum sits on a machined face, and as-cast or as-forged faces stay as they are.

Avoid. Too much stock cuts through the dense skin into porous core on a casting; too little leaves scale or draft on a forging.

Rule 11

Put critical features on a drawing

SLS/MJF ±0.3% (±0.012 in / ±0.3 mm minimum); SLA about ±0.005 in (±0.13 mm) over the first inch; flag tighter features for machining

Why: A mesh file carries no tolerances. The drawing tells the printer which features to measure, orient for or machine.
If you ignore it: Parts are printed to the default and critical fits fail at assembly with no basis for rejection.

Standard: ASME Y14.5

Fig. 8A complete drawing package

Do. Every requirement is on the drawing: general tolerance, material by specification, finish by specification, critical dimensions and revision.

Avoid. Whatever the drawing leaves blank, the supplier decides, usually with the cheapest local equivalent.

What tolerances can 3d printing hold?

Typical values for as-printed parts. Size, orientation and material move each number, and features that need better than the tight column are machined after printing.

Typical and tight tolerances with the cost of going tight
Feature	Typical	Tight	Cost of tight
SLS/MJF linear	±0.3%, ±0.012 in (±0.3 mm) min	±0.2%, ±0.008 in (±0.2 mm) min	Moderate
SLA linear, first inch (25 mm)Add about 0.001 in per added inch.	±0.005 in (±0.13 mm)	±0.002 in (±0.05 mm)	Moderate
FDM linear	±0.010 in (±0.25 mm)	±0.005 in (±0.13 mm)	Moderate
Metal LPBF linear	±0.004 in (±0.1 mm) + 0.2%	±0.001 in (±0.025 mm) machined	High
Hole diameter, SLS/MJF	±0.012 in (±0.3 mm), prints undersize	±0.002 in (±0.05 mm) drilled or reamed	Moderate
Flatness, SLS/MJF, up to 6 in (150 mm)Ribs and orientation matter more than process settings.	0.020 in (0.5 mm)	0.010 in (0.25 mm)	High

Basis: Industry-typical by process (SLS, MJF, SLA, FDM, metal LPBF). Put a general tolerance note on the drawing and tighten only the features that need it; every tight callout is priced. See the tolerance guide.

How does the material change the rules?

The same 3d printing rules shift with the alloy or compound.

Nylon 12 (PA12) for 3D printing
PA12 in SLS and MJF needs no supports and holds about ±0.3%, but walls under 0.030 in (0.8 mm) break during depowdering. Large flat areas can warp, so rib panels and keep sections even.
TPE (thermoplastic elastomer)
Flexible TPU and TPE prints need thicker walls, around 0.040 in (1.0 mm) or more, and larger clearances because the material drags and sticks. Fine features and small holes print poorly in soft grades.
Polycarbonate (PC)
PC is printed by FDM, so the 45° overhang rule, layer-direction weakness and a 0.040 in (1.0 mm) minimum wall all apply. It warps on large flat parts without a heated chamber.
PEEK (polyether ether ketone)
PEEK prints by high-temperature FDM and is prone to warping and layer weakness. Use fillets, even walls and orient load paths along the layers.
Stainless steel 316
316L in laser powder bed fusion follows the 45° overhang rule and reaches over 99% density. Leave 0.010–0.020 in (0.25–0.5 mm) of stock on bores and sealing faces for machining after stress relief.
Titanium Grade 5 (Ti-6Al-4V)
Ti-6Al-4V prints thin walls near 0.016 in (0.4 mm) but carries high residual stress, so parts are stress relieved on the plate. Design support removal access and radius internal corners.

3D printing design questions

What is the minimum wall thickness for 3D printing?

It depends on the process. SLS and MJF nylon need about 0.030 in (0.8 mm), SLA about 0.020 in (0.5 mm), FDM about 0.040 in (1.0 mm) and metal powder bed fusion about 0.016 in (0.4 mm). Walls that are tall and unsupported need more. Flexible materials such as TPU need about 0.040 in (1.0 mm) or more.

What overhang angle can be printed without supports?

FDM, SLA and metal laser powder bed fusion typically print overhangs of 45° or steeper from horizontal without supports. Shallower faces need support structures that add cost and leave marks. SLS and MJF have no overhang limit because unfused powder supports the part during the build, which is why they suit complex functional nylon parts.

How much clearance do 3D printed parts need?

Printed-in-place SLS and MJF assemblies such as hinges and chains need about 0.020 in (0.5 mm) between moving surfaces. Separately printed parts that must fit together typically need 0.010–0.020 in (0.25–0.5 mm), depending on the fit. Tighter gaps fuse or need sanding. Critical fits are best reamed or machined after printing.

Why do hollow 3D printed parts need escape holes?

Powder or liquid resin inside a closed cavity cannot drain. Trapped powder adds weight and cost, and trapped resin keeps curing and can crack the part. Use at least two holes at opposite ends, about 0.2 in (5 mm) for powder processes and 0.14 in (3.5 mm) for resin, so air enters as material leaves.

How small a hole can be 3D printed?

Holes and pins of about 0.060 in (1.5 mm) diameter are a practical minimum across most processes. Below that, SLS and MJF holes fill with partly fused powder and SLA holes close with uncured resin. Printed holes usually come out slightly undersize, so drill or ream any hole that needs a fit.

Should I design a printed part differently if it will be molded later?

Yes, if molding is the plan. Printing tolerates thick sections, zero draft and trapped undercuts that a mold cannot. Designing to molding rules from the start, with uniform walls, 1–2° draft and ribs at 50–60% of the wall, means printed prototypes test the same geometry that will go into steel.

Check your part against these rules.

Drop a STEP file in the builder for an instant DFM check and a budgetary estimate, then send it to principals who run 3d printing every day.

Build a part Send a drawing

3D printing design guidelines

Rule

Meet the process minimum wallSLS/MJF about 0.030 in (0.8 mm); SLA about 0.020 in (0.5 mm); FDM about 0.040 in (1.0 mm); metal about 0.016 in (0.4 mm)

Design self-supporting overhangsAt least 45° from horizontal for FDM, SLA and metal LPBF; no limit for SLS and MJF

Keep bridges and horizontal holes shortFDM bridges up to about 0.4 in (10 mm); horizontal holes in metal self-support to about 0.3 in (8 mm), teardrop above that

Add escape holes to hollow partsAt least two holes, about 0.2 in (5 mm) for powder or 0.14 in (3.5 mm) for resin, at opposite ends

Leave clearance between mating partsAbout 0.020 in (0.5 mm) for printed-in-place SLS/MJF assemblies; 0.010–0.020 in (0.25–0.5 mm) for separately printed fits

Size holes and pinsHoles and pins at least 0.060 in (1.5 mm) diameter; ream or drill holes that need a fit

Orient for loadLoad FDM parts in the X–Y plane; put cosmetic faces up in SLA and away from supports

Hollow or lattice thick sectionsHollow polymer sections over about 0.5 in (13 mm) thick; add ribs or lattice inside

Radius internal corners in metal and resinInside radius at least 0.020 in (0.5 mm)

Leave stock on critical metal featuresAbout 0.010–0.020 in (0.25–0.5 mm) for finish machining

Put critical features on a drawingSLS/MJF ±0.3% (±0.012 in / ±0.3 mm minimum); SLA about ±0.005 in (±0.13 mm) over the first inch; flag tighter features for machining

Feature

Typical

Tight

Cost of tight

SLS/MJF linear

±0.3%, ±0.012 in (±0.3 mm) min

±0.2%, ±0.008 in (±0.2 mm) min

Moderate

SLA linear, first inch (25 mm)Add about 0.001 in per added inch.

±0.005 in (±0.13 mm)

±0.002 in (±0.05 mm)

Moderate

FDM linear

±0.010 in (±0.25 mm)

±0.005 in (±0.13 mm)

Moderate

Metal LPBF linear

±0.004 in (±0.1 mm) + 0.2%

±0.001 in (±0.025 mm) machined

High

Hole diameter, SLS/MJF

±0.012 in (±0.3 mm), prints undersize

±0.002 in (±0.05 mm) drilled or reamed

Moderate

Flatness, SLS/MJF, up to 6 in (150 mm)Ribs and orientation matter more than process settings.

0.020 in (0.5 mm)

0.010 in (0.25 mm)

High

What are the 3d printing design rules?

When does a 3D print need supports?