What Is Sheet Metal Fabrication? Processes, Materials & Design Guide (2026)

Q: What is the difference between sheet metal fabrication and CNC machining?

Sheet metal fabrication starts with flat sheet stock (typically 0.020–0.250 in. / 0.5–6.4 mm thick) and transforms it through cutting, bending, and joining into 3D parts — enclosures, brackets, panels. CNC machining starts with a solid block (billet) and removes material to create the final shape. Sheet metal is typically 30–60% less expensive than CNC machining for parts that can be made from bent and welded sheet, because the raw material cost is lower and the processes are faster. However, CNC machining can produce tighter tolerances (±0.001 in. vs. ±0.005–0.030 in. for sheet metal) and more complex 3D geometry.

Q: What is bend allowance and why does it matter?

Bend allowance (BA) is the length of the arc through the bend zone — the amount of material consumed by the bend itself. When you flatten a bent part, the flat pattern length is not simply the sum of the outside dimensions; it is the sum of the flat segments plus the bend allowance for each bend. The formula is BA = π/180 × bend angle × (inside radius + K-factor × material thickness). If the bend allowance is wrong, the flat pattern will be the wrong size, and the finished part will not match the 3D model. CAD software (SolidWorks, Fusion 360) calculates this automatically if the K-factor and bend radius are set correctly in the sheet metal parameters.

Q: What is the K-factor?

The K-factor is a ratio (0 < K < 1) that defines the position of the neutral axis within the bend zone relative to the material thickness. A K-factor of 0.33 means the neutral axis sits at 33% of the thickness from the inside surface. For air bending, K ≈ 0.33 is a common starting point. For bottom bending (coining), K ≈ 0.42 is typical. The actual K-factor depends on material type, thickness, bend radius, and bend method. Incorrect K-factors produce flat patterns that are too long or too short — resulting in parts where the bend-to-edge or bend-to-hole dimensions are out of spec.

Q: What tolerances can sheet metal fabrication achieve?

Tolerances vary by operation: Laser cutting: ±0.005 in. (±0.13 mm) on flat dimensions. Single-bend dimensions: ±0.010 in. (±0.25 mm). Multi-bend (cumulative): ±0.030 in. (±0.76 mm). Bend angle: ±1°. Hole-to-bend dimensions: ±0.010 in. (±0.25 mm). PEM insert diameters: +0.003/−0.000 in. These are standard tolerances for CNC press brake and fiber laser equipment. Tighter tolerances are achievable on specific features with secondary operations (e.g., CNC machining a critical hole after forming), but this adds cost.

Q: When should I use laser cutting vs. waterjet vs. plasma?

Laser cutting (fiber or CO2) is the default for most sheet metal work — it handles aluminum, steel, and stainless up to 0.5 in. (12.7 mm) with ±0.005 in. tolerances and a clean, burr-free edge. Waterjet cutting is the choice when you need to cut heat-sensitive materials (titanium, composites, glass, stone), very thick stock (up to 6 in. / 150 mm), or when you cannot have a heat-affected zone (HAZ). Waterjet tolerances are typically ±0.003–0.005 in. Plasma cutting is the economical choice for thick carbon steel and stainless (0.5–2 in.) where edge quality is less critical — tolerances are ±0.015–0.030 in. with a rougher edge that typically needs grinding.

Q: What is the minimum bend radius for common sheet metals?

Minimum inside bend radius depends on the alloy and temper: 5052-H32 aluminum: 0.5× thickness (very formable). 6061-T6 aluminum: 1.0× thickness (less ductile, cracks at tighter radii). 304 stainless steel: 0.5–1.0× thickness depending on temper. A36 carbon steel: 0.5× thickness. 1008/1010 cold-rolled steel: 0.5× thickness. Brass C260: 0.5× thickness. Going below the minimum radius causes cracking on the outer surface of the bend. As a rule, softer tempers (annealed, H32) bend tighter than harder tempers (T6, full-hard). Always specify the bend radius on your drawing — do not leave it to the shop to guess.

Q: What file format should I send for a sheet metal quote?

Send a 3D model (STEP preferred) and a 2D engineering drawing (PDF). For sheet metal specifically: the 3D model should be modeled as a sheet metal part in your CAD software (SolidWorks Sheet Metal, Fusion 360 Sheet Metal) so the flat pattern can be extracted automatically. A DXF of the flat pattern is helpful but not required — most fabricators will unfold the model themselves. The 2D drawing should call out material, thickness, bend radii, tolerances, hardware (PEM inserts, rivets), and finish. Missing any of these creates an RFI that delays your quote.

Q: What are PEM fasteners and when do I use them?

PEM (Penn Engineering & Manufacturing) fasteners are self-clinching hardware — studs, nuts, and standoffs that are pressed into sheet metal during fabrication. They create permanent, load-bearing threads in thin sheet that would strip if you tried to tap directly. Use PEM fasteners when: the sheet is too thin to tap (< 3× thread pitch), you need the fastener flush with one surface, or you need a captive nut on a panel for field assembly. Common types: CLS (flush nuts), FH (flush-head studs), SO (standoffs), BSO (blind standoffs). Specify PEM part numbers on your drawing — e.g., "CLS-M4-2 (press from this side)."

Why sheet metal fabrication is a core skill for every ME

If you design anything with an enclosure, bracket, panel, or chassis, you will specify sheet metal parts. Sheet metal fabrication accounts for roughly 30–40% of all custom metal parts produced globally. Understanding how flat metal becomes a 3D part — and why bend allowance, K-factor, and minimum bend radius matter — is the difference between a design that quotes in 24 hours and one that comes back with 10 RFIs. This guide teaches the process from first principles.

Section 1 of 9

What Is Sheet Metal Fabrication?

Sheet metal fabrication is a set of manufacturing processes that start with flat metal stock — typically 0.020–0.250 in. (0.5–6.4 mm) thick — and transform it into functional 3D parts through cutting, bending, and joining. The raw material is called “sheet” (≤0.250 in.) or “plate” (>0.250 in.), and the finished parts range from tiny RF shields to full-size server rack enclosures.

Forming, not removing

Unlike CNC machining (subtractive — removes material from a block) or 3D printing (additive — builds layer by layer), sheet metal fabrication primarily reshapes existing material. You start with a flat sheet and bend, fold, or weld it into the final geometry. Very little material is wasted — only the cut-out scrap from holes and perimeter trimming.

The three core operations

Every sheet metal part is made from some combination of: (1) Cutting — separating the flat blank from stock using a laser, waterjet, plasma torch, or punch press. (2) Forming — bending the flat blank into 3D geometry using a press brake, roll former, or stamping die. (3) Joining — assembling multiple pieces using welding (TIG, MIG, spot), riveting, or self-clinching fasteners (PEM hardware).

Why "flat pattern" matters

Every 3D sheet metal part unfolds into a 2D flat pattern — the shape that gets laser-cut from the sheet before bending. Getting the flat pattern right requires understanding bend allowance, bend deduction, and K-factor. If the flat pattern is wrong, every bend-to-feature dimension on the finished part will be out of spec.

Cost advantage over CNC machining

Sheet metal is typically 30–60% less expensive than CNC machining for parts that can be made from bent and welded sheet — because the raw material cost is a fraction of billet, cycle times are shorter (seconds per bend vs. minutes per milled feature), and tooling is reusable across part numbers (standard V-dies vs. custom fixtures).

Section 2 of 9

Cutting Processes

Cutting is the first operation in virtually every sheet metal job. The goal is to separate the flat blank (the 2D flat pattern) from the raw sheet stock with the required profile accuracy and edge quality.

Laser Cutting (Fiber / CO₂)

A focused laser beam (fiber: 1.07 μm wavelength, CO₂: 10.6 μm) melts or vaporizes material along a programmed path. Fiber lasers dominate modern shops for metals — faster cutting speeds, lower operating cost, and cleaner edges than CO₂ on reflective materials like aluminum and copper. CO₂ lasers are still used for thicker non-metals and some specialty applications.

Tolerance: ±0.005 in. (±0.13 mm)

Max Thickness: 0.5 in. (12.7 mm) mild steel; 0.375 in. (9.5 mm) aluminum

Edge Quality: Clean, burr-free, minimal HAZ (0.005–0.020 in.)

Typical Use: Default choice for most sheet metal parts — profiles, holes, slots, tabs

Waterjet Cutting

A high-pressure water stream (60,000–90,000 PSI) mixed with abrasive garnet cuts through material without heat. No HAZ, no thermal distortion, no material property changes. The trade-off: slower cutting speed than laser (typically 5–20 in./min vs. 100–1,000 in./min for laser on thin sheet) and a wider kerf (0.030–0.050 in.).

Tolerance: ±0.003–0.005 in. (±0.08–0.13 mm)

Max Thickness: 6 in. (150 mm) — virtually any thickness

Edge Quality: Smooth, no HAZ, slight taper on thick cuts

Typical Use: Heat-sensitive materials, thick plate, composites, glass, titanium

Plasma Cutting

An electrically ionized gas jet (plasma arc at 20,000–30,000°F) melts and blows away material. Plasma is the workhorse for thick carbon steel and stainless where edge quality and tolerance are less critical than speed and cost. Modern high-definition plasma has improved edge quality, but still does not match laser or waterjet.

Tolerance: ±0.015–0.030 in. (±0.38–0.76 mm)

Max Thickness: 2 in. (50 mm) carbon steel typical

Edge Quality: Rougher edge, larger HAZ, may require grinding

Typical Use: Thick carbon steel plates, structural parts, cost-sensitive applications

Turret Punch Press

A CNC-controlled turret holds 20–60 punch tools that stamp holes, slots, and forms in sequence. Each hit creates one feature. Turret punching is economical for parts with many identical holes (e.g., perforated panels, ventilation grilles) because the per-hit cycle time is 0.3–1.0 seconds. Limitation: cannot cut arbitrary profiles like a laser — limited to combinations of standard tool shapes.

Tolerance: ±0.005 in. (±0.13 mm) on hole position

Max Thickness: 0.250 in. (6.35 mm) mild steel typical

Edge Quality: Sheared edge with slight burr (deburr required)

Typical Use: High-volume parts with many holes, louvers, or formed features

Section 3 of 9

Forming & Bending

Forming transforms a flat blank into 3D geometry by bending it between a punch and die on a press brake. This is where sheet metal gets its structural rigidity — a flat panel is flexible, but add a few bends and it becomes a stiff enclosure or bracket.

Air bending

The punch presses the sheet into a V-die but does not bottom out — the sheet "floats" in the die opening. Air bending uses roughly 60% of the tonnage of bottom bending, allows a range of bend angles from a single V-die (adjust the punch stroke to change the angle), and is the most common method on modern CNC press brakes. Typical tolerance: ±0.5–1.0° on angle, ±0.010 in. (±0.25 mm) on bend-line position.

Bottom bending (bottoming)

The punch pushes the sheet fully into the V-die until the material contacts both sides of the die. This produces more consistent angles (±0.25–0.5°) than air bending because the final angle is defined by the tooling geometry rather than the punch stroke. The trade-off: requires 3–5× more tonnage and a matched die set for each desired angle.

Coining

The punch applies enough force to plastically deform the material at the bend line — "coining" the radius into the sheet. Coining produces the tightest angle tolerance (±0.25°) and the smallest possible radius, but requires 5–10× the tonnage of air bending. Rarely used in modern shops except for high-volume stamping where the cost of extra tonnage is justified by the volume.

Roll forming

The sheet passes through a series of roller stations, each progressively forming the profile. Roll forming is used for long, constant-cross-section parts: C-channels, hat sections, angles, and structural rails. It is economical at high volumes (1,000+ linear feet) but has high NRE (non-recurring engineering) for the roller tooling. Not used for short-run custom work — that is press brake territory.

Design Tip

Keep bend lines parallel when possible. Parts with bends in multiple orientations require the operator to rotate the part between bends, adding setup time and increasing the chance of orientation errors. If your design has bends in two perpendicular directions, call out which bends are formed first in your notes — bend sequence affects final dimensions.

Section 4 of 9

Joining Methods

Joining assembles multiple sheet metal pieces into a single part or weldment. The method you choose depends on the material, load requirements, appearance, and whether the joint needs to be disassembled.

TIG Welding (GTAW)

Uses a non-consumable tungsten electrode with argon shielding gas. Produces clean, precise, cosmetically appealing welds. The default for aluminum, stainless steel, and visible joints. Slower than MIG (2–5 in./min vs. 10–30 in./min) but produces a narrower HAZ and less distortion.

Typical Use: Aluminum enclosures, stainless medical housings, cosmetic weldments

MIG Welding (GMAW)

Uses a consumable wire electrode fed through a torch with shielding gas (argon/CO₂ mix). Faster than TIG, easier to automate, and effective on carbon steel, stainless, and thicker sections. Produces a wider bead than TIG — not ideal for cosmetic joints unless ground and finished afterward.

Typical Use: Carbon steel frames, structural brackets, high-volume weldments

Spot Welding (Resistance)

Two copper electrodes clamp the overlapping sheets and pass current through them — the resistance at the interface generates heat and fuses the sheets. Each spot takes 0.1–0.5 seconds. Used extensively in automotive and appliance manufacturing for thin-gauge (≤0.125 in. / 3.2 mm) lap joints.

Typical Use: Thin-gauge lap joints, high-volume assembly, automotive panels

PEM Self-Clinching Fasteners

PEM studs, nuts, and standoffs are pressed into the sheet metal using a press brake or dedicated insertion press. The knurled body of the fastener cold-flows into the sheet, creating a permanent, flush, load-bearing thread. No welding, no tapping, no back-side access needed.

Typical Use: Threaded inserts in thin sheet, flush-mount hardware, field-serviceable panels

Riveting

Blind (pop) rivets or solid rivets join overlapping sheets or attach brackets to panels. Blind rivets require access from only one side — insert through the hole, pull the mandrel, and the rivet expands and locks. Solid rivets are stronger but require access to both sides.

Typical Use: Non-weldable joints, dissimilar materials, vibration-resistant assemblies

Adhesive Bonding

Structural adhesives (epoxy, acrylic, polyurethane) bond sheet metal without heat or fastener holes. Distributes load over the entire bond area rather than point loads at fastener locations. Used where appearance matters (no visible fasteners) or where thermal distortion from welding is unacceptable.

Typical Use: Cosmetic panels, dissimilar-metal joints, vibration damping

Section 5 of 9

Flat Pattern Fundamentals

Every 3D sheet metal part unfolds into a 2D flat pattern. Getting the flat pattern right is the single most important step in sheet metal design — if the flat is wrong, every bend-to-feature dimension on the finished part will be off.

Bend allowance (BA)

Bend allowance is the arc length of the material through the bend zone. Formula: BA = (π / 180) × bend angle × (inside radius + K × thickness), where K is the K-factor. The flat pattern length across a bend is: flat segment A + BA + flat segment B. BA accounts for the fact that the material stretches on the outside of the bend and compresses on the inside.

K-factor

The K-factor (0 < K < 1) defines where the neutral axis sits within the material thickness during bending. At the neutral axis, the material is neither stretched nor compressed. K = 0.33 is a common starting value for air bending; K = 0.42 for bottom bending. Actual values depend on material, thickness, radius, and bend method. In practice, shops calibrate K-factors by measuring test bends — your CAD K-factor should match your supplier's process.

Bend deduction (BD)

Bend deduction is an alternative to bend allowance. BD = 2 × (outside setback) − BA. The flat pattern length is: outside dimension A + outside dimension B − BD. Some CAD systems use bend deduction instead of bend allowance. Both produce the same flat pattern if the inputs are consistent — they are just two ways to express the same math.

Setting up your CAD correctly

In SolidWorks: Sheet Metal feature → Edit Sheet Metal Parameters → set K-factor, bend radius, and thickness. In Fusion 360: Sheet Metal Rules → create a rule with your K-factor and default radius. Always match these values to your supplier's process — ask them for their K-factor table by material and thickness. A 10% error in K-factor on a 4-bend part can shift a critical dimension by 0.020–0.040 in. (0.5–1.0 mm).

Pro Tip

Before placing your first sheet metal order, ask your supplier for their K-factor table and default inside bend radii by material/thickness. Enter these into your CAD sheet metal parameters. This single step eliminates the #1 source of dimensional errors on sheet metal parts: mismatched flat patterns between your design and their production process.

Section 6 of 9

Common Sheet Metal Materials

Material selection affects formability, weldability, corrosion resistance, and cost. Here are the most commonly fabricated sheet metals, with the specific alloy/temper you should specify on your drawing.

Material	Alloy / Grade	Min Bend Radius	Weldability	Typical Application
Aluminum	5052-H32	0.5× thickness	TIG (good)	Enclosures, panels, marine hardware
Aluminum	6061-T6	1.0× thickness	TIG (fair — cracks risk at weld)	Structural brackets, frames
Stainless Steel	304	0.5–1.0× thickness	TIG (excellent)	Food/medical equipment, outdoor
Stainless Steel	316L	0.5–1.0× thickness	TIG (excellent)	Chemical, marine, pharmaceutical
Carbon Steel	A36 / 1008/1010 CRS	0.5× thickness	MIG/TIG (excellent)	Structural frames, bases, painted enclosures
Galvanized Steel	G90 (hot-dip)	1.0× thickness	MIG (fair — zinc fumes)	HVAC, outdoor enclosures, no-paint applications
Copper	C110 (ETP)	0.5× thickness	TIG/brazing	Bus bars, RF shields, heat sinks
Brass	C260 (cartridge)	0.5× thickness	Brazing (TIG possible)	Decorative panels, electrical connectors

Specify the alloy, not just the family

Per §19: write “5052-H32 aluminum, 0.063 in. thick” on your drawing — not “aluminum sheet.” The alloy determines formability (min bend radius), the temper determines strength and ductility, and the thickness determines tooling selection. Missing any of these produces an RFI that delays your quote.

Section 7 of 9

Surface Finishing

Finishing protects the part from corrosion, improves appearance, and can add functional properties (electrical conductivity, wear resistance, biocompatibility). Specify the finish on your drawing — “per customer spec” is not a finish callout.

Powder Coating

Electrostatically applied dry powder, cured at 350–400°F (175–200°C). Produces a durable, uniform coat in any RAL color. Typical thickness: 2–4 mil (50–100 μm). Widely used for enclosures, brackets, and outdoor hardware.

Compatible: Carbon steel, aluminum (with primer)

Anodizing (Type II)

Electrochemical process that grows a hard oxide layer on aluminum. Available clear or dyed (black, blue, red, gold). Typical thickness: 0.3–1.0 mil (8–25 μm). Adds corrosion resistance and a professional appearance without changing dimensions significantly.

Compatible: Aluminum only (5052, 6061, 7075)

Hardcoat Anodizing (Type III)

Thicker oxide layer (1.0–3.0 mil / 25–75 μm) that adds wear resistance and hardness (60–70 HRC equivalent on surface). Used for high-wear aluminum parts — slides, rails, actuator bodies. Adds roughly half the coating thickness to each surface (growth is ~50% into the base metal, ~50% outward).

Compatible: Aluminum (6061-T6 preferred)

Passivation

Acid bath (citric or nitric acid per ASTM A967 or AMS 2700) that removes free iron from stainless steel surfaces and restores the chromium oxide passive layer. Required for medical, food-contact, and marine stainless steel parts.

Compatible: Stainless steel (304, 316L)

Zinc Plating

Electroplated zinc coating (0.2–0.5 mil / 5–12 μm) with optional chromate conversion (clear, yellow, black). Provides sacrificial corrosion protection for carbon steel. Typical cost: $0.50–$2.00/part for small brackets. Common for hardware and fasteners.

Compatible: Carbon steel, low-alloy steel

Bead Blasting

Glass bead or aluminum oxide media blasted at the surface to create a uniform matte texture. Hides tool marks and fingerprints. Often used as a pre-treatment before anodizing or powder coating. Specify media type and finish (e.g., "glass bead, 80–120 mesh, uniform matte").

Compatible: All metals

Section 8 of 9

Cutting Process Comparison

Feature	Laser (Fiber)	Waterjet	Plasma	Turret Punch
Tolerance	±0.005 in.	±0.003–0.005 in.	±0.015–0.030 in.	±0.005 in.
Max Thickness	0.5 in. steel	6 in.+	2 in. steel	0.250 in.
Edge Quality	Clean, burr-free	Smooth, no HAZ	Rough, large HAZ	Sheared, slight burr
Heat Affected Zone	Minimal	None	Large	None
Speed (thin sheet)	Very fast	Slow	Fast	Fast (holes)
Cost (per part)	Low–moderate	Moderate–high	Low	Low (high volume)
Arbitrary Profiles	Yes	Yes	Yes	Limited to tool shapes

Section 9 of 9

When to Choose Sheet Metal vs. CNC Machining

Sheet metal and CNC machining are complementary, not competing. Use this framework to decide which is the primary process for your part.

Is the part an enclosure, panel, or bracket made from bent sheet?

Yes →

Sheet metal fabrication — laser cut, bend, and finish. This is the natural process for box-like geometry from flat stock.

No →

CNC machining from billet if the part has thick walls, complex 3D features, or tight tolerances on all surfaces.

Is the wall thickness uniform and ≤0.250 in.?

Yes →

Sheet metal — uniform wall is inherent to the process (you start with sheet of constant thickness).

No →

CNC machining if the part requires varying wall thicknesses, deep pockets, or solid features.

Do you need tight tolerances (±0.001 in.) on mating features?

Yes →

CNC machining for the critical features — or use sheet metal for the body and CNC-machine critical holes/surfaces as a secondary operation.

No →

Sheet metal tolerances (±0.005–0.030 in.) are sufficient for most enclosure and bracket applications.

Is cost the primary driver and volume is 10+ parts?

Yes →

Sheet metal is typically 30–60% less expensive than CNC machining for qualifying geometry. The savings increase with volume.

No →

For 1–5 parts of moderate complexity, CNC machining from billet may be comparable in cost due to simpler programming.

Common Questions

Frequently Asked Questions

What is the difference between sheet metal fabrication and CNC machining?

Sheet metal fabrication starts with flat sheet stock (typically 0.020–0.250 in. / 0.5–6.4 mm thick) and transforms it through cutting, bending, and joining into 3D parts — enclosures, brackets, panels. CNC machining starts with a solid block (billet) and removes material to create the final shape. Sheet metal is typically 30–60% less expensive than CNC machining for parts that can be made from bent and welded sheet, because the raw material cost is lower and the processes are faster. However, CNC machining can produce tighter tolerances (±0.001 in. vs. ±0.005–0.030 in. for sheet metal) and more complex 3D geometry.

What is bend allowance and why does it matter?

Bend allowance (BA) is the length of the arc through the bend zone — the amount of material consumed by the bend itself. When you flatten a bent part, the flat pattern length is not simply the sum of the outside dimensions; it is the sum of the flat segments plus the bend allowance for each bend. The formula is BA = π/180 × bend angle × (inside radius + K-factor × material thickness). If the bend allowance is wrong, the flat pattern will be the wrong size, and the finished part will not match the 3D model. CAD software (SolidWorks, Fusion 360) calculates this automatically if the K-factor and bend radius are set correctly in the sheet metal parameters.

What is the K-factor?

The K-factor is a ratio (0 < K < 1) that defines the position of the neutral axis within the bend zone relative to the material thickness. A K-factor of 0.33 means the neutral axis sits at 33% of the thickness from the inside surface. For air bending, K ≈ 0.33 is a common starting point. For bottom bending (coining), K ≈ 0.42 is typical. The actual K-factor depends on material type, thickness, bend radius, and bend method. Incorrect K-factors produce flat patterns that are too long or too short — resulting in parts where the bend-to-edge or bend-to-hole dimensions are out of spec.

What tolerances can sheet metal fabrication achieve?

Tolerances vary by operation: Laser cutting: ±0.005 in. (±0.13 mm) on flat dimensions. Single-bend dimensions: ±0.010 in. (±0.25 mm). Multi-bend (cumulative): ±0.030 in. (±0.76 mm). Bend angle: ±1°. Hole-to-bend dimensions: ±0.010 in. (±0.25 mm). PEM insert diameters: +0.003/−0.000 in. These are standard tolerances for CNC press brake and fiber laser equipment. Tighter tolerances are achievable on specific features with secondary operations (e.g., CNC machining a critical hole after forming), but this adds cost.

When should I use laser cutting vs. waterjet vs. plasma?

Laser cutting (fiber or CO2) is the default for most sheet metal work — it handles aluminum, steel, and stainless up to 0.5 in. (12.7 mm) with ±0.005 in. tolerances and a clean, burr-free edge. Waterjet cutting is the choice when you need to cut heat-sensitive materials (titanium, composites, glass, stone), very thick stock (up to 6 in. / 150 mm), or when you cannot have a heat-affected zone (HAZ). Waterjet tolerances are typically ±0.003–0.005 in. Plasma cutting is the economical choice for thick carbon steel and stainless (0.5–2 in.) where edge quality is less critical — tolerances are ±0.015–0.030 in. with a rougher edge that typically needs grinding.

What is the minimum bend radius for common sheet metals?

Minimum inside bend radius depends on the alloy and temper: 5052-H32 aluminum: 0.5× thickness (very formable). 6061-T6 aluminum: 1.0× thickness (less ductile, cracks at tighter radii). 304 stainless steel: 0.5–1.0× thickness depending on temper. A36 carbon steel: 0.5× thickness. 1008/1010 cold-rolled steel: 0.5× thickness. Brass C260: 0.5× thickness. Going below the minimum radius causes cracking on the outer surface of the bend. As a rule, softer tempers (annealed, H32) bend tighter than harder tempers (T6, full-hard). Always specify the bend radius on your drawing — do not leave it to the shop to guess.

What file format should I send for a sheet metal quote?

Send a 3D model (STEP preferred) and a 2D engineering drawing (PDF). For sheet metal specifically: the 3D model should be modeled as a sheet metal part in your CAD software (SolidWorks Sheet Metal, Fusion 360 Sheet Metal) so the flat pattern can be extracted automatically. A DXF of the flat pattern is helpful but not required — most fabricators will unfold the model themselves. The 2D drawing should call out material, thickness, bend radii, tolerances, hardware (PEM inserts, rivets), and finish. Missing any of these creates an RFI that delays your quote.

What are PEM fasteners and when do I use them?

PEM (Penn Engineering & Manufacturing) fasteners are self-clinching hardware — studs, nuts, and standoffs that are pressed into sheet metal during fabrication. They create permanent, load-bearing threads in thin sheet that would strip if you tried to tap directly. Use PEM fasteners when: the sheet is too thin to tap (< 3× thread pitch), you need the fastener flush with one surface, or you need a captive nut on a panel for field assembly. Common types: CLS (flush nuts), FH (flush-head studs), SO (standoffs), BSO (blind standoffs). Specify PEM part numbers on your drawing — e.g., "CLS-M4-2 (press from this side)."