Sheet metal design guide
Plan flat, bent and assembled sheet metal parts with clear material, cut-feature, bend, hardware and inspection requirements. Explore bend allowance before releasing the flat pattern.
Start with the manufacturing route
A flat plate, formed bracket and welded enclosure share cutting requirements, but their final fit depends on different operations.
Flat
Plates, panels and gussets
Review the outline, holes, narrow webs, edge condition and flatness. Finishing and fastener installation may still change the delivered part.
Formed
Brackets and channels
Add the bend radius, angle, feature clearances and tooling access. Dimensions across bends need a separate tolerance review.
Assembled
Enclosures and frames
Include the joint, hardware, finish and final assembly datums. Review how the parts are located, joined and measured together.
Continue by part type: enclosures, brackets or welded assemblies.
Name the grade, condition and thickness
Choose the material for the environment, loads, forming route and finish. Stock form and temper matter; the alloy name alone is not a complete specification.
| Material | Sheet | Bend radius | Formability | Cost | Use it for |
|---|---|---|---|---|---|
| Steel 1008 | 0.5–3 mm | R ≥ 1 × Tmoderate spring-back · bend across grain | Excellent | $ | Stamped covers and enclosure panels; Sheet metal brackets; Deep-drawn appliance housings |
| Steel 1018 | 3–12 mm | R ≥ 1 × Tmoderate spring-back · bend across grain | Very good | $ | Motor shafts; Tie rods; Machined pins, spacers and bushings |
| Steel A36 | 3–20 mm | R ≥ 1.5 × Tmoderate spring-back · bend across grain | Very good | $ | Welded structural frames; Base plates and gussets; Machine bases and heavy weldments |
| Stainless Steel 304 | 0.5–6 mm | R ≥ 1 × Thigh spring-back · bend across grain | Very good | $$ | Food processing equipment; Kitchen appliances and sinks; Sanitary tanks and process piping |
| Stainless Steel 316L | 0.5–6 mm | R ≥ 1 × Thigh spring-back · bend across grain | Very good | $$$$ | Welded marine structures and hardware; Pump and valve bodies for seawater; Medical device enclosures and instruments |
| Stainless Steel 430 | 0.5–3 mm | R ≥ 1 × Thigh spring-back · bend across grain | Good | $$ | Refrigerator and appliance panels; Automotive trim strips; Kitchenware and sinks |
| Aluminum 3003 | 0.5–6 mm | R ≥ 0.5 × Tlow spring-back | Excellent | $ | Sheet metal enclosures and panels; Brazed heat-exchanger fins and tubes; Chemical process equipment |
| Aluminum 5052 | 0.5–6 mm | R ≥ 0.5 × Tlow spring-back | Excellent | $ | Sheet metal chassis and enclosures; Fuel and pressure tanks; Marine hardware |
| Aluminum 5754 | 0.5–6 mm | R ≥ 0.5 × Tlow spring-back | Excellent | $ | Automotive inner body panels; Floor and tread plate; Marine and vehicle sheet panels |
| Aluminum 5005 | 0.5–3 mm | R ≥ 0.5 × Tlow spring-back | Excellent | $ | Architectural curtain-wall and cladding panels; Decorative trim and sign faces; Electrical enclosures and covers |
| Aluminum 6061 | 1–12 mm | R ≥ 2.5 × Tmoderate spring-back · bend across grain · better kept flat | Fair | $ | General CNC machined parts; Aerospace and structural brackets; Hydraulic manifolds and valve bodies |
| Copper Alloy C11000 | 0.5–3 mm | R ≥ 0.5 × Tlow spring-back | Excellent | $$$$ | Electrical busbars; Grounding straps and connectors; Terminals and cable lugs |
| Copper Alloy C26000 | 0.5–3 mm | R ≥ 1 × Tmoderate spring-back · bend across grain | Excellent | $$$$ | Ammunition cartridge cases; Deep-drawn cups and shells; Brass enclosures and housings |
| Titanium Grade 2 | 0.5–6 mm | R ≥ 2 × Thigh spring-back · bend across grain · better kept flat | Good | $$$$$ | Marine hardware and seawater fittings; Heat exchanger tube and tubesheets; Chemical process piping and vessel liners |
These are library screening values, not guaranteed tooling limits or stock availability. Radius depends on temper, thickness, grain direction and forming method; confirm the selected material with the fabricator. Relative cost is not a quotation.
- Use a uniform starting thickness. A sheet-metal part starts as sheet stock. Local thickness changes require another operation or component and should be called out explicitly.
- Check availability. Specify thickness in millimeters or inches, with the grade and condition. Gauge numbers differ by material; preferred stock sizes vary by supplier and region.
- Check stiffness and strength. Deflection, buckling, fatigue, yielding and attachment loads can all matter. A return flange may improve stiffness, but the complete load path still needs evaluation.
Design the cut features for their final job
Minimum holes, webs and slots depend on the cutting process, stock and required edge quality. Treat a generic thickness multiple as an early screening aid, then confirm the actual feature.
Laser cutting, punching and waterjet have different process limits. A finished precision hole may need a secondary operation. The sheet metal cost guide explains how the route, cut length, operations and quantity affect a quotation.
| Feature | Define | Manufacturing check |
|---|---|---|
| Small hole | Finished diameter, tolerance and whether it locates or only clears a fastener. | Cut-edge taper, piercing quality and whether drilling or reaming is needed. |
| Narrow web or tab | Width, length and handling or structural function. | Heat distortion, stability during cutting, deburring and service loading. |
| Slot | Width, end radius, length and adjustment direction. | Cutting quality, web stability and adequate bearing under the fastener. |
| Countersink | Fastener standard, included angle, major diameter and remaining material. | Enough sheet for the recess; consider a formed dimple or different attachment where appropriate. |
| Lettering | Etched or cut-through, character size and artwork. | Cut-through islands need bridges; marking may avoid fragile fine features. |
| Edges | Deburring, edge break and any cosmetic or sealing requirement. | Which edges remain accessible after forming and assembly. |
Bend radius and clearance depend on the forming setup
Define the bend geometry
T is sheet thickness and R is the inside radius. The outside corner has radius R + T; mating parts must clear that real shape.
Keep features out of the forming zone
Dimension the hole edge from the bend tangent, then confirm the required clearance for the actual die opening and material. A center distance alone can hide an overlap.
| Decision | Define | Confirm with the fabricator |
|---|---|---|
| Inside radius R | Required geometry, alloy/temper and thickness T. | Feasible radius for the selected material and method; R = T is not universal. |
| Minimum flange | Finished flange height and bend angle. | Support on the die and ability to locate the part during forming. |
| Hole-to-bend clearance | Hole edge to bend tangent, with diameter shown. | Deformation zone for the chosen die opening, material and orientation. |
| Relief and corner gap | Relief geometry and whether the corner stays open or is joined. | Avoid torn edges, overlapping flanges and local distortion. |
| Hem or return | Fold geometry, finished gap and functional edge requirement. | Tooling, material ductility and access; a hem is not an ordinary single bend. |
| Bend sequence | The complete folded model and internal features. | Punch, back-gauge and part clearance throughout the sequence. |
- Use consistent radii where function permits. This can simplify tooling and bend tables, but do not change a mating radius without checking the assembly.
- Account for rolling direction. Some alloys and tempers are sensitive to bend direction relative to the rolling grain. Confirm it for tight or critical bends.
- Separate springback from flat development. A K-factor describes neutral-axis position in the flat-length model. It does not by itself determine springback compensation or minimum bendability.
Understand bend allowance before trusting the flat pattern
Bend allowance is the developed arc length through the bend. Bend deduction connects that arc to dimensions measured at the outside virtual sharp corner.
Explore one bend
This geometry example uses two outside leg dimensions measured to their virtual sharp corner. It does not select a safe bend radius, tooling or a production K-factor.
Illustrative developed length
62.084 mm flat length
Bend allowance: 4.084 mm · Outside setback: 3.5 mm · Bend deduction: 2.916 mm.
Included angle after bending: 90°. Rounded values are for display, not a precision guarantee.
BA = θ × π / 180 × (R + K × T). Outside setback = (R + T) × tan(θ / 2). Bend deduction = 2 × setback − BA. Flat length = A + B − bend deduction.
θ is in degrees. A and B are outside virtual-sharp dimensions, not straight lengths to the bend tangents. The model covers one ideal bend and excludes springback compensation, hems, stretch forming and material/process validation. Confirm the released flat pattern against the fabricator’s bend table.
For the starting example, T = 1.5 mm, R = 2 mm, K = 0.4 and a 90° bend give 4.084 mm of bend allowance. Outside legs of 40 mm and 25 mm give a 62.084 mm developed length in this ideal model. These inputs illustrate the calculation; the shop's measured bend table establishes the production values.
When CAD and a supplied flat DXF disagree, resolve which file controls the finished geometry before cutting. Do not silently mix one shop’s bend table with another shop’s tooling.
Let the exact fastener determine its installation feature
| Attachment | Define | Check |
|---|---|---|
| Self-clinching hardware | Maker, part number, material and installation side. | Sheet thickness/hardness, exact hole tolerance, edge distance and press access. |
| Rivet nut | Thread, grip range, body style and hole geometry. | Blind-side envelope, anti-rotation requirements and installation setting. |
| Welded nut or stud | Exact part, material and joint requirements. | Welding access, distortion and restoration of surface protection. |
| Tapped or formed thread | Thread standard, class and required engagement. | Material strength and wall thickness for the actual load; the ability to tap a hole does not prove retention. |
| Captive panel screw | Exact retaining system and mating thread. | Cover thickness, removal path and service tool access. |
Follow manufacturer instructions for hole preparation and finishing sequence. Self-clinching holes should not be casually chamfered or deburred; the specified edge is part of the installation.
Distinguish cut accuracy from formed and assembled fit
Measure from the functional interface
Locate critical holes from the mounting face and a shared origin. Long chains of intermediate dimensions accumulate variation.
Inspect the delivered condition
A welded, coated or hardware-installed assembly can differ from its cut components. Mark which dimensions apply after the final operation.
Illustrative angle effect: a 100 mm straight arm rotated by 0.5° moves its tip about 0.87 mm sideways relative to its intended direction. This geometric example explains why a hole far from a bend can move noticeably; it is not a stated press-brake tolerance.
| Requirement | Drawing approach | Process implication |
|---|---|---|
| Features on one flat | Use a common origin and define feature size/position. | Cutting quality and measurement method govern the result. |
| Feature across a bend | Define the functional datum and final location. | Bend angle, radius and flange geometry contribute to position. |
| Opposing flanges | Specify clear opening, parallelism or hole alignment as needed. | Several bends can accumulate variation; final machining or a locating feature may help. |
| Flat panel | State a flatness requirement and inspection support condition. | Stock, cutting, perforations and later operations affect flatness. |
| Finished assembly | Specify final datums and dimensions after required operations. | Welding, hardware and coating can change the assembled fit. |
Agree the general tolerance and critical feature requirements for the specific part. Do not apply a laser-cut tolerance to the entire formed box or copy a machining capability into a sheet-metal drawing.
Finish requirements belong in the dimensional plan
| Finish route | Review | Drawing detail |
|---|---|---|
| Paint or powder coat | Added layer, cure, appearance and edge/recess coverage. | Final fits, colour/texture reference, visible zones and masking. |
| Anodizing | Aluminum alloy response, conversion layer and dimensional growth. | Type/class, thickness where required, final fits and electrical contact areas. |
| Conversion coating | Substrate, corrosion and electrical-contact requirements. | Applicable type/class and acceptance test; do not specify by colour alone. |
| Plating | Substrate, thickness distribution and any embrittlement controls. | Specification, critical surfaces, final dimensions and required processing records. |
| Stainless cleanup/passivation | Contamination, weld oxides and the required surface condition. | Define cleaning versus oxide removal versus passivation as applicable. |
| Mechanical finishing | Material removal, texture and edge rounding. | Grain direction, roughness where functional and protected details. |
See surface-finish selection and the finish library for process-specific guidance. Total coating thickness and outward dimensional growth are not always the same quantity.
Carry the requirements through the full assembly
A cut and bent part is not necessarily the delivered product. Include purchased hardware, mating components, joining, surface treatment and final inspection in the same plan.
Locate
Choose functional datums
Establish where the part seats and which features locate it. Avoid asking every outside edge to control the same fit.
Assemble
Check access and sequence
Model the tools, fasteners, cover removal path and joining access. Resolve hardware and finish order before release.
Verify
Measure the final condition
Inspect critical interfaces after the operations that can change them. Use a first article to verify the assembly before repeat production.
Send files that define the finished part
- Formed geometry. STEP model and current drawing; include assembly context for important fits. Label any supplied DXF as reference or released manufacturing geometry.
- Material and operations. Grade/temper, thickness, hardware part numbers, joining requirements, finish and masking.
- Acceptance. Datums, critical dimensions, cosmetic requirements, inspection condition and required reports or tests.
- Order context. Quantity, expected repeats, revision and any first-article approval before the balance is produced.
Sheet metal design questions
What is the minimum bend radius for sheet metal?
It depends on alloy, temper, thickness, rolling direction, tooling and forming method. Use material-specific screening data, then confirm the radius with the fabricator. Inside radius equal to thickness is not a universal rule.
What is the difference between bend allowance and bend deduction?
Bend allowance is the developed neutral-axis arc length through the bend. For outside virtual-sharp dimensions, bend deduction is twice the outside setback minus bend allowance. The dimensions used in the calculation must follow that convention.
Which K-factor should I use?
Use a value or bend table calibrated to the material, thickness, tooling and process. A default CAD K-factor is suitable for an initial model, but it is not proof of production flat-pattern accuracy.
How close can a hole be to a bend?
Show the hole diameter and edge clearance from the bend tangent, then confirm the deformation zone for the actual tooling and material. If the feature must remain precise close to a bend, review a post-forming operation or a different layout.
What tolerances can sheet metal hold?
Cut, formed, welded and finish-machined features have different limits. Agree the general tolerance and critical features for the actual part size, stock and route; define which dimensions apply to the final assembly after finishing.
Should I upload STEP or DXF for a bent part?
Provide the formed STEP model and drawing so the finished intent is clear. If a flat DXF is also supplied, identify its authority and resolve the bend table with the fabricator before it is used for cutting.
Sources and further reading
- Autodesk — sheet metal rule referenceThickness, neutral-axis K-factor and bend/relief definitions.
- SOLIDWORKS — bend allowance optionsAllowance, deduction and outside virtual-sharp dimension conventions.
- SSAB — BendCalcMaterial, tooling, flange and springback variables in press-brake bending.
- TRUMPF — laser cutting technology comparisonCutting processes have different contour, material and quality constraints.
- PEM — self-clinching fastener handbookInstallation requirements are specific to the fastener and sheet.
Make the finished part clear
Upload the model and drawing with material, hardware, finish and the few dimensions that control function.