Super-Ingenuity (SPI)

Precision Manufacturing: 5-Axis CNC Machining, Injection Molds, and Rapid Prototyping Solutions.

ISO 9001 & IATF 16949 CERTIFIED
+(86) 0769 8166 7180 / sales-6@super-ingenuity.cn
24h Quotation · Free DFM Support · Global Shipping
Get Instant Quote

CAD Ready: STEP, IGES, STL supported

Sheet Metal Design Guide

Sheet Metal Design Guidelines (DFM): Bends, Holes, Hardware & Tolerances

Sheet metal design is the set of geometry, tolerance, and assembly decisions that determine whether parts can be cut, bent, joined, and finished reliably at the target cost and lead time. This guide focuses on practical DFM rules for bending, hole placement, relief features, self-clinching hardware, tolerances, and finishing.

Use the cheat sheet first, then follow the section-by-section rules to avoid common failures such as hole distortion near bends, corner tearing, weld distortion, and coating-related fit issues. If you’re designing an enclosure, bracket, panel, or chassis, start from the cheat sheet and treat this page as your DFM reference.

What you’ll get

  • Rule-based DFM tables for bends, holes, flanges, hardware, and finishing.
  • A copy-ready Pre-RFQ checklist to cut quoting back-and-forth.
  • FAQ and external references you can share with your team or suppliers.

Related resources: Laser Cutting service, Materials guide (grades + equivalency), Surface Finishing guide (coating thickness + masking), or Free DFM (upload CAD/drawing).

Sheet Metal DFM Quick Reference (Cheat Sheet)

Use this table to screen your sheet metal design in 60 seconds before RFQ. These are baseline rules—tight cosmetic or precision assemblies should be validated with a bend coupon and an inspection plan to confirm flat patterns, bend angles, and hole positions.

DFM Quick Rules
Topic Practical rule of thumb Why it matters
Minimum flange length Use flange length ≥ 4× thickness (4t) (e.g. 1 mm sheet → ≥ 4 mm / 0.16 in). Ensures tooling grip and bend stability; reduces angle drift and deformation. protolabs.com
Holes near bends Keep holes ≥ 2× thickness (2t) from the start of the bend radius (e.g. 1 mm sheet → ≥ 2 mm / 0.08 in). Prevents hole distortion, keyhole shapes, or unintended relief behavior during bending. Protolabs Network
Standardize bend radius Use a consistent inside radius across bends (e.g. 1.0–1.5 mm / 0.04–0.06 in for 1 mm sheet). Fewer tooling changes and bend setups, better repeatability and lower cost. protolabs.com
Bend relief at corners Add relief where flanges meet; keep width ≥ 0.8 mm / 0.03 in or above your cutting + deburr capability. Prevents corner bulging, tearing, and uncontrolled cracking at intersecting bends. protolabs.com
K-factor / flat pattern Start with K-factor in the range 0.30–0.45, then calibrate per material/thickness using a test coupon. Improves flat pattern accuracy and reduces tryout loops and scrap during first articles. cdn2.hubspot.net
Self-clinching hardware Follow manufacturer C/L-to-edge ≥ spec (typically a few mm / 0.1 in+ depending on series and sheet thickness). Too close to an edge weakens clinch performance and can cause cracking or pull-out. PEM + others
General tolerances Use an ISO 2768 general tolerance (for example, ISO 2768–mK) for non-critical dimensions, and specify CTQs with explicit tolerances. Avoids “tight everywhere” title blocks and focuses control effort on truly critical features. Super-Ingenuity (SPI)

Material & Thickness Selection

Choose sheet metal material based on strength, corrosion environment, formability, weldability, and finishing requirements. The right combination of grade and thickness decides how easily parts can be cut, bent, joined, and coated—and how stable they are in production.

Strength vs. weight Corrosion environment Formability & springback Finish & appearance

How to think about material & thickness

Start from performance and environment, then narrow by formability and finishing.

Avoid chasing one “perfect grade” before you understand loads, corrosion, and how the part will be assembled. Material choice, thickness, and forming method should be decided as a set.

  • Begin with function: define loads, stiffness targets, and whether the part is cosmetic, structural, or both.
  • Match environment: indoor vs. outdoor, wash-down, chemicals, and required life often decide between carbon steel, stainless steel, and aluminum.
  • Check forming window: tight bends, hems, and deep forms may push you toward more formable grades and larger minimum bend radii.
  • Plan the finish early: paint, powder, anodize, or plating all add thickness and can change clearances and edge behavior.
  • Thickness as a system decision: don’t just “go thicker”; combine thickness with ribs, flanges, beads, and weld strategy to control cost and distortion.

Related references: see Materials guide (grade equivalents, strength, machinability) and Surface Finishing guide (coating thickness and inspection) .

Bending Fundamentals (inside radius, springback, K-factor, flat pattern)

Good bend design starts with intentional inside radii, realistic springback expectations, and calibrated K-factors. These fundamentals drive flat pattern accuracy, bend consistency, and how many loops you need between CAD and the press brake.

1) Inside bend radius & springback

Standardize bend radii across a part or assembly to reduce setup time and variation. Use a small set of house radii that match available tooling and material thicknesses, instead of “random” values from CAD defaults. Source: protolabs.com

Expect more springback on high-strength alloys and stainless steels. Critical bend angles should be validated with a test coupon using the same material, thickness, grain direction, and tooling as production.

For cosmetic-critical bends, define an acceptable angle tolerance and inspection method (angle gauge or CMM) so the brake operator knows how much overbend is required to land within the finished tolerance.

Production approach (SOP)

  1. Choose house bend radii per material / thickness based on available tooling.
  2. Run a short coupon trial to confirm actual springback for each combination.
  3. Document overbend targets and angle tolerances in your bend table or work instructions.
  4. Apply the same parameters to all similar parts to stabilize angle and flat pattern results.

Flanges, Hems, Offsets & Formed Features

Use these rules to keep bends stable, edges safe to handle, and formed details compatible with hardware, coating, and press-brake capability.

Flanges — minimum length for press-brake grip

Baseline rule: flange length ≥ 4× thickness (4t)

A widely used manufacturability baseline is flange length ≥ 4t. Below this, parts become harder to grip and angle variation increases—especially for small parts and high-strength materials.

Common failures when flanges are too short: fingers slip and mark the part, bend angle drifts between hits, and operators start “double-hitting” bends to compensate, which hurts repeatability.

Hems — safety edge + stiffness

Use hems to remove sharp edges and increase stiffness and perceived quality. Plan hem direction so it does not clash with hardware, cable routes, or panel stacking, and leave room for coating build-up.

Typical issues when hems are not planned: trapped powder/paint causing fit problems, and hem legs that are too short to form cleanly, leaving a sharp “knife edge”.

Offsets / joggles

Offsets often require more clearance than a simple bend because of tool geometry and springback. Avoid extremely tight offset gaps unless you have validated them with actual tooling and sample parts.

Treat offsets as stack-up amplifiers: if the gap is critical, consider adding adjustability elsewhere or relaxing the cosmetic requirement.

Formed features (louvers, emboss, beads)

Use formed features to add stiffness without increasing thickness. Keep louvers, embosses, and beads away from tight bends, hardware keep-out zones, and sealing surfaces so the forming load does not disturb those areas.

Holes, Slots & Cutouts (distance rules + min sizes)

Holes and slots are often “easy” in CAD but costly on the shop floor when they sit too close to bends or edges. Use the rules and CTQ reminders below to keep roundness, fit, and deburring under control.

1) Hole-to-bend distance

If a hole is too close to a bend, it may ovalize or behave like an unintended relief cut. A common baseline rule is placing holes at least 2t from the start of the bend radius.

More conservative: 2.5t + R (or higher) Apply to slots, CTQ holes, and cosmetic faces
CTQ vs. non-CTQ guideline:
  • Locating / assembly CTQ holes: use 2.5t + R or your house conservative rule.
  • Visible cosmetic holes: treat as CTQ for distance and roundness control.
  • Non-critical clearance holes: 2t is usually acceptable if forming trials look stable.

2) Minimum hole / slot size

Very small features often lose roundness, burn, taper, or become hard to deburr consistently. A practical starting point is feature size ≥ thickness (≥ t), and increase for stainless or high-strength alloys.

If CTQ: drill / ream instead of tiny laser Reserve space for deburr tools

3) Hole-to-edge distance

Keep adequate edge margin to avoid tearing and distortion during bending and fastener installation. For hardware holes, follow the fastener manufacturer’s edge-distance rules instead of guessing.

With PEM / rivet nut: always use published C/L-to-edge Move non-CTQ holes inward to add margin

Quick takeaway

Protect the bend zone and the edge zone. Moving a hole 1–2 mm in CAD is cheap; scrapping parts after forming is not.

t = sheet thickness R = inside bend radius

Bend Relief & Corner Relief (when required + sizes)

Relief cuts are small details with big impact. They prevent bulging, tearing, and unpredictable corner distortion when flanges intersect—especially on tighter bends or thicker materials.

When do you need bend relief?

When two flanges meet at a corner, relief prevents bulging, tearing, and unpredictable deformation at the junction.

  • Two bends intersect at a corner (flange-to-flange junction).
  • Tighter inside radius or thicker sheet significantly increases corner stress.
  • Cosmetic corners or locating flanges need stable geometry and repeatable forming.

Too small reliefs tend to cut poorly, leave hard-to-control burrs, and may not fully open during forming; too large reliefs can weaken the corner, reduce stiffness, and visibly break the outer profile line.

Relief shape options: round, rectangular, or teardrop. Use round or teardrop for smoother stress distribution, and rectangular only when you need crisp alignment to adjacent features.

Practical minimums (baseline)

Stable corners
Relief width

A common published baseline for relief notch width is around 0.030 in (0.76 mm), treated as a small but non-zero cut. Use a consistent house minimum sized above your laser kerf and deburr capability.

Relief length

Extend relief beyond the bend radius so stress doesn’t concentrate at the corner.

Consistency

Keep relief geometry consistent across similar parts to stabilize results and reduce variation.

Design guidance

Use a simple internal checklist so reliefs are manufacturable, repeatable, and aligned with your forming window.

  • Extend relief past the bend radius; do not stop it inside the most stressed corner zone.
  • Use a repeatable relief shape (round / teardrop) for better stress flow and easier QC.
  • Size relief so it is manufacturable (clean cut + repeatable deburr), not “zero width” in CAD.
Corner relief before versus after: left without relief showing bulging and cracking, right with relief showing a clean, stable corner
Corner relief — before vs after: without relief (bulging / cracking) versus with relief (clean, stable corner). Use a small, repeatable notch instead of letting the corner tear unpredictably.

Hardware (PEM, rivet nuts, standoffs) & Assembly Clearances

Hardware is where “small geometry” becomes real assembly risk. Use manufacturer rules for edge distance, plan press access, and sequence finishing correctly to keep clinch strength and thread quality consistent.

Self-clinching hardware (PEM® style)

Do not guess edge distances—use the manufacturer’s C/L-to-edge rules. If a fastener is close to multiple edges, published performance may not apply and pull-out results will drift.

Rule: If you’re “close to two edges,” treat it as a special case and validate with the fastener spec (or redesign) before locking the flat pattern.
  • Install before paint/powder coating

    Do not install self-clinching fasteners after finishing—this reduces clinch performance and can crack coatings. Install hardware first, then finish; protect threads with masking if needed.

  • Match hardware series to sheet thickness

    Confirm the sheet thickness range supports the chosen hardware series. Avoid “almost fits” selections that sit off-spec for grip range or sheet hardness.

  • Reserve keep-out zones for press access

    Plan clearance around each fastener so the anvil and punch can reach the location without colliding with bends, flanges, or nearby hardware.

  • Define install direction & alternatives

    Specify installation direction and whether one-side access is required. If hardware must be installed after finishing or from one side only, consider rivet nuts or threaded inserts as alternatives to self-clinching studs.

Joining Methods (welding/riveting/adhesive) + distortion control

Joining choice affects cost, serviceability, and—most importantly—shape stability. Use the guidance below to keep assemblies easy to build, easy to repair, and predictable in final fit.

Weld distortion patterns & mitigation (visual)

Long, asymmetric welds tend to pull parts into bending or twist. Symmetric weld patterns, stitch welds, and proper fixturing help keep enclosures and frames within tolerance.

Weld distortion patterns showing bending and twisting from long welds, with symmetric and stitch welds reducing distortion
Weld distortion patterns & mitigation: long, asymmetric welds drive bending and twist; symmetric welds, stitch welds, and fixtures absorb distortion instead of the part.

Riveting / screws (fast iteration, serviceable)

Great for modular repair and rapid iteration. Watch for stacked tolerances, tool access, and vibration loosening in field applications.

Welding (strong, sealed, but distortion risk)

Predict distortion when weld lengths are long or asymmetric. For enclosures, plan weld sequence and fixturing early. Where fit is critical, add locating tabs/features and define post-weld straightening allowance.

Adhesive bonding (quiet, no heat, but process-sensitive)

Adhesives can reduce noise and avoid heat distortion, but require controlled surface prep, bond-line thickness, cure time, and inspection access. Define the process early so production stays repeatable.

Joining method — quick selection table

Use this as a first-pass filter. The final choice still depends on coating, environment, serviceability, and how much distortion you can tolerate.

Joining method Advantages Risks / limits Typical use cases
Welding High strength, sealed joints, no loose hardware. Good for permanent structures and frames. Distortion, residual stress, rework cost if geometry drifts. Sequence + fixture must be defined. Structural frames, sealed enclosures, brackets that never need disassembly.
Rivets / screws Serviceable, easy to replace in the field, low heat input, simple tooling. More parts and assembly steps, potential loosening under vibration, visible heads. Access panels, covers, modules that need frequent repair or design changes.
Adhesive bonding No weld distortion, good damping, can join dissimilar materials, clean exterior surfaces. Process-sensitive (surface prep, cure, environment), longer cycle time, harder to inspect. Large cosmetic panels, mixed-material assemblies, noise-critical housings and covers.

Tolerances & Drawing Practices (ISO 2768, datums, CTQ)

Good drawings keep general tolerances simple, highlight CTQ dimensions, and show how the part will be measured. Use ISO 2768 for unspecified dimensions, then build a datum scheme around the real mounting interfaces.

Drawing mini-example: datum scheme for an enclosure bracket

Engineering drawing example showing an enclosure bracket with datum A as the mounting face, datum B as the hole pattern, and datum C as a locating edge.
A = mounting face, B = hole pattern, C = locating edge. CTQ dimensions reference back to A–B–C so the part is inspected as assembled.
  • Choose datums from what the part actually bolts or seals to (faces and hole patterns).
  • Keep CTQ dimensions tied to those datums; avoid “floating” dimensions with no clear reference.
  • Group cosmetic notes (finish class, scratch limits, edge break) away from dimensional CTQs.

ISO 2768 & bend-angle clarity

ISO 2768 is a clean way to control non-critical dimensions without filling the print with repeated notes. It works best when CTQs and inspection methods are clearly separated.

  • Apply an ISO 2768 general tolerance class to cover non-critical dimensions consistently.
  • Mark CTQ dimensions with explicit limits (e.g. hole position, flatness, enclosure width) and, if needed, the inspection method.
  • Reserve very tight limits for mounting interfaces, sealing faces, and functional hole patterns—not for every edge.
  • For bend angles: state which angles are critical and how they are measured (inside vs outside angle, over which leg length, and relative to which datum).

Related pages

Quotation FAQ (what tolerances to specify) Use this to decide which tolerances and CTQs to include in your RFQ package. Quality assurance (CMM / inspection capability) See how CTQs are measured in production: CMM, gauges, sampling plans, and reporting.

Surface Finishing for Sheet Metal (powder/anodize/plating)

Choose finishing based on corrosion environment, appearance, electrical contact needs, and masking constraints. The right finish protects the part in the field and still fits after coating thickness is added.

Finish types: what they’re good at

  • Powder coating Durable, good coverage, wide color range. Plan masking for threads, grounding pads, and tight-fit interfaces; typical thickness (e.g. 60–100 µm) eats into clearance and can close small gaps.
  • Anodizing (Aluminum) Improves corrosion resistance and appearance while keeping weight low. Hard anodize is more brittle at bend radii, so avoid forming after coating and protect sealing faces from overbuild where fit is critical.
  • Plating / passivation Thin metallic layers (zinc, nickel, etc.) and chemical treatments for steel or stainless. Watch for brittle coatings at bends and edge chipping if parts are formed or reworked after plating.

Coating thickness & fit: always stack up coating on both mating parts in your clearance budget. A few tens of microns on each side can turn a smooth slide fit into an interference fit after finishing.

Masking & assembly gaps (fit-first view)

  • Mask threads and mating surfaces Do not coat internal threads, press-fit holes, or precision locating faces. Call out masking for tapped holes, dowel holes, and gasket contact areas on the drawing.
  • Plan electrical contact points Reserve bare-metal pads for grounding lugs, EMI gaskets, or bonding straps. Mark these as “no paint / no anodize” so masking and inspection can follow.
  • Sequence with forming and hardware Install self-clinching hardware before paint or powder coating, and avoid forming after brittle coatings unless validated. This reduces clinch failures and edge chipping at bend radii.

Use your coating vendor’s thickness and masking data in the tolerance stack so “as-coated” parts still meet gap, flatness, and alignment requirements in the final assembly.

Surface Finishing (thickness, masking, inspection) See full coating tables & masking examples

End-to-End Workflow (DFM → prototype → production)

A repeatable workflow turns sheet metal parts from “works on CAD” into “builds every time”. The steps below help you reduce iteration loops, stabilize bends, and lock inspection-critical dimensions early.

1

Requirements gathering

Capture loads, environment, and the assembly interfaces that drive fit and function.

LoadsEnvironmentInterfaces
2

Concept CAD + quick DFM screen

Run a fast feasibility screen using your cheat sheet before you invest in detailed drawings.

Quick screenCheat sheetRisk flags
3

DFM review with manufacturing + QA

Review bends, holes, reliefs, hardware, and finish—then align on inspection approach for CTQs.

BendsHardwareFinishCTQ
4

Prototype & fit-check

Build prototypes and confirm fit; use coupon bends to calibrate K-factor and angle repeatability.

PrototypeFit-checkK-factor
5

Update flat pattern tables + finalize drawing notes

Lock flat patterns, datums, and CTQs; finalize notes so production and inspection read the same intent.

Flat patternDatumsDrawing notes
6

Production release + inspection plan + continuous improvement

Release to production with an inspection plan; feed lessons back into standards to improve future builds.

Inspection planControlCI

Case Study — Telecom Base-Station Enclosure

A telecom OEM asked us to redesign a legacy base-station enclosure that was heavy, expensive to weld, and difficult to assemble in the field. By systematically applying the rules from this guide, we turned “one-off tribal knowledge” into a repeatable design pattern.

From over-built legacy to lean, repeatable enclosure

The original design used thick sheet, long continuous welds, and ad-hoc hardware placement. Installers struggled with alignment, and manufacturing saw high weld distortion and rework. Together with the customer, we re-mapped the enclosure using geometry-first stiffness, smarter joining, and process-appropriate cutting.

Results: Weight −25%, cost −18%, assembly hours −30%.

Cost Drivers & Economic Optimization (LCC)

When optimizing cost, focus first on the drivers you can influence at the design stage. Life-cycle cost (LCC) then becomes a structured way to measure how those design choices translate into material, processing, and rework spend.

Design-stage cost drivers

Control these early knobs before you negotiate price:

  • Batch size & setup Standardize radii, thickness, and hardware families to reduce changeovers and setup time.
  • Process complexity Reduce bend count, welding steps, and secondary operations where possible.
  • Inspection & rework Define CTQs, datums, and practical tolerances so inspection effort matches real functional risk.

Design actions with highest ROI

  • Reduce operations before reducing material thickness (keep stiffness and robustness first).
  • Replace welds with tabs/fasteners where sealing isn’t required to cut distortion and labor cost.
  • Avoid tight tolerances on non-functional faces; reserve precision for interfaces and CTQs.

Digitalization & Simulation (Digital twin/FEA/monitoring)

Digital tools shift sheet metal from “trial and error” to predictive control. Use simulation and data when the risk of distortion, rework, or downtime justifies a virtual test first.

Digital Twin

  • Build a digital twin of the sheet metal part to provide real-time feedback on production status, deformation trends, and residual stresses.
  • Optimize cutting paths and stress validation virtually to catch design flaws early.

Online Monitoring & Feedback

  • Integrate IoT sensors to capture bending force, vibration, and temperature data in real time, automatically adjusting bend speeds or tooling.
  • Leverage big-data analytics to continuously refine process parameters, reducing scrap rates and energy consumption.

Common Pitfalls (rule-based)

Use this table as a failure-prevention checklist during CAD review. Each pitfall maps to a simple, rule-based mitigation you can apply before releasing drawings.

Pitfall Consequence Mitigation
Holes too close to bends Oval holes, cracks Rule: keep ≥ 2t from bend radius start.
Missing bend relief at corners Bulging, tearing at junction Rule: add corner relief and maintain a consistent minimum size.
Flange too short Angle drift, press-brake marks Rule: use flange length ≥ 4t for stable gripping.
Hardware too close to edge Weak clinch, edge distortion Rule: follow PEM C/L-to-edge specification for the selected series.
Coating applied before hardware Clinch failure / reduced performance Rule: install self-clinching hardware before paint/powder; mask threads as needed.

Pre-RFQ Sheet Metal Checklist (copy-ready)

Use this checklist to reduce RFQ back-and-forth and speed up quoting + DFM. Confirm the points below before you send CAD and drawings to your supplier.

  1. Material / thickness / quantity are specified.
  2. Finish is specified (powder / anodize / plating), and masking zones are defined.
  3. Bend radii are standardized where possible.
  4. Flange length meets tooling constraints (baseline: flange ≥ 4t).
  5. Holes/slots clearance to bends and edges follows DFM rules; CTQs are marked.
  6. Bend relief / corner relief exists at junctions where flanges meet.
  7. Hardware type is defined (PEM / rivet nuts / standoffs) and follows manufacturer C/L-to-edge constraints.
  8. Joining method is specified (weld / rivet / screw / adhesive) and assembly access is considered.
  9. Datums + inspection plan are clear (CMM / gauges / go-no-go).
  10. Packaging / handling requirements are defined for cosmetic or sensitive parts.

FAQ

What is the minimum flange length in sheet metal bending?

A common baseline is flange length ≥ 4× thickness (4t). Shorter flanges reduce tooling grip and increase angle variation and marks.

How far should holes be from a bend line?

Keep holes at least 2× thickness away from the bend radius start. Increase distance for slots, CTQ features, and cosmetic faces.

What is a good bend radius for sheet metal parts?

Use a consistent bend radius across the part to improve repeatability. Validate extreme or tight radii with coupons due to springback.

When do you need bend relief or corner relief?

Add relief where flanges meet to prevent bulging and tearing. Keep the relief above your laser-cut + deburr capability.

What is K-factor and why does my flat pattern not match?

K-factor sets the neutral axis position and affects bend allowance. Start with a typical K-range and calibrate using test coupons.

What is the minimum hole size for laser cutting?

Avoid holes smaller than material thickness. Increase size for stainless, high-strength alloys, or tight roundness requirements.

Can I install PEM hardware after powder coating?

Generally no—coating reduces clinch performance. Install hardware before finishing and mask threads as needed.

How do I control welding distortion on large enclosures?

Use symmetric welds, proper fixturing, and stitch welding when sealing isn’t required. Add locating features to stabilize fit.

Should I use ISO 2768 for general tolerances?

Yes—ISO 2768 simplifies drawings for non-critical dimensions. Mark CTQs and datums clearly to avoid over-tolerancing.

Laser cutting vs punching—how do I choose?

Laser is best for complex profiles and low-mid volume; punching is efficient for high-volume hole patterns. Hybrid flows often save cost.

Get a 24-Hour DFM Check for Your Sheet Metal Part

Upload your CAD/drawing and we’ll return a concise 1-page DFM note to help you reduce bends/holes/relief risks, stabilize fit, and lock CTQ inspection intent before prototype or production.

What you get

  • High-risk bend & hole placement flags
  • Relief / keep-out / hardware access notes
  • Finish-related fit & cosmetic risk notes

What to upload

  • 3D CAD + drawing (or PDF)
  • Material, thickness, finish target
  • Quantity + CTQ / datum notes

Typical turnaround

  • DFM feedback: within 24 hours
  • Fast quote: after DFM alignment
  • Prototype → production support
Free DFM (24h) Contact Us Laser Cutting Service

Tip: Include material, thickness, finish, quantity, and CTQ dimensions for the fastest, most accurate feedback.

References (external) + Related Guides (internal)

The rules in this guide are grounded in widely used sheet metal references and our own manufacturing experience. Use the links below for deeper dives into standards, hardware specs, and related design topics.

External references

Protolabs — Sheet Metal Design Guidelines Baseline rules for flange length (4t), consistent bend radii, and general DFM limits. protolabs.com Hubs — Sheet Metal Fabrication Design Guide Practical guidance on hole-to-bend distances (≥ 2t), features, and process capabilities. hubs.com PEM — C/L To Edge Tech Sheet Defines centerline-to-edge requirements for self-clinching hardware. pemnet.com PEM — Self-Clinching Fastener Handbook Installation practices, including installing before paint/powder coating. pemnet.com

Partner with SPI

Work With a CNC & Mold Manufacturer You Can Audit

Welcome to SPI — an ISO9001/IATF16949-focused CNC machining and injection molding partner in Dongguan, China.

We combine tight-tolerance machining, documented inspection and responsive engineering support to help you move from RFQ to stable production faster, with full traceability and audit-ready quality records.

Share your drawings and requirements — our engineers can suggest practical tolerances, surface finishes and inspection plans before you lock your RFQ.

Go to Contact Us & Request a Quote

Use the Contact Us form to upload STEP/IGES files and add notes about tolerances, surface finish and inspection.

Prefer email? Reach us via the form on the Contact Us page and ask to be added to our CNC DFM mailing list.

SPI CNC and mold manufacturing facility in Dongguan, China
On-site audits & factory visits welcome

Related Posts