Tolerances / Metal Fabrication Guide
Sheet Metal Fabrication Tolerances: What to Expect from Your Parts
Typical sheet metal fabrication tolerances depend on the process. Laser cutting holds plus or minus 0.005 inch on cut feature positions in production. Press brake bending holds plus or minus 1 degree on bend angle. Overall part dimensions after multiple operations typically fall within plus or minus 0.010 to 0.030 inch depending on material, thickness, and how many bends accumulate in the part.
Laser Cutting Tolerances
Fiber laser cutting holds plus or minus 0.005 inch (0.13 mm) on cut feature position and size in standard production conditions. Kerf width runs 0.010 to 0.015 inch. Hole diameters land within plus or minus 0.005 inch of nominal. Tighter tolerances are possible on specific features, but come with added cost and slower cycle times.
Most flat laser cut parts ship from the table within these numbers without any special inspection or secondary operation. The CNC program drives the motion, so part-to-part repeatability is tight: the tenth part in a run matches the first. What introduces variation is material flatness, especially on thinner gauges that bow slightly, and thermal effects on narrow features cut in sequence on the same part.
Hole tolerances deserve a separate note. A circular hole cut by a fiber laser at high speed holds diameter well, but the kerf width means the actual hole diameter is the programmed diameter minus the kerf offset. Your laser cutting service team accounts for kerf offset in the CNC program so the finished hole matches the drawing dimension. If you have critical clearance holes, call them out explicitly in your drawing rather than assuming the programmer will apply a kerf correction to match fit-up.
For part geometry relative to datums, positional accuracy across a 36-inch sheet typically stays within 0.010 inch cumulatively. Beyond that range, beam path and thermal expansion factors can add a few thousandths more. For large plates with tight features at the extremes, discuss this with our team before committing to a tolerance callout.
Press Brake Bending Tolerances
Standard press brake bending holds plus or minus 1 degree on bend angle in air bending, and plus or minus 0.010 inch on formed dimensions between bends. Coining and bottoming methods reduce springback and can hold tighter angle tolerances, around plus or minus 0.5 degree, but require more tonnage and specific die selection for each material and thickness.
Angle variation in press brake work comes from springback, which is the tendency of metal to recover a small amount of bend angle after the punch withdraws. Mild steel springs back a few degrees depending on material grade and thickness; stainless steel springs back more; aluminum more still. Experienced operators compensate by overbending slightly, and CNC press brakes use back-gauge feedback to automate this. But on first-article parts in new materials, expect a setup piece or two before the angle lands reliably in tolerance.
Flange length tolerances after bending run around plus or minus 0.010 inch per bend on typical shop setups. Each bend adds a small accumulated error, so a part with five bends can accumulate plus or minus 0.050 inch on an overall envelope dimension by the time all operations are complete. If your assembly depends on a specific overall envelope size, design the tolerance around the worst-case stack-up, not the individual operation tolerance.
For detailed DFM guidance on bending, see our page on designing for press brake bending, which covers minimum radii, hole placement, and bend relief rules that keep parts within standard tolerances without special processes.
Welded Assembly Tolerances
Welded fabrications carry wider tolerances than individual cut or formed parts. Structural weldments typically hold plus or minus 1/16 inch on overall dimensions for smaller assemblies, widening to plus or minus 1/8 inch on larger frames. Weld distortion from heat input causes most of the variation. Jig welding and fixture-controlled setups bring distortion down significantly for higher-precision assemblies.
Weld distortion is the primary driver of dimensional variation in welded assemblies. Heat from the weld pool causes metal to expand and then contract as it cools, pulling the structure out of flat or square. Thin material (under 3/16 inch) distorts more readily than heavy plate. Stainless steel distorts more than mild steel because it has lower thermal conductivity and higher thermal expansion.
For production weldments where dimensional consistency matters, fabricators use welding fixtures and jigs that hold components in position during welding. The fixture forces the part to cool into the correct geometry, limiting distortion to what the material recovers on its own. This is a setup cost that adds to first-article price but pays off quickly on production runs.
Our welding service handles both structural fabrications and precision assemblies. If your assembly has critical mating dimensions, provide them as toleranced dimensions on the drawing and discuss them with our team before the first article. We’d rather address a tight call before the job starts than after.
Tolerance Stack-Up Across Multiple Operations
Each fabrication operation adds a small amount of dimensional error that accumulates across a part. A laser cut blank, then bent four times, then welded into an assembly can see three to five times the error of a simple cut part. Designing only the critical features to tight tolerances, while using a relaxed blanket tolerance for everything else, keeps parts manufacturable and cost under control.
Tolerance stack-up is where most design-fabrication disconnect happens. Engineers assign plus or minus 0.005 inch to every dimension on a drawing because that’s what the laser can hold, not realizing that the bend operations and weld ops that follow each carry their own error budget. The end result: a part that the laser cut perfectly but that fails assembly inspection on a formed dimension that had no realistic path to plus or minus 0.005 inch through bending.
The fix is selective tolerancing. Put tight tolerances on features that genuinely control assembly fit-up: the slot your hinge pin rides in, the hole your fastener must clear, the datum face your assembly references. Put a relaxed general tolerance (plus or minus 0.010 to 0.030 inch) on everything else and let the process work to its natural capability. This reduces inspection friction, avoids unnecessary scrap, and doesn’t add cost to dimensions that don’t need it.
| Process | Typical Tolerance | Notes |
|---|---|---|
| Laser cutting (feature position/size) | ±0.005" (±0.13 mm) | Repeatability excellent run-to-run; large parts accumulate slightly more across full sheet |
| Laser cutting (hole diameter) | ±0.005" | Kerf offset applied in CNC program; call out critical clearance holes explicitly |
| Press brake bend angle | ±1° (air bending) | Coining/bottoming achieves ±0.5° with higher tonnage; stainless/aluminum spring back more |
| Press brake formed dimension | ±0.010" per bend | Accumulates with each bend; design blanket tolerance for multi-bend parts |
| Welded assembly (overall) | ±1/16" to ±1/8" | Jig welding tightens distortion; varies by size, material, and heat input |
| Waterjet cutting | ±0.005" to ±0.010" | No heat distortion; consistent at all thicknesses; speed affects edge taper |
| CNC milling (vertical mill) | ±0.001" to ±0.005" | Tightest available; used for critical features after fabrication |
How to Specify Tolerances Correctly in Your RFQ
Use a blanket tolerance on your drawing title block, such as plus or minus 0.010 inch for all linear dimensions unless otherwise noted, and add explicit tight tolerances only on features where fit-up genuinely requires them. Over-tolerancing every dimension makes quotes more expensive and forces shops into inspection and rework on dimensions that don’t affect how your assembly works.
The most common tolerance mistake in fabrication RFQs is copying a machining tolerance block (plus or minus 0.001 inch on all dimensions) onto a sheet metal drawing. That number is achievable in a machine shop on turned or milled features, but it’s not realistic for a press brake bend or a weld, and asking for it in those operations either adds inspection cost or results in a lot of technically out-of-tolerance parts that actually work fine.
A practical approach: identify the two or three features in your design that control assembly fit-up and call those out with the tight tolerance they actually need. Apply a general tolerance of plus or minus 0.010 to 0.030 inch to everything else, depending on how critical the overall envelope is. Then note explicitly: “All other dimensions plus or minus 0.020 inch.” This gives the fabricator a workable target and gives you a genuine check on the dimensions that matter. See our metal fabrication RFQ checklist for a full breakdown of what to include in a complete quote request.
When Tighter Tolerances Are Needed
When fabrication tolerances aren’t tight enough for a critical feature, two options are available: CNC milling after fabrication or switching the cutting step to waterjet. The vertical mill at Paragon can hold plus or minus 0.001 to 0.005 inch on machined features added after fabrication. Waterjet cutting holds plus or minus 0.005 to 0.010 inch on cut geometry in thicker material with no heat distortion.
CNC machining after fabrication is the most reliable way to achieve tight tolerances on specific features in a welded or formed part. The part is fabricated to normal tolerances, then fixtured on the vertical mill for the critical operations: a precision bore, a datum face, a close-tolerance slot. This is how complex assemblies with both fabricated and machined features are produced routinely in industrial work.
Our CNC vertical mill handles this in-house, so your part doesn’t leave the building for secondary machining. For thicker flat plate where laser cutting’s heat affects edge geometry, waterjet cutting delivers consistent tolerances through the full thickness without thermal effects.
If you’re working with a design that requires tighter tolerances than standard fabrication can achieve, send us your drawing. Our team will identify which features drive the tight requirement, recommend the right process for each, and give you an honest assessment of what the part will cost versus what you’d get from relaxing a non-critical tolerance.
- Laser cut features: ±0.005" positional, ±0.005" hole diameter in production
- Press brake angle: ±1° air bending; ±0.5° coining or bottoming
- Press brake formed dimension: ±0.010" per bend, accumulates
- Welded assembly: ±1/16" to ±1/8" overall; tighter with jig welding
- Blanket general tolerance: ±0.010" to ±0.030" recommended for most sheet metal
- CNC milling: ±0.001" to ±0.005" on machined features
Need Accurate Parts?
Send us your drawings. Our team reviews tolerance callouts before quoting, so you know what’s achievable before a single piece of metal is cut. Paragon has 40+ years of fabrication experience in Northern Kentucky and Greater Cincinnati.
Frequently Asked Questions
What is the standard tolerance for laser cut parts?
Fiber laser cutting in production holds plus or minus 0.005 inch on cut feature positions and hole diameters. Kerf width runs approximately 0.010 to 0.015 inch, and the CNC program applies a kerf offset so finished dimensions match the drawing. Repeatability part-to-part is excellent; variation comes primarily from material flatness and thermal effects on large sheets.
How accurate is press brake bending?
Standard air bending holds plus or minus 1 degree on bend angle and plus or minus 0.010 inch on formed linear dimensions per bend. Coining and bottoming methods can tighten angle tolerance to plus or minus 0.5 degree with higher tonnage. Tolerances accumulate with each bend, so a multi-bend part should be designed with a blanket tolerance that accounts for the full stack-up.
Why does specifying tight tolerances on every feature increase cost?
Tight tolerances require slower machine speeds, additional inspection steps, potential rework, and sometimes secondary machining operations that wouldn’t otherwise be needed. Applying a tight tolerance to a feature that doesn’t control assembly fit-up adds cost without adding function. The right approach is a relaxed blanket tolerance with explicit callouts on the two or three features that actually drive assembly performance.
Can I get tighter tolerances than standard for a critical feature?
Yes. For cut features, tighter tolerances are achievable by slowing machine speed and adding inspection. For features requiring plus or minus 0.001 to 0.005 inch, CNC milling after fabrication is the standard solution. For cut geometry in thick plate where heat distortion is a factor, waterjet cutting delivers consistent tolerances without thermal effects. Discuss critical features with our team before quoting.
or call 1-800-467-0121