Use this Minimum Bend Radius Calculator to estimate a practical starting inside radius for a sheet metal bend. Select the material and sheet thickness, identify the bend line relative to the rolling grain, and optionally enter a proposed drawing radius. The tool returns a recommended starting radius or range, the corresponding radius-to-thickness ratio, a conservative planning value, and a comparison of your proposed radius.
Thickness multiplied by the lower factor in the selected material tier.
When the chart gives a bounded range, the upper value is shown for conservative planning.
Factors reproduce ShincoFab's published DFM starting guidance. Open-ended bands remain open-ended.
Minimum bend radius is not a guaranteed machine capability. Grade, temper, heat treatment, rolling direction, edge quality, punch and die geometry, bend method, angle and surface requirements can change the production limit.
Select MM or IN in the unit control. Switching units converts the existing sheet thickness, proposed inside radius, and calculated results; it does not merely relabel them. The material factors remain dimensionless.
Choose the exact available option that matches the drawing: mild or cold-rolled steel, stainless steel 304, aluminum 5052-H32, or aluminum 6061-T6. Grade and temper matter. In particular, 5052-H32 and 6061-T6 must not be treated as interchangeable just because both are aluminum.
If the actual alloy, temper, heat treatment, or material condition is not represented, do not substitute the closest-looking material and treat the result as final. Use the Minimum Bend Radius Chart as a starting reference and request a material-specific review.
Enter the nominal sheet thickness in the active unit system. The calculator supports 1.00 to 12.00 mm, equivalent to approximately 0.039 to 0.472 in. Values below, above, blank, nonnumeric, zero, or negative produce a validation message instead of a misleading result.
The lookup uses a thinner-sheet tier below 6.00 mm and a heavier-sheet tier from 6.00 through 12.00 mm. This boundary convention removes ambiguity where published chart ranges meet.
The Proposed inside radius field is optional. Enter the radius shown on the drawing or planned in CAD to compare it with the selected guideline. Leave the field blank if you only need the recommendation.
The comparison reports whether the proposed radius is below, within, or at or above the starting band. For an open-ended recommendation such as 4.00 x T or more, the check only confirms whether the proposal reaches the published lower limit.
Choose whether the bend line is perpendicular/across grain, parallel/along grain, or unknown. A bend line perpendicular to the rolling direction is the preferred orientation for a tight bend because the outside surface is generally less prone to cracking.
The published table does not provide one universal numeric grain-direction adjustment, so the calculator does not silently add one. Parallel or unknown orientation produces a review warning instead. Confirm the required increase with the material supplier and fabricator.
Results update live whenever an input changes. Use Copy results to copy the material, dimensions, guideline factors, radius results, proposed-radius status, and orientation review. Copy radius copies only the primary recommendation. Reset values restores a documented stainless steel example without changing the selected unit system.
This is the primary result. It is the preliminary inside radius obtained by multiplying sheet thickness by the published factor or factor range for the selected material and thickness tier.
For example, 2.00 mm stainless steel 304 uses a 1.50-2.00 x T starting band:
Lower radius = 2.00 mm x 1.50 = 3.00 mm
Upper radius = 2.00 mm x 2.00 = 4.00 mm
Recommended starting inside radius = 3.00-4.00 mm
The guideline factor is the radius-to-thickness ratio, commonly written as R/T or F x T. It has no unit. A result of 1.50-2.00 x T means the starting inside radius is between 1.5 and 2 times sheet thickness.
For a bounded range, this value uses the upper factor. It is useful when early CAD work needs one provisional radius rather than a band. For an open-ended recommendation, the calculator displays the lower threshold with a greater-than-or-equal sign and requires a production-specific review.
The word “conservative” applies only within this lookup method. It does not guarantee freedom from cracking, springback, marks, or tooling conflicts.
This status compares the optional drawing radius with the calculated starting band:
This result describes the grain-direction risk flag. Preferred direction corresponds to a bend line perpendicular to the rolling direction. Increase radius / review appears for a bend line parallel to the grain, while Confirm grain direction appears when orientation is unknown.
The calculator implements the starting factors published in ShincoFab’s Minimum Bend Radius Chart. The values are practical DFM screening guidance, not values taken from a universal material standard and not guaranteed machine capabilities.
| Material and condition | 1.00 to less than 6.00 mm | 6.00 to 12.00 mm |
|---|---|---|
| Mild steel / cold-rolled steel | 1.00 x T | 1.00-1.50 x T |
| Stainless steel 304 | 1.50-2.00 x T | 2.00-3.00 x T |
| Aluminum 5052-H32 | 1.00 x T | 1.50 x T or more |
| Aluminum 6061-T6 | 3.00-4.00 x T | 4.00 x T or more |
The calculation is direct:
R_low = T x F_low
R_high = T x F_high, when the published range has an upper factor
Where:
R_low is the lower starting inside radius.R_high is the upper planning inside radius for a bounded range.T is nominal sheet thickness.F_low and F_high are the material- and thickness-specific factors.All calculations are performed internally in millimeters. Inch inputs are converted to millimeters before the lookup and converted back only for display, which keeps the metric and imperial results consistent.
This calculator does not use bend angle, K-factor, bend allowance, V-die opening, punch radius, or press-brake tonnage to redefine the material guideline. Those variables still affect the manufactured bend and flat pattern. After selecting a radius, use the Sheet Metal Bend Allowance and Bend Deduction Chart and a fabricator-approved bend table for developed-length work.
For a broader release review, work through the Sheet Metal DFM Checklist and the Complete Guide to Sheet Metal Bending.
Nominally similar sheet can have different yield strength, elongation, hardness, heat treatment, and surface condition. Aluminum 6061-T6, annealed aluminum, and 5052-H32 have substantially different forming behavior. A generic material-family label cannot capture those differences.
The outer surface of the bend carries tensile strain. A bend parallel to the rolling direction can crack earlier than a bend perpendicular to it. Burrs, laser-cut edge condition, sheared edges, scratches, and small notches can also become crack initiators.
In air bending, the achieved radius depends on the V-die opening, punch geometry, material behavior, angle, and press-brake setup. Bottoming or coining changes the relationship between tooling and the finished radius. The radius modeled in CAD may not match a shop’s standard tooling without a deliberate process choice.
The lookup factors do not calculate springback. Stainless steel and heat-treated aluminum may require overbending or process-specific compensation. The final unloaded angle and radius should be validated against the selected tooling and material lot.
CAD defaults often use generic K-factors and radii. A supplier’s proven bend table may use different values based on its equipment, dies, material sources, and inspection method. For production flat patterns, the supplier’s validated data should take precedence over a general web calculator.
These answers address common decisions that arise when a calculator result differs from CAD, a supplier chart, or an existing part. Use them to identify the input convention and determine when a test bend or drawing-specific DFM review is necessary.
It is the smallest inside radius that a material and process can form without unacceptable cracking, thinning, distortion, or surface damage. There is no single universal value because alloy, temper, thickness, grain direction, edge quality, tooling, bend method, and acceptance criteria all matter.
This calculator uses the inside bend radius. If a drawing gives an outside radius, do not enter it directly. For an idealized constant-thickness section, the outside radius is approximately the inside radius plus sheet thickness, but real forming and measurement practices should be confirmed with the fabricator.
6061-T6 is heat treated for higher strength and is generally less forgiving in tight sheet bends. 5052-H32 is commonly selected for formed sheet parts because it has better bendability. The calculator therefore applies different published starting factors rather than grouping both under a generic aluminum option.
It changes the production risk, but this tool does not apply a fixed numeric multiplier because the published guidance does not define one universal adjustment. A bend line parallel to the rolling direction receives an increase-radius warning. Confirm the required radius with the material supplier and fabricator.
The source chart presents ranges that meet at 6 mm. To make the calculator deterministic, exactly 6.00 mm enters the heavier-sheet tier. This also avoids understating the starting radius at the boundary. The convention is shown in the interface and should still be checked against the intended process.
Not automatically. The output is a recommended finished inside bend radius for preliminary design. Punch nose radius, V-die opening, air bending, bottoming, coining, springback, and material response all affect the relationship between the tool and the finished part.
No. A larger radius generally reduces outer-fiber strain, but it does not verify flange length, tooling clearance, hole-to-bend distance, springback, cosmetic quality, flat-pattern accuracy, or press capacity. It is one input to a complete DFM review.
Do not select a different alloy only to obtain a number. Provide the material specification, temper or condition, thickness, bend angle, grain direction, desired radius, and applicable quality requirements to the fabricator. Material supplier bend data or a representative test bend is more reliable than an unsupported substitution.
A generic calculator cannot see your flange lengths, cutouts, bend sequence, cosmetic faces, tolerance stack, tooling constraints, or exact material certificate. ShincoFab’s sheet metal bending service can review the radius together with the full part geometry and manufacturing plan.
Request a DFM review or fabrication quote with the CAD model and drawing, material grade and temper, sheet thickness, bend angles, inside radii, grain-direction requirements, quantities, tolerances, and surface-finish expectations.
ShincoFab specializes in precision sheet metal fabrication, delivering high-quality custom metal solutions to clients worldwide with advanced technology and expert craftsmanship.
Ready to start your sheet metal project? Contact the ShincoFab team to discuss your custom fabrication requirements. We support you through design, manufacturing, and delivery—at every stage.