Calculation method
For bend angle A in radians, inside radius R, material thickness T, and K-factor K, bend allowance is BA = A(R + KT). Outside setback is OSSB = (R + T) tan(A/2), and bend deduction is BD = 2OSSB − BA. Because this tool accepts outside mold-line face dimensions, the flat length is their sum minus every bend deduction.
A bend centerline is placed after the preceding faces and deductions, at the bend's first tangent plus half its allowance. The tool refuses face dimensions where adjacent setback regions overlap, because that simple virtual-sharp model cannot describe the requested profile.
Using the SVG and DXF
The SVG declares physical millimeter or inch dimensions and contains a rectangular cut outline plus directional bend classes. The ASCII R12 DXF uses drawing units matching the selected input and separates entities onto CUT, BEND_UP, and BEND_DOWN layers. Open and measure the file in the destination CAD/CAM system before use; layer names do not automatically assign tooling or forming operations.
Choosing a K-factor
K-factor locates the neutral axis as a fraction of stock thickness from the inside surface. It changes with material condition, thickness, grain direction, formed radius, punch and die, bend method, and machine setup. A generic value is only a planning input. For production, bend a representative coupon, measure the actual result, and use an approved bend table or calibrated value for that exact process.
Manufacturing boundary
This is a one-dimensional calculation and drawing aid, not a production-ready CAD model. It creates a rectangular blank without holes, corner treatments, bend reliefs, notches, hems, seams, collision analysis, minimum-flange checks from tooling, springback compensation, tonnage calculations, or bend sequencing. DXF export does not certify manufacturability or machine safety. Preserve the engineering drawing, compare against approved CAD and shop bend data, and test a coupon before cutting valuable stock.
Frequently asked questions
What angle should I enter?
Enter the angle through which the sheet turns: a conventional right-angle flange is a 90° bend. Do not enter the remaining included angle unless you first convert it to the turn angle.
Why is bend direction absent from the length formula?
Up versus down changes the formed profile and shop instructions, but not the neutral-axis arc length for the same thickness, radius, angle, and K-factor. Direction is retained in the drawing layers.
Why was a short middle face rejected?
Its two adjacent outside setbacks overlap. The independent virtual-sharp bend-deduction model no longer produces separate tangent regions, so this calculator deliberately stops rather than emit crossed or reversed bend lines.
Can I send the DXF directly to a laser?
No. First verify units, scale, layer interpretation, material, bend lines, reliefs, tolerances, and the final profile in your supported CAD/CAM and manufacturing workflow.
Technical references
Autodesk's sheet-metal unfold-rule equations describe the relationship among bend allowance, bend deduction, and K-factor. SOLIDWORKS flat-pattern export guidance documents exporting bend lines and mapping bend directions to DXF/DWG layers.