Single Bend Flat Pattern Configurator
Enter the finished flanges, say which datum you measured them to, and get the flat blank: flat length, bend line position and a clean DXF. The formed section and the flat pattern both update as you type, so you can see the part you asked for before you cut it.
The method behind it: How to work out the flat length of a bent part — step by step, with sources.
Dimensions
Results
Enter valid dimensions to see results.
Preview
Formed section
- Material
- Bend centre
- Selected datum
True to the entered thickness, inside radius and through angle. The dashed grey construction runs out to the sharp corner your flange lengths are measured to, so the datum is visible rather than just named.
Flat pattern
- Cut
- Bend line
- Bend region
Only the cut outline and the bend line are exported. The two dashed lines mark the tangent points where the bend region starts and ends, for reference.
No part width entered, so the long edges of this strip are indicative only — they are drawn as construction, not as a cut edge.
How this tool is verified
- Geometry checked against hand-derived golden cases and geometric invariants — developed arc equals true circumference, metric and imperial inputs give identical millimetre geometry.
- Every exported DXF is read back and audited by ezdxf, an independent DXF library that had no part in writing it (ezdxf 1.4.4).
- Output is deterministic: the same inputs produce the same file, byte for byte, with a version tag in the header.
The method, the reports and the responsibility boundary are on the Verification page.
Built by Ruthen Systems
Free, with no account, and the dimensions you type never leave your browser. If a result looks wrong, or the option your shop needs is missing, say so — reports of a wrong result are dealt with first.
Report a problem or request a toolAssumptions and limits
Read these before you cut anything. They describe exactly what this tool does and does not account for.
- One bend, two flanges. Multi-bend parts are not modelled: bends interact once flanges are short relative to thickness.
- The bend angle is the angle bent through — 90° is a square corner, not the included angle between the flanges.
- Flange lengths are measured to the theoretical outside sharp corner — where the two outside faces would meet if extended. This is the apex, not a point on the formed part.
- Geometry is deterministic from the values entered. Nothing is inferred from a material.
- K-factor is yours. Real production values depend on material, temper, grain direction, tooling and forming method.
- Springback is not predicted. Bend to your own shop allowance.
- This does not replace a validated shop bend table — use it to plan, then confirm against a test bend.
Output is a planning and fabrication aid. You are responsible for verifying dimensions, tolerances and material behaviour before production — full disclaimer.
Worked example
A 2 in and a 3 in flange, both measured to the outside apex, in 0.125 in material with a 0.250 in inside radius, bent through 90° at K = 0.33.
- Outside setback0.3750 in
- Straight legs1.6250 / 2.6250 in
- Bend allowance0.4575 in
- Bend deduction0.2925 in
- Flat length4.7075 in
Both routes agree, which is the useful check: adding the legs to the allowance gives 1.625 + 2.625 + 0.4575, and subtracting the deduction from the outside dimensions gives 2 + 3 − 0.2925. Both are 4.7075 in.
Method
A bend is developed on its neutral axis, which sits inside the material at a fraction K of the thickness measured from the inside face. Everything else follows from that one idea.
The four quantities
With inside radius R, thickness T, K-factor K and θ the angle bent through:
- Neutral-axis radius Rn = R + K·T
- Bend allowance BA = θrad · Rn — the arc length of material consumed by the bend
- Outside setback OSSB = (R + T) · tan(θ/2) — tangent point to the outside sharp corner
- Bend deduction BD = 2·OSSB − BA
One algorithm, three datums
The flat length is always the two straight legs plus the bend allowance. What changes between conventions is not the arithmetic but which number you typed, so the datum is removed at the input rather than carried through the maths:
- tangent basis — the entered length already is the straight leg
- inside basis — subtract R · tan(θ/2)
- outside basis — subtract (R + T) · tan(θ/2)
The familiar outside-dimension shortcut, flat = A + B − BD, is the same identity rearranged rather than a competing method: substituting A = leg + OSSB into it returns leg A + leg B + BA exactly. The test suite asserts the three routes agree across a grid of thicknesses, radii, angles and K-factors rather than taking the algebra on trust.
Why the datum matters more than K
Take a 0.060 in part with a 0.060 in inside radius bent through 90° with 2 in flanges. Sweeping K across its typical range, 0.33 to 0.50, moves the blank by about 0.41% (with the flanges to the outside). Measuring the flanges to the wrong datum moves it by 6.18% — about fifteen times further, and with nothing on screen to warn you. That is why the basis control sits above the flange fields and why the section diagram draws the datum you picked.
What the bend line is
The exported BEND line is the developed mid-arc: straight leg A plus half the bend allowance, measured from edge A. Formed, that material point lands in the middle of the bend, which for a symmetric bend is the press-brake centreline. It is deliberately not the middle of the blank, and it is not the tangent line — the preview draws the tangent lines separately so the bend region is visible. This is nominal geometry only: it does not model your machine's own back-gauge or tooling compensation.
Limits
Angles run from just above 0° to 180°. Above 90° the setback grows quickly, and at 180° the faces are parallel so no sharp corner exists at all — at that angle the flanges must be given to the tangent. A flange shorter than its own setback is rejected rather than quietly returned as a negative leg, because it means the datum or the angle is wrong.
Questions
Where exactly do I measure flange A and B to?
Wherever you tell it. That is the point of the dimension basis control, and it is the single most important input on this page. "Outside apex" means the theoretical sharp corner where the two outside faces would meet if extended — the datum most drawings use. "Inside apex" is the same idea on the inside faces. "Tangent" means the straight material only, measured to where the bend starts. Pick the wrong one and the blank is wrong by roughly twice the setback, which for a 90° bend is about twice the sum of radius and thickness.
Is 90° the bend angle or the included angle?
This tool takes the angle bent through: 0° is flat stock, 90° is a square corner, 180° folds the flanges back onto each other. The included angle between the flanges is 180° minus that. The two happen to be identical at exactly 90°, which is why the ambiguity survives in so many places — at 135° the two readings differ by about 18 mm on this page’s default part (3 mm sheet, R 3, K 0.33, two 50 mm flanges to the outside). The formed section updates as you type, so you can see which shape you asked for.
Why does the bend line sit where it does?
It is the developed mid-arc: the material point that ends up in the middle of the bend once formed, at straight leg A plus half the bend allowance from edge A. It is not the middle of the blank — those only coincide when the two flanges are equal — and it is not the tangent line where the bend starts. The bend region between the two tangent lines is drawn on the preview so you can see the difference.
What K-factor should I use?
One from your own shop, ideally measured from a test bend in the material and tooling you will actually run. The two presets are commonly cited starting values for air bending and bottoming; they are not measurements taken by us and they are not properties of any material. K locates the neutral axis as a fraction of thickness from the inside face, so it cannot exceed 0.5.
Why is there no material or gauge dropdown?
Because we have no press, no tooling data and no test coupons, so any K-factor attached to a material name here would be invented. Gauge is left out for a related reason: the same gauge number means different thicknesses in steel, galvanised and aluminium series, and a dropdown that quietly picks one is a good way to cut the wrong blank. Enter the thickness you are actually running.
Why do I need a part width for the DXF?
A DXF is a blank, and a blank has two dimensions. Every number on this page — flat length, bend line, allowance, deduction — is computed without a width, so the calculation works whether or not you supply one. But rather than invent a width so the button can be enabled, the export stays off until you give a real one.
Does this account for springback?
No. Everything here is nominal geometry derived from the values you entered. Springback depends on material, temper, tooling and forming method, and predicting it is not something this tool attempts. Add your own overbend allowance.
What is in the DXF?
The blank perimeter on the CUT layer and one bend line on the BEND layer. Nothing else — no dimensions, no text, no annotation, no construction lines. The unit is recorded in the $INSUNITS header variable (4 for millimetres, 1 for inches). The tangent lines and labels you see in the preview are display only and are deliberately not exported.
Missing an option?
A different datum, an offset, a shop allowance, another shape altogether — say what this tool does not cover yet. Requests decide what gets built next, and a report of a wrong result is dealt with before anything new.
Rather have the whole part drawn — a shop drawing or a cut file from your sketch? That is paid drafting, quoted per job: drafting for small shops.
Related tools
Cone / Frustum Configurator
Flat pattern with inside/outside dimension basis, plate-roll or press-brake forming, bend angles and out-of-round — plus a clean DXF.
Open the tool →Hopper & Transition Builder
Develop a rectangular hopper or duct transition into four flat panels — centred or offset — with exact developed geometry and a DXF per panel.
Open the tool →Pipe Cut Template Builder
Wrap-around templates for angled pipe ends and pipe-to-pipe saddles, with the export deviation stated rather than assumed.
Open the tool →Segmented (Lobster-Back) Elbow Calculator
Mitred elbows from straight pipe or rolled sheet: cut angle, heel and throat lengths, a cut list for one pipe, and 1:1 templates plus DXF for each piece.
Open the tool →Square / Rectangle to Round Transition
One exact flat pattern for a square-to-round or rectangle-to-round, centred or offset — with true lengths, corner bend lines and a DXF.
Open the tool →Eccentric (Offset) Reducer Flat Pattern
Flat on one side or any offset: one exact flat pattern for an eccentric reducer or oblique cone, a true-length table for hand layout, and a DXF.
Open the tool →Sheet Metal Profile Builder
Build a multi-bend open profile from segments and bends. Live formed section, live flat pattern, and a DXF blank with a directed centreline per bend.
Open the tool →Rolled Cylinder Blank Calculator
Blank length for a rolled cylinder or shell course from the inside, outside or mean diameter and the plate thickness, with a seam gap and a DXF.
Open the tool →Box and Tray Blank Calculator
The flat blank for a sheet metal tray or open box: blank size from the outside dimensions and bend deductions, bend lines, corner notches and a DXF.
Open the tool →Sphere and Dome in Zones
Flat patterns for a sphere or dome built from zones: each band developed as a cone frustum on the chords, a flat crown disc, every pattern radius and angle, and a DXF.
Open the tool →Pipe Offset Calculator (Simple and Rolling)
Travel, run and cut length for simple and rolling pipe offsets at any fitting angle, with the constants and cut-length rule from the US Army pipe-fitting manual.
Open the tool →Metal Weight Calculator (Plate, Tube, Bar)
Weight of plate and sheet, discs and rings, tube and pipe, and round bar — per piece and per quantity — with every density traced to a US government document.
Open the tool →Sheet Metal Gauge Chart and Converter
What a gauge number means in inches and millimetres for steel and aluminium, what a galvanized gauge weighs, both ways — every value traced to a US government source.
Open the tool →Cone in Segments (Multi-Piece Cone)
A cone too big for one plate, split into identical segments: give a count or your plate size, get one segment’s size, angle and chords, and a DXF.
Open the tool →Press Brake Tonnage Calculator
An estimate of the force for a 90° air bend from thickness, die opening, bend length and material: kN, metric and US tons, whole bend and per length, with how far to trust it.
Open the tool →K-Factor Calculator (from a Test Bend)
Bend a strip, measure it, and get your own K-factor — with the bend allowance and deduction it implies, and how far a measuring error would move it.
Open the tool →Bend Deduction & Allowance Chart
Your own bend deduction, allowance or setback chart for one thickness and K: any radii, any angles, mm or inch, with a CSV download.
Open the tool →Flange / Bolt Circle DXF Generator
Lay out a bolt circle from OD, ID, PCD, hole size and count. Get exact hole coordinates and a DXF with centrelines.
Open the tool →Saved. Need a part drawn from your sketch or photo? A simple flat pattern or DXF of one part is typically C$40–80, with a free quote: drafting for small shops.