Skip to content
TaskNinja

HomeBlog

Sheet metal flat pattern length: K-factor, bend allowance and bend deduction, worked on a real bracket

Work out a sheet metal flat pattern by hand with the K-factor, bend allowance and bend deduction, then check it in free browser CAD and export the DXF.

By the TaskNinja team · · 7 min read

A laser shop cuts your bracket from a flat blank and a press brake folds it. If the blank is half a millimetre too long, a box with four bends can be two millimetres out. The blank size is the flat pattern length, and it hangs on one small ratio called the K-factor.

This guide works one L bracket through: the formulas by hand, the same part in Trevolyx (our free browser CAD), and the DXF for the shop. Every flat length below was reported by the live app on 10 Nov 2026, and each matches the hand calculation.

The bracket

ItemValue
Material thickness T2 mm
Inside bend radius R2 mm
Bend angle A90°
K-factor K0.44
Base leg (outside)50 mm
Flange leg (outside)30 mm
Width100 mm
The example part. Both leg lengths are outside dimensions, measured to the virtual sharp (where the outer faces would meet if the bend had no radius).

Three terms you need

When sheet bends, the inside face is squashed and the outside face stretches. Somewhere between them is a layer that keeps its length, the neutral axis. The K-factor says where it sits: K = t / T, where t is the distance from the inside face to the neutral axis. K = 0.5 means the middle of the sheet, smaller values mean closer to the inside face.

  • Bend allowance (BA) is the length of the neutral axis through the bend. SOLIDWORKS Help gives it as BA = π x (R + K x T) x A / 180, with A in degrees.
  • Outside setback (OSSB) is how far the bend pulls back from the virtual sharp: OSSB = (R + T) x tan(A / 2). At 90° that is simply R + T.
  • Bend deduction (BD) is what you subtract from the two outside legs: BD = 2 x OSSB - BA.

So the flat length is the outside legs minus one bend deduction per bend.

Working it by hand

  1. BA = π x (2 + 0.44 x 2) x 90 / 180 = 1.5708 x 2.88 = 4.524 mm.
  2. OSSB = (2 + 2) x tan 45° = 4 mm.
  3. BD = 2 x 4 - 4.524 = 3.476 mm.
  4. Flat length = 50 + 30 - 3.476 = 76.524 mm. Check it the other way: straight base 50 - 4 = 46, straight flange 30 - 4 = 26, and 46 + 4.524 + 26 = 76.524.

The bend line a fabricator marks on the blank sits in the middle of the bend zone, at 46 + 4.524 / 2 = 48.262 mm from the base edge.

The same bracket in Trevolyx

  1. Open Trevolyx in desktop Chrome or Edge and start a Part. Sketch a 100 by 50 mm rectangle on the Front Plane.
  2. Open the Sheet Metal tab and click Base Flange/Tab. Leave Gauge table on Custom, set Thickness T1 to 2 and Bend radius R1 to 2. In Bend Allowance, keep the type on K-Factor and type 0.44. The panel works out the allowance for a 90° bend as you type: 4.524 mm, the same as step 1 above.
  3. Click OK. The tree gains a Sheet-Metal folder with a cut list, Base-Flange1 and Flat-Pattern1.
  4. Click Edge Flange, then click the top edge of the plate. Set Length to 30, leave Measured to on Outer Virtual Sharp and Position on Material Inside. The foot of the panel reads Flat pattern size: 100.00 x 76.52 mm before you even press OK.
Trevolyx Base Flange panel with thickness 2 mm, bend radius 2 mm, K-Factor 0.44 and the hint showing 4.524 mm bend allowance for a 90 degree bend
Base Flange with T 2, R 2 and K 0.44. The hint under the K box shows the 90° bend allowance, 4.524 mm.
Edge Flange panel with Length 30 mm measured to Outer Virtual Sharp and Material Inside, and the flat pattern size of 100.00 by 76.52 mm
Edge Flange, 30 mm to the outer virtual sharp. Flat pattern size: 100.00 x 76.52 mm, matching the hand result.

How much does the K-factor matter?

We rebuilt the same bracket with three K-factors. Only the bend allowance changes, so the difference per bend is small, but it adds up on a part with four or six bends.

K-factorBend allowanceBend deductionFlat length
0.334.178 mm3.822 mm76.178 mm
0.444.524 mm3.476 mm76.524 mm
0.504.712 mm3.288 mm76.712 mm
Same bracket, T 2, R 2, 90°, legs 50 and 30 to the outer virtual sharp. Flat lengths as reported by Trevolyx on 10 Nov 2026.

Going from 0.33 to 0.5 moves this one bend by 0.53 mm. Trevolyx starts new parts at K = 0.5, and a SOLIDWORKS blog post on bend allowance options suggests 0.5 when you have no shop data. The best number is still the one your fabricator measures on their own brake, die and material.

The trap: what the flange length is measured to

A flat pattern is more often wrong because the flange length was typed against a different reference than the drawing uses. We kept K at 0.44 and the length at 30 mm, and changed one setting at a time.

SettingWhat 30 mm meansFlat length
Measured to: Outer Virtual Sharp30 to the outside corner76.52 mm
Measured to: Inner Virtual Sharp30 to the inside corner78.52 mm
Measured to: Tangent Bend30 of straight flange after the bend80.52 mm
Position: Material OutsideFlange sits outside the 50 mm edge78.52 mm
Position: Bend OutsideWhole bend sits outside the 50 mm edge80.52 mm
One setting changed per row, everything else as in the bracket above. Trevolyx flat lengths, 10 Nov 2026.

That is up to 4 mm from one drop-down. Each row is right for what it describes, so match the setting to your drawing. Most shop drawings give outside dimensions: Outer Virtual Sharp with Material Inside.

Flatten, then export the DXF

  1. Click Flatten in the Sheet Metal tab to see the blank with its bend line. Click it again to fold the part back.
  2. Click Export Flat Pattern DXF. The file is 1:1 in millimetres with layers for the OUTLINE, the dashed BEND lines, BEND_NOTES such as "UP 90° R 2", and a NOTES block with the cut list: thickness, radius, K-factor, bounding box, blank area and cutting length.
  3. Open the DXF in the TaskNinja DXF viewer to check it before you send it. Ours showed the 100 x 76.52 outline with the bend line at 48.26 mm, the same as the hand calculation.

We also added two dimples with Forming Tool (Dimple, Louver or Lance). They arrive on their own FORM layer with a note such as "DIMPLE D 12 H 2 UP", and the outline did not change.

The exported flat pattern DXF open in the TaskNinja DXF viewer: rectangular outline, dashed bend line labelled UP 90 degrees R 2, and two dimples labelled DIMPLE D 12 H 2 UP
The flat pattern DXF in the TaskNinja DXF viewer: outline, dashed bend line with its note, and two dimples on the form layer.

Finding your own K-factor from one test bend

  1. Cut a strip of the real material to a known length L, say 100 mm, and measure the thickness T.
  2. Bend it to 90° on the same punch and die you will use for the job.
  3. Measure both outside legs X and Y and the inside radius R.
  4. BD = X + Y - L. For a 90° bend, BA = 2 x (R + T) - BD.
  5. K = (BA / 1.5708 - R) / T.

Example numbers: a 100 mm strip of 2 mm sheet with a 2 mm inside radius that measures 51.75 mm on each leg gives BD = 3.5, BA = 8 - 3.5 = 4.5 and K = (4.5 / 1.5708 - 2) / 2 = 0.43. If your shop gives a bend allowance or bend deduction value instead, the Bend Allowance Type list takes those directly.

Honest limits

Trevolyx is desktop first (Chrome or Edge on a laptop). It does not open native SOLIDWORKS or Inventor files, and an imported STEP solid has no sheet metal history, so rebuild it with sheet metal features to flatten it. Excel bend tables are not supported yet. Your files stay in your browser tab.

FAQ

What is a good K-factor for mild steel?

It depends on the radius, die and material. 0.5 is the usual CAD starting point; one test bend gives your shop's real number.

What is the difference between bend allowance and bend deduction?

Bend allowance is the length added for the bend between the two straight parts. Bend deduction is the amount taken off the sum of the outside legs. They describe the same blank from two directions: BD = 2 x OSSB - BA.

Why is my flat pattern 2 mm longer than I expected?

Check what the flange length is measured to. In our test, the same 30 mm typed against the inner virtual sharp instead of the outer one made the blank exactly 2 mm longer.

Can I get the flat pattern DXF free?

Yes. Export Flat Pattern DXF in Trevolyx is free, with no account and no watermark. See the sheet metal flat pattern to DXF page for the full feature list.

Sources

Written by the TaskNinja team with help from an AI writing tool, then checked against the live Trevolyx app, the hand formulas and the SOLIDWORKS documentation.