Skip to content
SOLID WORKS ClubSOLID WORKS Club

Sheet metal · Lesson 10

K-factor, bend tables and gauge tables

A flat pattern is only as accurate as its bend calculation. SOLIDWORKS can work from a K-factor (the default method), a bend allowance, a bend deduction, a bend table, an Excel bend calculation or a gauge table that sets thickness, radius and K-factor together. The values belong to your fabricator's press brake, so ask them — or measure a test bend.

Kevin Walsh Kevin Walsh Updated Checked for SOLIDWORKS 2026
Sheet metal bend cross-section with the neutral axis and a gauge table spreadsheet

Where to find it

Sheet-Metal feature (right-click → Edit Feature) → Bend Allowance; Use gauge table

The six bend calculations

Method What you enter
K-Factor (default) Neutral axis position: BA = A × (R + K·T)
Bend Allowance Arc length on the neutral axis, added to legs to the tangent lines
Bend Deduction Amount subtracted from legs to the virtual sharp: BD = 2·OSSB − BA
Bend Table Excel table of BA, BD or K by thickness, radius and angle
Bend Calculation Excel sheet with equations by angle range
Gauge Table Thickness, available radii and K or BA per gauge

The formulas and a worked example are on the K-factor calculator page. A rough check for 90° bends: the flat is about two thicknesses shorter than the outside legs per bend.

Gauge table tips

  • Set the K-factor and units at the top; leave the header row alone.
  • Separate several radii with a semicolon and a space.
  • List gauges from thinnest to thickest.
  • With a gauge chosen, Thickness is greyed out until you tick Override thickness.

Since 2023 the gauge can also appear in the cut list.

Step by step

  1. 1

    Open the sheet metal parameters

    In the bracket, right-click Sheet-Metal at the top of the tree → Edit Feature. The part's default thickness, bend radius, bend allowance and relief live here.

    Sheet-Metal feature PropertyManager with thickness, bend radius and Bend Allowance set to K-Factor 0.5
    The part's default thickness, radius and K-factor live in the Sheet-Metal feature.
  2. 2

    Change the K-factor

    Under Bend Allowance, keep K-Factor and change the value from 0.5 to 0.33. Click the tick.

  3. 3

    Compare the flat

    Flatten and read the bounding box in the cut list. A smaller K puts the neutral axis closer to the inside, so the blank gets shorter.

  4. 4

    Use a gauge table for real parts

    On the first Base Flange, tick Use gauge table and pick a table from the samples or your own. Choose the gauge and one of its bend radii — thickness and K-factor come from the table.

Common mistakes

  • Using a 90° bend deduction for other angles — on acute bends the flat comes out much too long.
  • Bend tables that set only the allowance while thickness and radius are still typed by hand. Gauge tables lock all three.
  • Copying K-factors from the internet. Your shop's tooling and material decide the value; update tables when tooling changes.

Lesson 10 of 13 in the sheet metal course.

Practice

Change the bracket's K-factor from 0.5 to 0.33. Check: the flat pattern bounding box changes from 100 × 86.71 to 100 × 86.18 mm. Confirm both values in the K-factor calculator.

Sources

Checked November 2026. SOLID WORKS Club is independent; menu names can differ slightly between releases.

Frequently asked questions

What is the default bend calculation in SOLIDWORKS?

+

K-Factor. GoEngineer calls it fairly conservative and suitable for most cases; the alternatives are bend table, bend allowance, bend deduction, bend calculation and gauge table.

What K-factor should I use in SOLIDWORKS?

+

Ask your fabricator. SOLIDWORKS' tech blog suggests 0.5 as a start if you have nothing else; K-factors usually lie between about 0.3 and 0.5.

Where are the sample bend and gauge tables?

+

In the install folder under lang\english\Sheet Metal Bend Tables and lang\english\Sheet Metal Gauge Tables. Check the path in Tools → Options → File Locations.

Gauge table or bend table?

+

A gauge table controls thickness, available radii and the bend value per gauge. A bend table controls only the allowance, deduction or K, so many resellers prefer gauge tables.