If your flat pattern dimensions are wrong, the K-factor is usually why. But “set the K-factor” is the third step in a process that starts with understanding what K-factor is, what bend deduction is (they are different things expressed in different units), and — critically — knowing which of three separate places in SOLIDWORKS is actually controlling your flat pattern.

K-Factor and Bend Deduction Are Not the Same Thing

Both K-factor and bend deduction describe what happens to material during bending, but they describe it differently.

Bend Allowance (BA) is the arc length along the neutral axis as the material wraps around the bend radius. It is the actual amount of material consumed by the bend zone. For a 90° bend:

BA = (π/2) × (R + K × T)

Where:

  • R = inside bend radius (mm)
  • T = material thickness (mm)
  • K = K-factor (dimensionless ratio, 0.0–0.5)

K-factor is the ratio that locates the neutral axis. K = 0 means the neutral axis is at the inner surface (no stretch). K = 0.5 means it is at the midpoint of the material. Physical values range from 0.25 for hard materials with sharp bends to 0.50 for soft aluminum with large radii. Most production steels fall between 0.33 and 0.42.

Bend Deduction (BD) is the amount you subtract from the sum of the two flat legs to get the total flat blank length. If a part has one 90° bend and the two legs measure 40mm and 60mm to the outside face of the bend:

Flat blank = 40 + 60 − BD

The relationship between BD and BA:

BD = 2 × (R + T) × tan(θ/2) − BA

For a 90° bend: BD = 2 × (R + T) − BA

These two formulations contain the same physical information and are mathematically equivalent. The reason both exist is practical: K-factor scales cleanly across different radii and gauges when you have a consistent material property (it is a ratio), while bend deduction is simpler for shops that have empirical tables of measured BD values for their specific tooling and do not want to work through the geometry every time.

SOLIDWORKS supports both. The choice of which to enter depends on how your shop characterizes its press brake tooling.

The Three Places SOLIDWORKS Reads K-Factor

This is where most confusion lives. SOLIDWORKS has three separate locations that can supply K-factor data, and they have a strict priority order:

Source 1: Material Library (Lowest Priority)

Every material in the SOLIDWORKS Materials dialog (right-click a part > Manage Materials, or Edit Material) has a Sheet Metal tab under the material properties. This tab includes:

  • Bend radius
  • Bend allowance type (K-factor, bend deduction, or bend table)
  • The K-factor or BD value for that material

This is the fallback — if nothing else overrides it, SOLIDWORKS uses the K-factor defined in the material library for the assigned material. The defaults are approximate values from general forming data and are almost never accurate for your specific tooling.

If you are using the default SolidWorks materials (1060 Alloy, AISI 1020, etc.) without modification, you are using generic K-factors that may or may not match your actual press brake. The first step in any precision sheet metal workflow is updating the material library with values derived from your actual test bends (covered below).

Source 2: Sheet Metal Feature (Middle Priority)

The Base Flange/Tab feature (the feature that creates a sheet metal part from a sketch) and the Insert Bends feature each have a K-factor or bend table field in their PropertyManagers. When you create or edit this feature, the value set here overrides the material library for all bends in the part.

This is the most common place to set K-factor. It takes precedence over the material, so even if the material database has the wrong value, the feature value controls the flat pattern.

The feature PropertyManager shows:

  • Bend Allowance type: K-Factor, Bend Allowance, Bend Deduction, or Bend Table
  • The value field (K-factor coefficient, or BD in the active unit, or the table filename)

One critical subtlety: if you created the sheet metal part and then changed the material, the feature K-factor remains unchanged. The material K-factor has no effect because the feature overrides it. Engineers sometimes change the material expecting the flat pattern to update, and it does not — because the feature is still supplying the old K-factor.

Source 3: Bend Table (.btl File) (Highest Priority)

A bend table is a text file (.btl extension) that maps combinations of material gauge and bend radius to specific bend allowance values. If a bend table is loaded into the document — either via the Sheet Metal feature PropertyManager or embedded in the document template — it silently overrides both the feature K-factor and the material K-factor for any bend radius and gauge combination that has a matching entry in the table.

This is the source of the most confusing behavior: you set K-factor to 0.38 in the Base Flange feature, the flat pattern comes out wrong, and debugging shows the model is using 0.33. A bend table, invisible in normal editing, is supplying the actual value.

To check whether a bend table is in effect: Edit the Sheet Metal feature (or Insert Bends feature) and look at the Bend Allowance dropdown. If it shows a filename rather than “K-Factor” or “Bend Deduction,” a table is loaded. The table filename also appears in the feature’s tooltip in the FeatureManager.

The override chain:

Bend Table (.btl) > Sheet Metal Feature > Material Library

The table wins when loaded. The feature wins over the material. The material is only consulted if neither of the other two provide a value.

How to Derive K-Factor Empirically From Your Tooling

Generic K-factors from textbooks or material databases describe average behavior. Production precision work — aerospace sheet metal, semiconductor enclosures, tight-tolerance brackets — requires K-factors derived from your actual press brake, your actual punch radius, and your actual material from your actual supplier.

The procedure:

Step 1: Cut test strips.

Cut strips of the actual material at the actual gauge you will use in production. Make them long enough to have two measurable legs after bending — 150mm total length is generally enough for moderate bend radii.

Step 2: Measure and record the flat length.

Measure the total flat strip length to 0.01mm precision before bending. Record this as Lflat. Weigh the strip if you want to correlate to material density as a secondary check.

Step 3: Bend at 90°.

Bend the strip to 90° with the actual tooling (punch radius and die width) you will use in production. The bend angle matters — use 90° because the math is simplest and 90° bends are the most common.

Step 4: Measure the bent legs.

After bending, measure:

  • L1 = length of first leg, measured from the outside surface of the bend tangent to the inside face of the leg
  • L2 = length of second leg, same measurement

Use a height gauge or calipers; do not guess from the inside face.

Step 5: Calculate K-factor.

BA = Lflat − L1 − L2
K = (BA / (π/2) − R) / T

For a 90° bend: π/2 ≈ 1.5708.

Example: Lflat = 150mm, L1 = 73mm, L2 = 73mm, R = 1.5mm, T = 2mm:

BA = 150 − 73 − 73 = 4mm
K = (4 / 1.5708 − 1.5) / 2 = (2.546 − 1.5) / 2 = 0.523

That K of 0.52 is on the high end — soft aluminum with a generous radius would produce this. For 3mm mild steel with a 1mm punch radius you might get 0.34.

Step 6: Verify with a second test.

Repeat with a different radius (1.5× and 2× material thickness are typical production radii) to confirm K stability across your expected range. If K varies significantly (>0.03) between radii for the same material, your tooling is introducing radius-dependent behavior that a single K-factor cannot capture — at that point, a bend table is the correct tool because it can map individual BA values per radius per gauge.

Step 7: Update SOLIDWORKS.

Enter the derived K-factor in the Sheet Metal feature PropertyManager for each material/gauge combination, or better: update the material library entry for the material. If you have multiple unique tooling setups, build a .btl bend table file that encodes each radius-gauge pair explicitly. For more on bend tables, see our guide to sheet metal gauge tables in SOLIDWORKS.

When to Use K-Factor vs Bend Deduction vs Bend Table

The choice is practical, not philosophical:

K-factor is best when:

  • You are modeling parts across multiple radii and gauges from one material on one machine
  • K is stable across your radius range (varies less than 0.02 between the radii you use)
  • You want SOLIDWORKS to compute bend allowance at design time based on the geometry

Bend deduction is best when:

  • Your shop already has a table of empirical BD values per tool/die setup
  • You receive BD values from tooling manufacturers or CNC press brake data sheets
  • The BD value is what gets entered into the CNC controller directly

Bend table is best when:

  • K varies enough across your radius or gauge range that a single K-factor produces unacceptable error on some bends
  • You need radius-specific BA values (precision aerospace, semiconductor parts)
  • You can afford to maintain the table file as your tooling inventory changes

A practical note: many production shops in North America program their press brake controllers with bend deduction values derived from the machine’s spring-back tables rather than K-factor. If your downstream CNC path starts from the SOLIDWORKS flat pattern DXF, the flat pattern geometry must match what the press brake will actually produce — and if the controller uses BD rather than K, your model’s K-factor should be set to produce a BA that gives the same flat blank as the BD the controller expects. They are different inputs to the same physical result.

Batch DXF Export and K-Factor Consistency

When exporting flat patterns for laser cutting or nesting, the K-factor in the model directly determines the geometry in the DXF. An incorrect K-factor produces a flat blank that, when bent, gives the wrong finished dimensions. For tight assemblies this is the difference between a part that fits and one that does not.

For teams exporting dozens or hundreds of flat patterns at once, verifying K-factor consistency across the batch is harder than verifying a single file. The approach: check the Sheet Metal feature in the FeatureManager for each part before including it in the batch, confirm it shows the correct method (K-Factor vs Bend Table vs Bend Deduction) and the expected value. Parts with unexpected bend table entries, or whose Sheet Metal feature shows a different K than the production standard, should be corrected before the export runs.

Our batch DXF export guide covers the DXF export pipeline itself. The K-factor audit step belongs before you run the batch, not after — catching a wrong K-factor in the exported DXF at the laser table is significantly more expensive than catching it in the model.

If you are still seeing wrong flat pattern dimensions after verifying K-factor, the flat pattern dimensions troubleshooting guide covers the less obvious causes: incorrect bend radius at the sketch fillet, linked vs overridden gauge values, and the K-factor rounding behavior that SOLIDWORKS applies when it translates between K-factor and bend table entries internally.