Busbar Bend Allowance: From K-Factor to a Verified Flat Pattern

An accurately cut blank can still produce the wrong busbar if the flat pattern was calculated from the wrong dimensions. The common mistake is mixing straight lengths measured to bend tangencies with outside flange dimensions measured to an imaginary sharp corner.

Both dimensioning methods can work. They simply require different arithmetic. Before adjusting the bender, determine whether the error comes from the developed length, the unloaded bend angle, the radius, or a misplaced hole.

A verified bend table links those calculations to a specific material and process. It is more dependable than treating one K-factor as a property of all copper.

Decide Which Dimensions the Drawing Actually Gives

On a bent part, a straight section ends where it meets the bend tangency. An outside flange dimension may instead extend to the virtual intersection of the outside faces. That virtual corner is not a physical length of material.

If the drawing supplies straight tangent lengths, the developed length is their sum plus the material length within the bend. If it supplies outside flange dimensions, a bend deduction is subtracted from their sum. Applying both adjustments to the same geometry counts the bend twice.

Confirm the thickness and inside radius as well. A tool’s nominal radius and the measured radius in the unloaded part are not automatically identical. Where the drawing controls the finished radius, the manufacturing trial must establish how it will be achieved.

The distinction between allowance and deduction is also explained in SendCutSend’s bend-calculation guide. The drawing convention should be resolved before moving dimensions between CAD, CAM, and the machine control.

Calculate One Bend With an Explicit K-Factor

K-factor represents the location of the neutral axis relative to material thickness. In the conventional model, bend allowance is:

BA = (θ × π / 180) × (R + K × t)

θ is the bend-through angle in degrees, R is the inside radius, t is thickness, and K is dimensionless. SOLIDWORKS’ K-factor documentation defines the same relationship. BA, R, and t must use compatible length units.

Take an illustrative 90° bend with t = 10 mm, R = 10 mm, and an assumed K = 0.40:

BA = (90 × π / 180) × (10 + 0.40 × 10) = 21.991 mm

If the two straight tangent lengths are 80 mm and 60 mm, the predicted blank length is:

L = 80 + 60 + 21.991 = 161.991 mm

These dimensions demonstrate the calculation. They do not establish an approved radius or K-factor for a particular copper grade. Do not issue a production blank to three decimal places merely because the calculator displays them; drawing tolerance, measurement capability, and process variation determine the meaningful precision.

Avoid Mixing Bend Allowance With Bend Deduction

For this same 90° example, the outside setback on each side is R + t, or 20 mm. The corresponding outside flange dimensions are therefore 100 mm and 80 mm.

The bend deduction is the sum of the two outside setbacks minus the bend allowance:

BD = 20 + 20 − 21.991 = 18.009 mm

Using the outside dimensions gives the same developed length:

L = 100 + 80 − 18.009 = 161.991 mm

Dimension basis	Correct calculation for this example
Straight lengths to tangencies	80 + 60 + BA
Outside lengths to the virtual corner	100 + 80 − BD
Outside lengths plus BA	Incorrect: bend-region geometry is counted again

For other bend angles, use the appropriate setback geometry and confirm the angle convention. A 135° included angle may describe a 45° change in direction. Confusing those values produces a large error that cannot be corrected by a small adjustment to K.

Calibrate the Bend Table With Coupons

Begin with material from the intended supply route. Measure the blank before bending and the finished geometry after unloading. Record grade, temper, thickness, width, rolling orientation where relevant, tooling, and machine settings.

If nominally identical lots require different force or begin cracking, do not hide the change in a new K-factor. The copper busbar temper and annealing guide explains how to specify material condition, qualify coupons and control any approved heat-treatment step before revising the bend table.

For a coupon whose straight tangent lengths and finished radius can be measured reliably, the observed allowance is the original blank length minus the straight lengths. Rearranging the model gives:

K = [BA / (θ × π / 180) − R] / t

This is a way to fit the model to the observed process, not an instruction to hide inconsistent measurements inside K. Repeat the trial and investigate variation in radius, angle, or setup before adopting the resulting value.

Keep developed-length calibration separate from springback compensation. If the unloaded angle is wrong, changing K may alter the blank length without fixing the angular error. Likewise, a correct angle does not prove that the terminal-to-terminal dimension is right.

The manufacturer’s practical Rittal busbar-bending discussion connects fabrication with digital planning. The useful production lesson is to keep planning data and the actual bend process aligned, rather than treating a CAD export as independent of tooling.

Carry Holes and Datums Through Multiple Bends

For separated bends with valid local assumptions, the developed length can be assembled from the straight segments and individual allowances. But the sequence still matters: an earlier bend can affect access, clamping, and the reference used for the next operation.

Locate terminal holes from defined datums. Distinguish a hole coordinate in the flat blank from a terminal position in the finished three-dimensional part. A hole close to a bend may also distort, so its manufacturing order and acceptance method need specific review.

When the part has several offsets, inspect the completed geometry in a fixture or coordinate system that represents its assembly task. Checking each bend angle independently may miss the accumulated error at the final terminal.

In a trial for a DHAC-BB-H workstation, include a representative multi-bend component with its actual hole pattern. The bending-machine selection guide addresses capacity and architecture; this trial establishes whether the drawing-to-part workflow is sound.

Release the Flat Pattern as a Controlled Manufacturing Record

The release package should identify the finished drawing, unfolded file, material condition, bend-table revision, tooling, bend sequence, and inspection datums. Assign one place where each compensation is applied. If CAD has already unfolded the part using a bend table, the machine should not unknowingly apply the same adjustment again.

Archive the accepted first-article measurements with the program. When material, tooling, radius, or design revision changes, review the affected bend data rather than reusing the previous file by name alone.

Make this chain part of the FAT and SAT part trial when purchasing equipment. A successful demonstration is not just a clean bend: it is a controlled drawing producing the intended finished geometry, with the calculation and setup available for the next batch.