Box / Tray / Pan Blank Calculator

The Box / Tray / Pan Blank Calculator estimates the flat rectangular blank and square corner notches for an open-top sheet metal pan with four 90-degree walls. Enter the finished outside length, width, and height, then define material thickness, inside bend radius, and K-factor. The tool returns a planning estimate for laser cutting, quoting, and an early design check; production geometry should still be verified in sheet metal CAD and against the fabricator's proven bend data.

Box / Tray / Pan Blank Calculator
01 / Parameters

Finished pan

mm
L / outside mold lines
mm
W / outside mold lines
mm
H / four equal walls
mm
T / nominal stock
mm
R / formed radius
Neutral axis ratio, 0-0.5
02 / Output

Flat blank

Live calculation
Rectangular blank size
374.3 × 274.3
mm
Corner notch (square)38.6 mm
Bend line from edge38.6 mm
Net blank area0.097 m²
Bend allowance / bend3.134 mm
Bend deduction / bend2.866 mm
Flat pattern / four square corner notches374.3 × 274.3 mm
Rectangular tray flat patternA rectangular blank with four square corner notches and dashed bend lines around the center base. BLANK LENGTHBLANK WIDTH FINISHED BASE / OUTSIDE MOLD LINESNOTCH WALL FLANGEWALL FLANGE
Planning estimate only. Add process-specific corner relief and validate against CAD or a formed coupon.
90° bend allowance
BA = (π / 2) × (R + K × T)

Neutral-axis arc length for each of the four equal bends.

Bend deduction
BD = 2 × (R + T) − BA

Deduction applied at each bend when dimensions are outside mold-line dimensions.

Blank and notch
BL = L + 2H − 2BD
BW = W + 2H − 2BD
N = H − BD / 2

The same centered deduction establishes the square notch and bend-line offset.

The net area subtracts four square corner notches from the rectangular blank. It does not include bend relief extensions, hems, corner seams, tabs, welding gaps, or kerf compensation.

How to Use the Calculator

1. Select MM or IN

Choose millimeters or inches with the unit switch. Changing units converts every dimensional value already entered. K-factor is dimensionless and does not change.

2. Enter the outside length

Enter the finished pan length, measured between the two opposing outside mold lines at the base-to-wall bends. Do not enter a developed flat length or an inside cavity dimension.

3. Enter the outside width

Enter the finished width between the other pair of outside mold lines. The tool assumes a rectangular base with length and width at right angles.

4. Enter the outside height

Enter the finished outside wall height. One value is applied to all four sides. A pan with unequal wall heights, sloped walls, hems, or stepped flanges requires a separate flat-pattern model.

5. Enter material thickness

Use nominal sheet thickness, not a gauge number. If the drawing specifies gauge, confirm its actual thickness for the material family with the sheet metal gauge thickness chart before calculating.

6. Enter the inside bend radius

Use the expected formed inside radius. This is a geometry input, not automatically equal to material thickness or punch nose radius. Check feasibility against the minimum bend radius chart and the selected tooling.

7. Enter the K-factor

K-factor describes the neutral-axis location as a fraction of material thickness measured from the inside bend surface. Enter a value from 0 to 0.50. Use a value proven for the actual alloy, temper, thickness, bend method, radius, and tooling whenever available.

8. Review, copy, or reset

Results update as inputs change. Copy results captures the input assumptions and all primary outputs; Copy blank size captures the rectangular blank size. Reset values restores the documented example in the active unit system.

What Each Result Means

Rectangular blank size

This is the overall length by width of the starting rectangle before the four corners are removed. It is calculated from the finished outside base dimensions, two wall heights in each direction, and two bend deductions in each direction.

Corner notch (square)

This is the estimated side length of each of four square corner cutouts. It equals the bend-line offset under the calculator’s centered-deduction convention. It does not add a bend-relief slot, corner gap, weld allowance, overlap tab, or seam treatment.

Bend line from edge

This is the distance from each outside blank edge to its parallel 90-degree bend line. The four bend lines outline the finished base area in the flat pattern.

Net blank area

Net blank area is the rectangular blank area minus the four square corner notches. In metric mode it is shown in square metres; in imperial mode it is shown in square inches. It is useful for rough material comparison but is not a nesting or purchasing quantity.

Bend allowance / bend

Bend allowance (BA) is the neutral-axis arc length consumed by one 90-degree bend. The calculator applies the same BA to all four bends.

Bend deduction / bend

Bend deduction (BD) is the amount subtracted from the sum of two outside flange dimensions to obtain their developed flat length. Here it is derived from the outside setback and BA for one 90-degree bend.

Formula and Engineering Assumptions

The calculator uses radians in the bend allowance equation. For a 90-degree bend, the bend angle is π / 2 radians.

BA = (π / 2) × (R + K × T)

BD = 2 × (R + T) − BA

Blank length, BL = L + 2H − 2BD
Blank width,  BW = W + 2H − 2BD

Corner notch, N = H − BD / 2
Bend-line offset = N

Net blank area = BL × BW − 4N²

Where:

  • L = finished outside length
  • W = finished outside width
  • H = finished outside wall height
  • T = material thickness
  • R = formed inside bend radius
  • K = K-factor
  • BA = bend allowance for one 90-degree bend
  • BD = bend deduction for one 90-degree bend

The notch equation splits each bend deduction equally between the two adjoining outside flange dimensions. That convention provides a useful symmetric layout for an early estimate, but it is not a universal corner-detail standard. For more background, compare the entered values with ShincoFab’s bend allowance and bend deduction chart.

Worked example

For a pan with L = 300 mm, W = 200 mm, H = 40 mm, T = 1.5 mm, R = 1.5 mm, and K = 0.33:

BA = 3.134 mm per bend
BD = 2.866 mm per bend
Blank length = 374.3 mm
Blank width = 274.3 mm
Square corner notch = 38.6 mm
Net blank area = 0.0967 m²

Small displayed differences can occur because the calculator retains full internal precision and rounds only the visible result.

Design and Fabrication Checklist

  • Confirm whether the drawing dimensions are outside, inside, or to bend tangency; this calculator requires outside mold-line dimensions.
  • Verify actual sheet thickness, alloy, temper, grain direction, and any protective film before final nesting.
  • Match K-factor and formed inside radius to the intended press-brake process and tooling rather than relying on a generic material label.
  • Add a suitable corner gap, bend relief, weld preparation, overlap, tab, or seam detail for the intended assembly method.
  • Check that wall height meets tooling access and minimum flange requirements using the minimum flange length chart.
  • Keep holes, slots, and formed features far enough from bend zones to avoid distortion.
  • Account for deburring, corner finishing, coating buildup, and dimensional inspection datums.
  • Run a CAD flat pattern and form a coupon or first article before releasing repeated production.

Why Results May Differ

CAD bend tables use different calibration data

CAD systems may use bend allowance, bend deduction, K-factor, Y-factor, or a shop-specific bend table. A calibrated table can produce a different flat pattern even when the nominal radius and thickness match.

The real inside radius may differ from the input

Air bending, bottoming, and coining do not create the same radius. Die opening, punch geometry, material strength, and press setup all affect the formed result.

Material behavior changes by lot and orientation

Thickness tolerance, alloy, temper, rolling direction, and work hardening can move the neutral axis and change springback. K-factor should therefore be treated as process data, not a universal material constant.

Corner details consume or remove additional material

Real trays often need relief slots, weld gaps, corner overlaps, tabs, radiused notches, hems, or sealed seams. These details change the cut contour even when the overall rectangle and bend lines remain similar.

Production dimensions may use another datum

Inside cavity size, outside envelope, tangent dimensions, and virtual-sharp dimensions are not interchangeable. See the sheet metal tolerance chart and define drawing datums before comparing a formed part with the estimate.

Frequently Asked Questions

These answers address the most common differences between an early blank estimate, a CAD flat pattern, and a formed production tray. They also clarify when the simple four-bend model is appropriate and when a drawing-specific review is necessary.

Is this calculator for sheet metal or cardboard boxes?

It is for a simple open-top sheet metal box, tray, or pan formed with four 90-degree bends. Packaging dielines use board caliper, scores, glue flaps, tuck panels, and style-specific allowances, so they require a different method.

Enter finished outside length, width, and wall height measured to the outside mold lines. If your specification is based on inside usable space, first create or review the formed cross-section so radius and thickness are handled correctly.

The flat flange that produces an outside wall height is reduced by half of the bend deduction under the centered-deduction convention. The result is the calculated bend-line offset and square notch size.

No. The output is a theoretical square corner removal. Bend relief shape and size depend on thickness, radius, tooling, corner closure, welding plan, coating, and appearance requirements.

Use a value established from the actual material and bend process. A supplier table or previous production record is a better starting point than a generic material preset; a measured test coupon is preferable when the final dimensions are important.

Use it as a planning estimate or independent check, not as unattended production geometry. Add the required relief and seam features, verify the flat pattern in CAD, and confirm the bend data with the fabricator before issuing the cut file.

No. It assumes four equal-height vertical walls, a rectangular base, identical bend parameters, and no hems or secondary bends. Unequal, tapered, lidded, nested, or multi-flange parts require a dedicated model.

Need a Production-Ready Tray Blank?

A drawing-specific design for manufacturability (DFM) review can reconcile your dimensional datums, material specification, corner closure, tooling, bend data, welding, finish, and inspection requirements. Include a dimensioned drawing or 3D model, material and thickness, quantity, finish, critical dimensions, and the intended corner construction.

Whatsapp

+86 13392819510

Address

Building 1, No.8, Second Street, Huangjiang Town,
Dongguan City, Guangdong Province

Socials

Facebook Youtube
Please enable JavaScript in your browser to complete this form.
Click or drag files to this area to upload. You can upload up to 3 files.

ShincoFab specializes in precision sheet metal fabrication, delivering high-quality custom metal solutions to clients worldwide with advanced technology and expert craftsmanship.

Contact Info

  • Building 1, No.8, Second Street, Huangjiang Town, Dongguan City, Guangdong Province
  • Whatsapp: +86 13392819510
  • [email protected]

Support

Get In Touch

Ready to start your sheet metal project? Contact the ShincoFab team to discuss your custom fabrication requirements. We support you through design, manufacturing, and delivery—at every stage.

Facebook-f Youtube
Scroll to Top