Hole-to-Bend Distance Chart

Q: Is 2.5T + R measured to the hole edge or the hole center?

This chart measures 2.5T + R to the nearest hole edge. If the drawing dimensions the hole center, add half the hole diameter: Dcenter = 2.5T + R + d/2. Other published guides may use a different origin, so read their diagram or definition before comparing values.

Q: How do I calculate hole-center distance from a bend?

First calculate the edge distance with D = 2.5T + R. Then add the hole radius, d/2. For example, with T = 2 mm, R = 2 mm, and d = 8 mm, the edge distance is 7 mm and the corresponding center distance is 11 mm under this chart’s convention.

Q: Do slots need more distance from a bend than round holes?

Often, yes. Geomiq’s general design guide recommends 4T + R for slots, compared with 2.5T + R for holes. Treat that as a starting reference because slot length, width, orientation, end radius, material, and forming process can change distortion risk.

Hole-to-Bend Distance Formula

A widely used first-pass rule for a round hole near a bend is:

D = 2.5T + R

Where:

D = distance from the flat-pattern bend reference line to the nearest edge of the round hole, using this chart’s convention
T = sheet thickness
R = planned inside bend radius after forming

For a drawing that locates the hole by its center, add half the hole diameter:

Dcenter = 2.5T + R + d/2

Where:

Dcenter = distance from the same bend reference line to the hole center
d = hole diameter

The bend reference line in this page means the bend-location line shown in the flat pattern, commonly represented as the bend centerline. Some suppliers instead measure from the tangent, the start of the inside radius, the outside mold line, or the formed outside corner. Those origins are not interchangeable. Show the measurement origin on the drawing or provide both the folded model and flat pattern for review.

The selected R should agree with the material and production tooling. Use the minimum bend radius chart as an initial material-specific reference before calculating the hole distance.

Quick Distance Multipliers

The formula can be expressed as a multiple of thickness when the inside radius is known as an R/T ratio.

Inside Radius	Calculation	Hole-Edge Distance D
R = 0.5T	2.5T + 0.5T	3.0T
R = 1.0T	2.5T + 1.0T	3.5T
R = 1.5T	2.5T + 1.5T	4.0T
R = 2.0T	2.5T + 2.0T	4.5T
R = 3.0T	2.5T + 3.0T	5.5T

This table is calculated directly from D = 2.5T + R. A larger bend radius increases the bend-line-to-hole distance under this convention, even though the clear distance from the hole edge to the bend tangent may be stated separately by another supplier.

Hole-to-Bend Distance Chart for R = T

The following chart assumes a 90-degree bend with an inside radius equal to material thickness, so D = 3.5T. It is useful for layout and early quoting, but the actual inside radius and tooling should control the released design.

Sheet Thickness T	Assumed Inside Radius R	Hole-Edge Distance D	Inch Equivalent of D
0.50 mm	0.50 mm	1.75 mm	0.069 in
0.80 mm	0.80 mm	2.80 mm	0.110 in
1.00 mm	1.00 mm	3.50 mm	0.138 in
1.20 mm	1.20 mm	4.20 mm	0.165 in
1.50 mm	1.50 mm	5.25 mm	0.207 in
2.00 mm	2.00 mm	7.00 mm	0.276 in
2.50 mm	2.50 mm	8.75 mm	0.344 in
3.00 mm	3.00 mm	10.50 mm	0.413 in
4.00 mm	4.00 mm	14.00 mm	0.551 in
5.00 mm	5.00 mm	17.50 mm	0.689 in
6.00 mm	6.00 mm	21.00 mm	0.827 in

Metric values control this calculated table. Inch equivalents are converted from millimeters using 1 in = 25.4 mm and rounded to the nearest 0.001 in; they are not additional tolerance requirements.

Worked Example

For a part with:

T = 1.5 mm
R = 2.0 mm
round-hole diameter d = 6.0 mm

The distance from the chart’s bend reference line to the nearest hole edge is:

D = 2.5(1.5) + 2.0 = 5.75 mm

If the drawing dimensions to the hole center:

Dcenter = 5.75 + 6.0/2 = 8.75 mm

For an inch drawing, 5.75 mm converts to 0.226 in and 8.75 mm converts to 0.344 in, both rounded to the nearest 0.001 in from the controlling metric calculations.

How to Use This Hole-to-Bend Distance Chart

Confirm the specified sheet thickness rather than relying only on gauge. Gauge-to-thickness relationships vary by material.
Confirm the planned inside bend radius from the material, grain direction, bend angle, tooling, and forming method.
Calculate D = 2.5T + R for a round through-hole made before bending.
Measure D to the nearest hole edge. If the drawing locates the center, add d/2.
Label the bend reference used on the drawing. If the supplier uses a tangent or outside-corner convention, reconcile the two origins before releasing the flat pattern.
Review any slot, countersink, extruded hole, louver, hardware hole, or large cutout separately because the round-hole formula may not represent its deformation risk.
Ask the fabricator to confirm the value when the hole is function-critical, carries a tight position tolerance, or sits near another bend, edge, relief, weld, or inserted fastener.

Why Hole-to-Bend Rules Differ

Published values often look contradictory because they describe different processes or measure from different locations. The following references should not be treated as numerically interchangeable without checking the original diagram or drawing convention.

Reference Context	Published Starting Guidance	Measurement or Scope Note
General sheet metal design guide	Round holes: 2.5T + R	Geomiq describes distance away from the bend; this page applies that value to its explicitly defined bend-line-to-hole-edge convention.
General sheet metal design guide	Slots: 4T + R	A slot has a longer unsupported edge and may distort more readily; orientation and slot size still require review.
Progressive-die or metal stamping guidance	2T + R for holes or slots below 0.100 in; 2.5T + R for larger features	Xometry presents these as stamping recommendations, not universal press-brake requirements.
Mild-steel job-shop press-brake experience	Keep the hole edge at least 2T from the start of the bend radius	The Fabricator article states this clear tangent-based distance for mild steel about 0.02-0.13 in thick.
Supplier-specific bend table	Material- and thickness-specific minimum-hole values	Protocase publishes values tied to its stocked materials and its outside-corner convention; supplier tables should control when that supplier is selected.

The practical lesson is to compare both the number and its definition. A hole-edge-to-tangent distance cannot be substituted directly for a hole-center-to-bend-line or outside-corner distance. Bend angle, bend allowance, setback, and the CAD system’s flat-pattern definition affect the conversion.

What Changes the Required Distance?

Material Grade, Temper, and Grain Direction

The basic 2.5T + R expression does not contain a material factor, but material still affects the result through the feasible inside radius and the amount of local strain. High-strength, work-hardened, or low-ductility material may need a larger bend radius or a different bend orientation. Aluminum alloy and temper should be identified explicitly rather than described only as “aluminum.”

Bend Radius and Forming Method

Air bending, bottoming, coining, wipe forming, and progressive-die forming do not create the same strain distribution or inside radius. Tool opening and punch geometry influence the formed radius in press-brake work. A radius assumed in CAD should be checked against the intended sheet metal bending process before the final hole position is frozen.

Hole Diameter and Feature Shape

An edge-based distance is not the same as a center-based distance. Larger holes place their centers farther from the bend when the same edge clearance is maintained. Slots and irregular cutouts can leave a longer, less-supported ligament near the bend, so one common general-design reference increases slot spacing to 4T + R.

Bend Angle and Bend Sequence

A shallow bend, a 90-degree bend, and an acute bend do not form the same geometry. A nearby return flange or second bend can also restrict tool access or change how the part is gauged. Review the entire sequence rather than checking each bend independently on a finished 3D view.

Hole-Creation Sequence

The chart addresses holes made in the flat blank before bending. A hole drilled, reamed, bored, or otherwise machined after forming avoids pre-bend ovalization, but it introduces fixture, access, datum-transfer, and cost considerations. The best sequence depends on quantity and the required relationship between the hole and formed datums.

Design Checks Before Releasing a Drawing

Specify the material grade or alloy and temper, not only the generic material family.
State the nominal thickness and confirm the actual thickness range used for bend calculations.
Define the inside bend radius, bend angle, and any grain-direction requirement.
Show whether the hole location is measured to its edge or center and identify the bend reference line.
Provide the folded 3D model and, when controlled by the buyer, the flat pattern or bend table.
Mark function-critical hole position, diameter, datums, and inspection condition after forming.
Confirm whether cutting, deburring, forming, machining, hardware insertion, welding, and finishing occur before or after the critical inspection.
Review bend-angle and bend-location variation together with hole position. The sheet metal tolerance chart explains why a formed feature may need a drawing-specific tolerance strategy.
Check nearby holes, slots, edges, bend reliefs, fasteners, embosses, countersinks, and return flanges for interaction with the bend and tooling.
Request a fabrication review when the available distance is below the selected supplier’s normal design reference.

Why Holes Distort Near a Bend

Material on the outside of a bend stretches while material toward the inside compresses. A hole that enters this highly strained region interrupts the load path and reduces the ligament supporting the feature. Depending on its location and the forming setup, the hole may become oval or teardrop-shaped, the nearby web may bulge, or the feature may shift relative to the formed flange. These effects matter even when the hole remains visually acceptable. A small shape or position change can interfere with screws, pins, bearings, self-clinching hardware, or mating panels. A tight hole tolerance also does not by itself control its final relationship to a flange; bend location, bend angle, springback, and datum selection contribute to the assembled result.

What to Do When the Hole Is Too Close to the Bend

Option	When It Helps	Trade-Off
Move the hole farther from the bend	The surrounding envelope and mating part have available space	May require a mating-part or bracket-layout change
Move the bend or lengthen the flange	The hole location is functionally fixed but the formed envelope can change	Can affect overall size, stiffness, material use, and tool access
Create the hole after forming	Final hole position relative to formed datums is critical and machining access is available	Adds setup, fixturing, cycle time, and cost
Change the feature into a reviewed relief or open-ended notch	The feature can intersect the bend region without carrying a fastener or sealing function	Removes material and may reduce strength, appearance, or edge protection
Use specialized forming or localized restraint	Production volume or part value supports dedicated development	Requires supplier-specific tooling, trials, and documented acceptance criteria
Relax or redefine the positional requirement	The current tolerance is tighter than the assembly needs	Requires engineering approval and may not solve visible distortion
Cut a pilot feature, then finish after bending	Accurate final location is needed but full post-form material removal is undesirable	Adds operations and requires reliable datum transfer

If a feature will be cut in the flat blank, laser cutting can create complex reliefs and pilot geometry without dedicated punches. It does not remove the need to verify how the remaining ligament behaves during forming.

Frequently Asked Questions

Find quick answers to common sheet metal DFM questions regarding hole-to-bend calculations, measurement conventions, and how features like slots or hardware affect your design rules.

What is the minimum hole-to-bend distance in sheet metal?

There is no single universal minimum. A common early DFM starting point for a round through-hole made before forming is D = 2.5T + R, measured under this chart’s bend-line-to-nearest-hole-edge convention. The selected fabricator’s material, tooling, process, and measurement convention should control the released drawing.

Is 2.5T + R measured to the hole edge or the hole center?

This chart measures 2.5T + R to the nearest hole edge. If the drawing dimensions the hole center, add half the hole diameter: Dcenter = 2.5T + R + d/2. Other published guides may use a different origin, so read their diagram or definition before comparing values.

How do I calculate hole-center distance from a bend?

First calculate the edge distance with D = 2.5T + R. Then add the hole radius, d/2. For example, with T = 2 mm, R = 2 mm, and d = 8 mm, the edge distance is 7 mm and the corresponding center distance is 11 mm under this chart’s convention.

Do slots need more distance from a bend than round holes?

Often, yes. Geomiq’s general design guide recommends 4T + R for slots, compared with 2.5T + R for holes. Treat that as a starting reference because slot length, width, orientation, end radius, material, and forming process can change distortion risk.

Does hole-to-bend distance change with material?

Material is not an explicit term in the basic formula, but it affects the bend radius, springback, grain-direction sensitivity, and local deformation. A design that works in annealed or ductile material should not automatically be copied to a harder alloy or temper without review.

Can a hole be placed closer if it is drilled after bending?

Potentially. Creating the hole after forming avoids distortion caused by bending a pre-existing hole, but the operation needs physical access, stable fixturing, suitable datums, and an economical production plan. Confirm whether the final hole is inspected from formed datums and whether the secondary operation can reach it consistently.

Does the same chart apply to countersinks, extruded holes, or self-clinching hardware holes?

Not automatically. Countersinks and extrusions change local thickness and stiffness, while self-clinching hardware adds manufacturer-specific hole size, panel thickness, edge distance, hardness, and installation requirements. Use the self-clinching fastener hole size chart as a starting reference and confirm the exact fastener series and installation sequence.

What should be shown on the drawing for a hole near a bend?

Show the material and thickness, inside radius, bend angle, hole diameter, hole edge or center dimension, measurement origin, functional datums, and inspection condition. If the dimension is critical after forming, identify that requirement on the formed view and provide the 3D model so the fabricator can review bend allowance, springback, tooling, and sequence together.

Need Help Reviewing a Hole Near a Bend?

ShincoFab’s engineering team can review the part geometry before production. Send the folded CAD model and drawing with material grade or temper, thickness, inside radius, bend angle and sequence, hole or slot dimensions, critical position requirements, quantity, finish, and application details through the ShincoFab contact page for a part-specific DFM review.

Capabilities

Fabrication

Value-Added

3D Printing

Material

Products

Sheet Metal Parts

Thermal & Electrical

Sheet Metal Enclosure

Energy & Infrastructure

Industries

Resource

Why Choose Us