Key takeaways
- Keep a hole at least R + V/2 + t from the bend line; for a 3 mm CRCA part on a 24 mm V die with a 3 mm radius that is 18 mm, not the 6 mm a 2t rule would allow.
- Halving the V-die opening to protect a nearby hole doubles the bending tonnage, so a full 4,450 mm bend can move from about 109 tf to 217 tf and exceed a 200 T brake.
- One degree of bend angle error moves a feature 1.75 mm at 100 mm from the bend, so a hole 8 mm from a bend will be out of position long before it looks oval.
- If the hole cannot move, pierce it after forming, add a relief slot at the bend line, or change the part to a stamped tool where the hole and form happen in one hit.
A hole 8 mm from a bend line comes back oval, and no amount of gauge adjustment fixes it. The hole was inside the zone the die deforms, so the material around it stretched before the punch reached the bottom of the stroke. The drawing said 6 mm diameter; the part measured 6.4 mm across one axis and 5.7 mm across the other, and the fastener no longer sat flat.
The rule that prevents this is not a multiple of thickness. It comes from the die opening. Hole-to-bend distance in sheet metal design is set by three numbers: the inside bend radius, the V-die opening and the material thickness. Change any of them and the safe distance changes, which is why a drawing that carries one fixed offset for every gauge will fail on at least one of them.
Hole-to-bend distance: the formula, and why it is not two times thickness
The deformation zone during air bending extends roughly half the die opening to each side of the bend line. Material inside that zone is being drawn into the radius, and any hole in it is stretched in one direction and compressed in the other.
So the minimum distance from the bend line to the near edge of the hole is:
L_min = R + V/2 + t
where R is the inside bend radius in mm, V is the V-die opening in mm, and t is the material thickness in mm. Measure from the bend line as drawn on the flat pattern, which is the centre of the bend zone, to the nearest edge of the hole, not to its centre.
The common rule of thumb that a hole should be at least 1.5t or 2t from the bend is a proxy that only works when the die opening is about 8t and the radius is about 1t. It fails on thick material with a small radius, and it fails whenever a job is set with a tighter die to form a short flange.
For a hole that must be dimensioned to its centre, add half the hole diameter:
Centre distance = R + V/2 + t + d/2
Limits by thickness
The table below assumes air bending in mild steel with a die opening of about 8t and an inside radius of 1t, which is the normal starting setup. Distances are from the bend line to the near edge of the hole.
| Thickness | V die | Inside radius | Minimum hole-to-bend | Bending force | Ganesh note |
|---|---|---|---|---|---|
| 1.0 mm | 8 mm | 1.0 mm | 6 mm | 8 tf/m | Thin gauge, distortion is local and small |
| 1.5 mm | 12 mm | 1.5 mm | 9 mm | 12 tf/m | Common for panels and covers |
| 2.0 mm | 16 mm | 2.0 mm | 12 mm | 16 tf/m | Standard enclosure gauge |
| 3.0 mm | 24 mm | 3.0 mm | 18 mm | 24 tf/m | Typical canopy and frame gauge |
| 4.0 mm | 32 mm | 4.0 mm | 24 mm | 33 tf/m | Watch flange length against the die |
| 6.0 mm | 50 mm | 6.0 mm | 37 mm | 47 tf/m | Formed on the 200 T brake |
| 8.0 mm | 64 mm | 8.0 mm | 48 mm | 65 tf/m | Full-length bends exceed 200 T; short bends only |
| 10.0 mm | 80 mm | 10.0 mm | 60 mm | 81 tf/m | Top of the brake range, short bends only |
Force is calculated as F = 1.42 × σ_b × t² / V kN per metre, using a tensile strength of 450 MPa for CRCA. That is the number that decides whether a design change is even possible: a smaller die closes the gap to the hole but costs force.
A worked example you can reproduce
Take a 3 mm CRCA bracket, 200 mm wide, with a 10 mm hole whose centre is 20 mm from the bend line. Inside radius 3 mm, die opening 24 mm.
Near edge of the hole is at 20 − 5 = 15 mm from the bend line. The limit is 3 + 12 + 3 = 18 mm. The hole is 3 mm inside the zone, and the near side of the hole will pull towards the bend and go oval.
Two fixes are available on the drawing. Move the hole to 23 mm from the bend line, giving 18 mm to the edge, or reduce the die to 16 mm V. The second option changes the limit to 3 + 8 + 3 = 14 mm and would work, but the force per metre goes from 24 tf/m to 36 tf/m, and the inside radius will no longer be 3 mm unless the punch radius is changed to match. Most of the time, moving the hole is the cheaper decision.
Now the same bracket at 1° of bend angle error. The hole is 100 mm from the bend on the flange, so the positional error is:
100 × sin(1°) = 1.75 mm
That is larger than most hole position tolerances on a bracket, and it happens before any distortion. On a 3 mm part, angular error dominates hole position long before the V-die zone does. This is why the bend allowance calculation and the flat pattern matter more than the hole itself: a hole 8 mm from a bend is a tolerance problem twice over.
Four ways to keep a hole that cannot move
Sometimes the hole has to sit close to the bend, because the mating part is fixed or the envelope is tight. There are four honest options.
Pierce after forming. Cut the blank without the hole, form it, then punch in a dedicated tool or on a press with a piercing station. This costs a second operation and a fixture, and it is the most reliable answer for a critical hole. On a repeat part the cost per piece is small; on a one-off it is not.
Add a relief slot along the bend line. A narrow slot or a pair of notches at the bend line lets the material flow without dragging the hole. It weakens the bend and shows on the outside face, so it only suits non-cosmetic parts.
Move the bend instead of the hole. Shortening the flange moves the bend line away from the hole while keeping the hole where the assembly needs it. The limit is the minimum flange length, which is set by the die: roughly V/2 + t plus clearance for the punch. A 3 mm flange on a 24 mm die is not formable at all.
Change the process to stamping. In a press tool the hole is pierced and the form is drawn in the same station, so the relationship between them is fixed by the tool rather than by the brake setup. Above a few thousand pieces a year, a progression tool often beats a laser-and-bend route for exactly this reason. The comparison of laser cutting and stamping by quantity sets out where the crossover sits.
What happens to the ligament
A hole can be far enough from the bend line and still fail, because the ligament between the hole and the bend is thin. If the ligament is under about one material thickness, the bend will bulge it and the hole will pull out of round even outside the die zone.
Keep the ligament at 1.5t where the part carries load, and never below 1t on a visible face. On stainless and aluminium the ligament needs to be thicker, because both materials work-harden and the stretch concentrates at the hole edge. A laser-cut hole has a slightly hardened recut edge that cracks more readily than a punched hole when the ligament is thin, which matters on 304 stainless canopies and on 5052 aluminium covers.
After bending: welding and assembly
Most bent brackets do not stay bent brackets. They are welded into a frame, and the hole that was carefully placed becomes a locating feature in a fixture. Two consequences follow.
First, if the hole is used as a fixture locator, it must be round within the fixture's pin clearance. A pin of 10.0 mm in a hole that has gone oval to 10.3 mm will locate loosely, and every part welded on that fixture inherits the play. Where a hole is used for location, treat it as a critical feature: specify the diameter tolerance and the roundness, and expect it to be pierced after forming.
Second, welding moves the hole again. Heat from a 4 mm fillet 20 mm away will pull the surrounding material, and a hole 30 mm from a weld seam can move 0.3–0.8 mm on cooling. That is why the assembly tolerance stack has to include forming error, bend angle error and weld shrinkage, not just the cutting tolerance.
At Ganesh, robotic MIG cells weld to fixtures and datums, not to the holes, so a hole that has drifted does not get corrected by welding. The fixture holds the part where the design says it should be, and any hole error stays where it is. That is the right behaviour for repeatability and the wrong behaviour for hiding a drawing error.
What Ganesh runs
Bending happens on a 200 T, 4,450 mm, 5-axis CNC press brake with Delem control, forming up to 10 mm. The length matters for this topic: a long part can often be formed in one setup instead of two, which removes a repositioning step where hole-to-bend relationships drift between hits. Tooling is selected per job from the die set, and the die opening is recorded so the flat pattern and the hole distances are calculated from the die that is actually used.
Cutting is on a 12 kW fibre laser with a 40 ft × 16 ft bed, so a 3,000 mm blank with its holes and bend marks comes off in one setup. Downstream, three CLOOS robotic cells and more than 30 manual MIG, spot and SPM stations weld the bent parts into assemblies, with fixtures designed and built in the in-house tool room. Parts then go through seven-tank pretreatment and powder coating where the specification calls for it, with DFT and cross-hatch checks.
Typical sheet metal tolerance is ±0.5 mm, with tighter control on critical features by agreement, and PPAP plus first article inspection are available. The bending capability page covers the machine and tool set, and the bend allowance calculator turns the radius, thickness and K-factor into a flat length so the hole can be placed correctly in the first place.
Fields for the drawing
- Material grade, thickness and actual measured thickness range.
- Inside bend radius, and whether it is fixed by the punch or "natural".
- Bend line positions on the flat pattern, with the K-factor or bend allowance assumption.
- Hole diameters and positional tolerance, with roundness where the hole locates.
- A clearance note for any hole within 40 mm of a bend line.
- Minimum flange dimension on every bend.
- Bend sequence note where a hole or a flange blocks the punch.
- Weld symbols and whether the hole is a fixture datum.
When this route is wrong
If the design needs a hole 3 mm from a bend on a 2 mm part, no press brake setup will hold it. The answer is a stamped tool, a post-form pierce, or a redesign. Sending it to a brake and hoping is how a prototype becomes a rework loop.
We do not run tube laser cutting, 3D five-axis laser trimming or in-die tapping, so a formed part that needs a hole in a position only reachable after forming is outside the route here. Parts that need a hemmed edge tighter than the die allows, or a bend radius below the material's minimum without cracking, are also better re-designed than forced. The minimum bend radius guide gives the material limits, and the minimum flange guide covers the other half of the same problem.
Get the flat pattern right and the rest of the part follows. Send the revision with the bend lines, the holes within 40 mm of a bend and the assembly datum to request a quote, and the pattern can be checked against the actual die set before the job is scheduled. More on forming tolerances sits in the bending and welding hub and in the bending tolerance and inspection guide.
Frequently asked questions
What is the minimum hole-to-bend distance for 2 mm sheet metal?
About 12 mm from the bend line on a 16 mm V die with a 2 mm inside radius, using R + V/2 + t. A 2t rule would say 4 mm, which puts the hole inside the die opening and it will ovalise on the first hit.
Does a hole near a bend always distort?
It distorts when any part of the hole falls inside the deformation zone, which spans roughly half the die opening either side of the bend line. If the hole is fully outside that zone and the ligament is thick enough, it will survive; the diameter may still change slightly from the bend's thickness reduction.
Can you laser the hole after bending?
Not on a 3D formed part on a flat-bed laser. The exceptions are a tube laser or a 5-axis machine, which we do not run for this. In practice the hole is cut before forming, punched in a dedicated tool after forming, or relocated.
How close can a hole be to a bend if I use a smaller V die?
A smaller V die shortens the deformation zone but raises the tonnage roughly in proportion to 1/V. Dropping from a 24 mm to a 12 mm V die halves the safe distance and doubles the force per metre, which often exceeds the brake capacity on a long bend.
What is the difference between hole-to-bend and edge-to-bend distance?
Edge-to-bend sets the minimum flange: you need enough material outside the bend for the punch and the back gauge to hold, typically V/2 + t. Hole-to-bend is about the hole staying round; the two limits are calculated from the same geometry but fail in different ways.
Sources
Send the flat pattern with the bend lines marked
Include the material, thickness, inside radius, the holes within 40 mm of a bend and the assembly datum. We will check the pattern against the V dies we will actually run before quoting.
Send a drawing